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Knowledge Advisor
Table Of Contents
Overview ...................................................................................................... 1 Knowledge Advisor in a Nutshell .................................................................... 1 Before Reading this Guide ............................................................................ 2 Getting the Most out of this Guide ................................................................. 2 Accessing sample documents ........................................................................ 2 Conventions Used in this Guide ..................................................................... 2 What's New? ................................................................................................. 3 New Functionalities...................................................................................... 3 Getting Started.............................................................................................. 5 Using Parameters ........................................................................................ 5 Using Formulas ........................................................................................... 6 Using Rules ................................................................................................ 8 Using Checks .............................................................................................10 User Tasks ...................................................................................................13 User Tasks ................................................................................................13 Working with Parameters ............................................................................13 Working with Parameters..........................................................................13 Introducing Parameters ............................................................................13 Creating a Parameter ...............................................................................14 Copy/Pasting Parameters..........................................................................15 Specifying the Material Parameter ..............................................................16 Valuating the Mechanical Property Parameters .............................................17 Specifying a Parameter Value as a Measure .................................................17
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knowledgewareAdvisor Importing Parameters ..............................................................................20 Creating Points, Lines... as Parameters .......................................................21 Applying Ranges to Parameters by Using a Rule ...........................................22 Creating an Associative Link Between Measures and Parameters ....................24 Publishing Parameters ..............................................................................29 Activating and Deactivating a Component ...................................................34 Creating an External Parameter .................................................................39 Deactivating and Re-activating External Parameters .....................................40 Getting Familiar with the Parameters Explorer .............................................41 Adding a Parameter to a Feature ...............................................................43 Adding a Parameter to an Edge .................................................................45 Locking and Unlocking a Parameter ............................................................47 Creating Sets of Parameters......................................................................49 Working with Formulas................................................................................50 Working with Formulas .............................................................................50 Introducing Formulas ...............................................................................50 Getting Familiar With the f(x) Dialog Box ....................................................51 Using the Dictionary.................................................................................54 Creating a Formula ..................................................................................62 Creating Formulas based on Publications.....................................................63 Specifying a Measure in a Formula .............................................................66 Using Geometry to Create a Formula ..........................................................68 Refering to External Parameters in a Formula ..............................................69 Using the Equivalent Dimensions Feature ....................................................72 Associating URLs and Comments with Parameters or Relations..........................74
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Table Of Contents Associating URLs & Comments with Features ...............................................74 Assigning a Comment to a Knowledge Feature .............................................74 Working with Design Tables .........................................................................76 Working with Design Tables ......................................................................76 Introducing Design Tables.........................................................................77 Getting Familiar with the Design Table Dialog Box ........................................81 Creating a Design Table from the Current Parameters Values .........................86 Creating a Design Table from a Pre-existing File...........................................88 Interactively Adding a Row To a Design Table External File ............................90 Controlling Design Tables Synchronization...................................................93 Storing a Design Table in a Power Copy ......................................................96 Creating and Using a Knowledge Advisor Law .................................................98 Using the Knowledge Inspector .................................................................. 102 The 'What If' Mode................................................................................. 103 The 'How To' Mode ................................................................................ 105 Working with the Rule Feature ................................................................... 107 Working with the Rule Feature................................................................. 107 Creating a Rule ..................................................................................... 108 Using Rules and Checks in a Power Copy................................................... 110 Using the Rule Editor ............................................................................. 111 Handling Errors ..................................................................................... 112 Working with the Check Feature ................................................................. 114 Working with the Check Feature .............................................................. 114 Creating a Check ................................................................................... 114 Performing a Global Analysis of Checks..................................................... 116
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knowledgewareAdvisor Using the Check Editor ........................................................................... 126 Using the Action Feature......................................................................... 127 Working with the Reaction Feature.............................................................. 130 Working with the Reaction Feature ........................................................... 130 Using the Reaction Feature Window.......................................................... 131 Creating a Reaction Event....................................................................... 134 Creating a Loop in a Reaction .................................................................. 156 Launching a VB Macro with Arguments ........................................................ 159 Working with Relations.............................................................................. 161 Working with Relations ........................................................................... 161 Creating Sets of Relations ....................................................................... 161 Using Relations based on Publications at the Product Level .......................... 162 Activating and Deactivating a Component ................................................. 166 Instantiating Relations from a Catalog ...................................................... 171 Updating Relations Using Measures .......................................................... 172 Controlling Relations Update ................................................................... 173 Working with the List Feature..................................................................... 177 Working with the List Feature ................................................................. 177 Using the List Edition Window.................................................................. 178 Creating a List....................................................................................... 180 Working with the Loop Feature ................................................................... 183 Working with the Loop Feature ................................................................ 184 Introducing the Loop Feature .................................................................. 184 Getting Familiar with the Loop Edition Window and Menus ........................... 184 Creating a Loop..................................................................................... 188
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Table Of Contents Creating a Power Copy Containing a Loop ................................................. 191 Using the Scripting Language .................................................................. 196 Declaring Input Data.............................................................................. 208 Defining the Context .............................................................................. 209 Solving a Set of Equations ......................................................................... 210 Solving a Set of Equations ...................................................................... 210 Using the Equations Editor ...................................................................... 211 Using the Knowledge Advisor Language ....................................................... 213 Using the Knowledge Advisor Language .................................................... 213 Attributes ............................................................................................. 220 Object Methods ..................................................................................... 220 Messages and macros ............................................................................ 227 Limitations .............................................................................................. 231 Parameters and Formulas ....................................................................... 231 Design Tables ....................................................................................... 231 Rules ................................................................................................... 231 Sets of Equations .................................................................................. 231 Macros with Arguments .......................................................................... 231 Loops .................................................................................................. 231 Useful Tips .............................................................................................. 232 Relations .............................................................................................. 232 Rules ................................................................................................... 233 Parameters ........................................................................................... 234 Formulas .............................................................................................. 235 Design Tables ....................................................................................... 235
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knowledgewareAdvisor Loops .................................................................................................. 236 Reactions ............................................................................................. 238 Use Cases ............................................................................................... 238 Use Cases ............................................................................................ 238 The Ball Bearing .................................................................................... 238 System of Three Equations in Three Variables............................................ 245 Reference .................................................................................................. 247 Reference ............................................................................................... 247 Basic Wireframe Package........................................................................... 247 GSMPoint ............................................................................................. 247 GSMLine............................................................................................... 252 GSMPlane............................................................................................. 256 GSMCircle............................................................................................. 262 Part Design Package ................................................................................. 265 Box ..................................................................................................... 265 Chamfer............................................................................................... 266 Cone.................................................................................................... 267 Counterbored Hole................................................................................. 268 Counterdrilled Hole ................................................................................ 268 Countersunk Hole .................................................................................. 269 Cylinder ............................................................................................... 270 Hole .................................................................................................... 270 Pad ..................................................................................................... 271 Shaft ................................................................................................... 272 Shell.................................................................................................... 273
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Table Of Contents SimpleHole ........................................................................................... 275 Sphere................................................................................................. 275 Tapered Hole ........................................................................................ 276 Thickness ............................................................................................. 276 ThickSurface ......................................................................................... 277 Torus ................................................................................................... 279 Part Shared Package................................................................................. 279 Fillet Object .......................................................................................... 279 Constant Edge Fillet Object ..................................................................... 280 Pattern ................................................................................................ 281 Standard Package .................................................................................... 283 GSD Shared Package ................................................................................ 283 GSD Package ........................................................................................... 283 GSMAssemble ....................................................................................... 284 GSMCurve ............................................................................................ 284 GSMCurvePar........................................................................................ 285 GSMExtrude.......................................................................................... 286 GSMFillet.............................................................................................. 287 GSMProject........................................................................................... 287 GSMSplit .............................................................................................. 288 GSMSweepSegment ............................................................................... 289 Knowledge Expert Package ........................................................................ 289 KWECheck ............................................................................................ 290 KWERule .............................................................................................. 290 KWERuleBase........................................................................................ 291
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knowledgewareAdvisor KWERuleSet.......................................................................................... 291 Mechanical Modeler Package ...................................................................... 292 BodyFeature ......................................................................................... 292 Workbench Description ................................................................................ 293 Workbench Description ............................................................................. 293 Toolbars ................................................................................................. 294 Knowledge Toolbar ................................................................................ 294 Reactive Features Toolbar....................................................................... 294 Organize Knowledge Toolbar ................................................................... 294 Control Features Toolbar ........................................................................ 295 Actions Toolbar ..................................................................................... 295 Tools Toolbar ........................................................................................ 295 Set of Equations Toolbar......................................................................... 296 Project Standards ....................................................................................... 297 Customizing for Knowledge Advisor............................................................. 297 Customizing.......................................................................................... 297 Knowledge............................................................................................ 297 Language ............................................................................................. 301 Report Generation ................................................................................. 302 Part Infrastructure for Knowledgeware Applications .................................... 305
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Overview
This book is intended for the user who needs to become quickly familiar with Knowledge Advisor. This overview provides the following information: • • • • • Knowledge Advisor in a Nutshell Before Reading this Guide Getting the Most out of this Guide Accessing sample documents Conventions Used in this Guide
Knowledge Advisor in a Nutshell
CATIA - KNOWLEDGE ADVISOR is a CATIA product which allows users to embed knowledge within design and leverage it to assist in engineering decisions, in order to reduce errors or automate design, for maximum productivity. Users can embed knowledge in design such as formulas, rules and checks and leverage it when required at any time. Knowledge is then taken into account and acts according to its definition. Its meaning is also accessible: For example a check intent can highlight the parameters involved in a verification, it is easy and immediate to understand in what way a standard has been violated. In short, Knowledge Advisor enables users to: • Capture corporate engineering knowledge as embedded specifications allowing complete consistency. • • • • • • • • Easily define and share know-how among all users. Automate product definition. Ensure compliance with corporate standard. Increase productivity. Increase Knowledge management for sharing and understanding intents. Build Knowledge components management for customization and reuse. Allow early attention to final design specifications preventing costly redesigns. Guide and assist users through their design tasks.
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Before Reading this Guide
Before reading this guide, you should be familiar with basic Version 5 concepts such as document windows, standard and view toolbars. Therefore, we recommend that you read the Infrastructure User's Guide that describes generic capabilities common to all Version 5 products. It also describes the general layout of V5 and the interoperability between workbenches.
Getting the Most out of this Guide
To get the most of this guide, we suggest that you start performing the step-by-step Getting Started tutorial. Once you have finished, you should move on to the User Tasks section. The Workbench Description section, which describes the Knowledge Advisor workbench, and the Customizing section, which explains how to set up the options, will also certainly prove useful.
Accessing sample documents
To perform the scenarios, you will be using sample documents contained in either the online/kwrug/samples folder. For more information about this, please refer to Accessing Sample Documents in the Infrastructure User's Guide.
Conventions Used in this Guide
To learn more about the conventions used in this guide, refer to the Conventions section.
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What's New?
New Functionalities
Deactivating and Re-activating External Parameters Users can now re-activate and synchronize external parameters previously deactivated.
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Getting Started
Using Parameters
This task explains how to use parameters. For a fuller outline of the parameters-related tasks, see Knowledgeware Infrastructure - Tips and Techniques - Summary dedicated to the knowledgeware infrastructure capabilities. Check the settings below: • From the Tools menu, select Options->General>Parameters and Measure.
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In the Knowledge tab, check the With Value and Wi Formula check boxes, and click OK.
When working in a Japanese environment, check the Surrounded by the symbol' check box under Parameter names. • From the Tools menu, select Tools->Options...>Infrastructure->Part Infrastructure. Check at least the Relations and Parameters boxes the Display tab, and click OK. It is recommended to check all the options located below the Specification tree settings.
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1. Open the KwrStartDocument.CATPart document. If you expand the Parameters node in the specification tree, the Material parameter is the only one displayed. At this stage of the scenario, don't pay any attention to this default parameter.
The Relations node can't be expanded as there is no default relation in a CATIA document.
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2. Click the
icon. The Formulas dialog box is displayed.
3. In the New Parameter of type scrolling list, select the Length type, then click the New Parameter type button.
4. In the Edit name or value of the current parameter field, replace the Length.1 string with PadLen and click Apply. A new parameter is added to the document parameter list both in the Formulas dialog box and in the specification tree. You have just created a user parameter. 5. Click OK in the Formulas dialog box to terminate the dialog. Keep your document open and proceed to next task.
Using Formulas
This task explains how a parameter can be constrained by a formula. See the Knowledgeware Infrastructure - Tips and Techniques - Summary dedicated to the infrastructure knowledgeware capabilities for more information on formulas.
1. Click the
icon. The Formulas dialog box is displayed.
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Getting Started
2. In the parameter list, select the PartBody Sketch.1 Radius.1 item, then click Add Formula. The Formula editor is displayed.
Radius
The icon located on the right is simply a rubber you can use to erase the formula. 3. Enter the 2 * PartBody Hole.1 Diameter relation.
4. Click OK in the Formula Editor once you have typed your relation. The Formula.1 relation is added to the specification tree. In the parameter list of the dialog box, a formula is now associated with the sketch radius. 5. In the parameter list, select the PadLength item, click Add Formula to create the formula below: PadLength = PartBody PartBody Pad.1 Pad.1 SecondLimit FirstLimit Length Length +
In the parameter list, the Formula.2 relation is now associated with the PadLength user parameter. In the specification tree, PadLength is also displayed with the value resulting from Formula.2. 6. Click OK twice in the Formulas dialog box to terminate this task. Keep your document open and proceed to the next task. This is now what you should see in the specification tree under "Relations":
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Using Rules
This task introduces the Knowledge Advisor rules. Unlike the parameter and formula capabilities which are available to all CATIA users, the rule and check capabilities require the Knowledge Advisor product. For more information about Rules, see Working with the Rule Feature. To know more about the Rule Editor, see Using the Rule Editor. 1. Select the KwrStartDocument item in the specification tree 2. Access the Knowledge Advisor workbench from the Start>Knowledgeware menu. 3. Click the rule icon. The following dialog box is displayed:
4. The dialog box fields display default values that can be modified: 5. a - The rule name: Rule.1. The first rule created in a document is Rule.1 by default. This name is the one displayed in the specification tree unless you modify the default name at creation. 6. b - The user and the date of creation. 7. c - The destination, i.e. the feature you are going to add the rule to. By default, in this scenario, the destination is the Relations feature (the Relations node in the specification tree). But a rule could be added to another feature, then only apply to this feature. 8. Replace the Rule.1 string with Cylinder_Rule, if need be modify the comments but don't modify the destination. Click OK. The Rule Editor is displayed (see below).
9. Type the code below into the edition box or copy/paste it from your browser to
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the edition box. PartBody Hole.1 Activity = true if PadLength <= 50mm and PadLength > 20mm { PartBody Hole.1 Diameter = 20mm Message("PadLength is: # | Internal Diameter is: #", PadLength,PartBody Hole.1 Diameter) } else if PadLength > 50mm and PadLength < 100mm { PartBody Hole.1 Diameter = 50mm Message("PadLength is: # | Internal Diameter is: #", PadLength,PartBody Hole.1 } else if PadLength >= 100mm { Diameter)
PartBody Hole.1 Diameter = 80mm Message("PadLength is: # | Internal Diameter is: #", PadLength,PartBody } else { Hole.1 Diameter)
PartBody Hole.1 Activity = false Message("PadLength is: # | Internal Diameter is: #", PadLength,PartBody } Hole.1 Diameter)
10. Users working in a Japanese environment should use the script below: `PartBody Hole.1 Activity` = true if `PadLength` <= 50mm and `PadLength` > 20mm { `PartBody Hole.1 Diameter` = 20mm Message("PadLength is: # | Internal Diameter is: #", `PadLength`,`PartBody Hole.1 Diameter`) } else if `PadLength` > 50mm and `PadLength` < 100mm { `PartBody Hole.1 Diameter` = 50mm Message("PadLength is: # | Internal Diameter is: #", `PadLength`,`PartBody } Hole.1 Diameter`)
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else if `PadLength` >= 100mm { `PartBody Hole.1 Diameter` = 80mm Message("PadLength is: # | Internal Diameter is: #", `PadLength`,`PartBody } else { Hole.1 Diameter`)
`PartBody Hole.1 Activity` = false Message("PadLength is: # | Internal Diameter is: #", `PadLength`,`PartBody } Hole.1 Diameter`)
11. Click Apply. An information window displays the PadLength and Pad internal diameter values. Click OK in the Information window. The Cylinder_Rule relation is added to the specification tree. 12. Click OK to terminate this part of the dialog. Keep your document open and proceed to the next task.
Using Checks
This task explains how to create a check and what happens when you add a check to a document. The Knowledge Advisor product is required for this task. See the Rule and Check Tasks for more information on check-related tasks.
1. Click the
icon. The first "Check Editor" dialog box is displayed.
2. Replace the Check.1 default name with Cylinder_Check, then click OK. The Check Editor box is displayed. It is similar to the Rule Editor. The Incremental box must be unckecked.
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3. Select the Information item in the Type of Check list. 4. Enter a string in the message field (for example: Pad too short). This message is to be displayed whenever the statement specified by the check is not fulfilled. 5. Enter the following statement into the edition box: PadLength > 20mm 6. Click OK to confirm the check creation. The Cylinder_Check relation is added to the specification tree. A green icon in the specification tree means that the check is fulfilled. No message is displayed. 7. Change the Pad limits so that PadLength <= 20mm. The Cylinder_Rule relation is re-applied. An information window displays the new PadLength and Pad internal diameter values. Then, you are warned by another window ("Pad too short") that the check is no longer valid. The check icon in the specification tree turns to red.
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User Tasks
User Tasks
Refer to the Quick Reference of Tasks for a comprehensive list of interactions to be carried out on rules and checks. See also the Useful Tips, the Limitations, and the CATIA Knowledgeware Infrastructure sections. This section shows you how to manage the Knowledge Advisor relations.
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Working with Parameters
Working with Parameters
Select the Formula icon to create parameters. Select the Add Set of Parameters icon to create sets of parameters. These sets of parameters are all grouped below the Parameters node. Select the Parameters Explorer icon to add new parameters to a feature. Select the Add parameters on geometry icon to add new parameters to a face, a vertex, or an edge.
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Introducing Parameters
When you create a part like the hollow cylinder of our "Getting Started" example, you often start by creating a sketch, then you create a pad by extruding the initial sketch, then you add other features to the created pad. The final document is made up of features which define the intrinsic properties of the document. Removing one of these features results in a modification of the document. These features are called parameters. Parameters play a prominent role in Knowledgeware applications. They are features that can be constrained by relations and they can also be used as the arguments of a relation. In addition to these parameters, CATIA allows you to create user parameters. These user parameters are extra pieces of information added to a document. User parameters are very handy in knowledgeware applications:
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knowledgewareAdvisor • • • They can be used to add specific information to a document They can be defined or constrained by relations They can be used as the arguments of a relation.
Parameters are created clicking one of the following icons: The parameters are created using the Formulas Editor. To find out more about this editor, see Getting Familiar With the f(x) Dialog Box. The parameters are created using the Parameters Explorer Editor. To find out more about this editor, see Getting Familiar with the Parameters Explorer. The created parameters only apply to edges, faces and vertex. The editor is similar to the Parameters Explorer editor. The Set of Parameters enables you to gather user parameters below a set.
A given relation may take as its arguments both types of parameters (intrinsic and user). For the parameters to display in the specification tree, check the settings below: • From the Tools menu, select Options>General->Parameters and Measure. In the Knowledge tab, check the With Value and With Formula check boxes, and click OK if you want the parameters to display their values and associated formulas (if any.) When working in a Japanese environment, check the Surrounded by the symbol' check box under Parameter names. • From the Tools menu, select Tools->Options...>Infrastructure->Part Infrastructure Check at least the Relations and Parameters boxes in the Display tab, and click OK.
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Creating a Parameter
This task explains how to create a Time type parameter and assign a value to it.
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1. Open the KwrStartDocument.CATPart document. 2. Click the icon. The f(x) dialog box is displayed.
3. Select the Time item with Single Value in the New Parameter of type list, then click New Parameter of type. The new parameter appears in the Edit name or value of the current parameter field. 4. Replace the Time.1 name with Machining_Time and assign the 1000s value to this parameter. Then click Apply. The Machining_Time parameter is added to the specification tree. The dialog box is modified as follows:
5. 6. Click OK when done to close the dialog box. • You can add properties to a .CATPart or a .CATProduct document by using the Properties command from the contextual menu. You just have to click the Define other properties... button in the Product tab then click New parameter of type. The dialog is similar to the f(x) dialog. See the Product Structure User's Guide for more information. The properties you define that way are also displayed in the parameter list of the f(x) dialog box. You can specify that a parameter is constant by using the Properties command from the contextual menu. This command also enables you to hide a parameter.
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Copy/Pasting Parameters
The Tools->Options->General->Parameters and Measure check boxes allow you to: • Paste a parameter without the formula which defines it. For example:
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knowledgewareAdvisor Holeplus= 15 = Diameter + 10 will be pasted as Real.i = 15 (if the With Value box is checked)
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Paste a parameter as well as the formula which defines it, but only if the parameters referred to in the formula are also selected in the copy. For example: Holeplus= 15 = Diameter + 10 will be pasted as Real.i = 15 if the Diameter parameter does not belong to the items selected for the copy but HolePlus will be pasted as Real.i = 15 = Real.j + 10 if Diameter is selected in the copy (use multi-selection).
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Paste a parameter as well as the formula. Holeplus= 15 = Diameter + 10 will be pasted as Real.i = Diameter + 10 When copying parameters sets containing hidden parameters, these parameters are automatically pasted when pasting the parameters sets and appear as hidden parameters.
Specifying the Material Parameter
Whatever your document, the Material parameter is always displayed in the specification tree. The Material parameter is created only after a material is applied to a Part or a Product. The Mechanical_Property features are calculated from the Material value. Specify a material to set the values of the Mechanical_Property features. 1. Open the KwrStartDocument.CATPart document. The Material parameter is displayed by default in the specification tree. Its value is set to None. 2. Double-click the Material feature in the specification tree to edit the parameter. The dialog box below is displayed.
3. Click OK and select the root feature in the specification tree. icon in the standard toolbar to display the available material 4. Click the library. Select the Metal->Iron material. 5. Click Apply Material and OK.
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This is what you should see now in the specification tree. The Iron feature is added to the specification tree and a new material is added under the Parameters node.
6. Remember: To display parameter values, check Tools->Options>General->Knowledge->Parameters and Measure->With value. 7. Keep your document open and proceed to the next task.
Valuating the Mechanical Property Parameters
Once the Material value has been specified, the Mechanical_Property parameters are automatically updated when the Properties option is selected in the contextual menu. 1. Select the root item in the specification tree and open the Properties dialog box from the contextual menu. 2. Select the Mass tab. The document mechanical properties have been updated from the value assigned to the Material parameter. 3. Click OK to go back to your document.
Specifying a Parameter Value as a Measure
This scenario shows how to assign a value to a parameter deducing it from a graphic selection. In this scenario, you deduce the value assigned to the Thickness parameter by selecting 2 circular edges. A common way to assign a value to a parameter is to use the Edit name or value of the current parameter field of the Formulas dialog box. But there is another way to proceed. The value you assign to a parameter can be deduced from a graphic selection. 1. In Tools->Options->General->Parameters and Measure, check the Load extended language libraries box of the Language tab. 2. Open the KwrStartDocument.CATPart document. 3. Click the icon. The f(x) dialog box is displayed.
4. Select the Length item with Single Value in the New Parameter of type list, then click New Parameter of type. The new parameter appears in Edit name or value of the current parameter. 5. Replace the Length.1 name with Thickness, then right-click in the value field of Edit
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name or value of the current parameter.
6. 7. Select the Measure Between... command from the contextual menu. The Measure Between dialog box is displayed. Select Edge only as Selection 1 mode and Edge only as Selection 2 mode. 8. In the document geometry area, select successively one of the inner circular edge of the part, then the outer circular edge located on the same face. The 17.5 mm value is displayed in the Measure Between dialog box.
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8. Click OK when done in the Measure Between dialog box. The 17.5 mm value is displayed in the Formulas dialog box. 9. Click OK to close the Formulas dialog box. The parameter is displayed below the Measure node in the specification tree and below the Parameters node. To edit this parameter: • • • Double-click it in the specification tree. The Edit Parameters dialog box is displayed. icon located next to the value field. The Click the Measure between dialog box is displayed. Edit the parameter and click OK when done.
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Importing Parameters
This scenario shows how to import parameters from an excel or a .txt file into a CATPart document. • Parameters and parameter values can be imported from a text file or from an Excel file (Windows) into documents (CATPart, CATProduct, Drawings...). If imported parameters already exist in the document, the import process automatically updates the document. Note that if 2 parameters have the same name in the import file, no clone is created and the parameters are not renamed. Make sure that the parameters have different names before importing them. Identical parameters names are not supported.
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Please find below the formatting rules the external file should comply with: • Column 1 Parameter names Column 2 Parameter values. Multiple values are allowed. Values should then be separated by a ";". The imported value is the one delimited by the "<" and ">" tags. Use the Tab key to skip from one column to the other in a tabulated text file. Column 3 Formula. If no formula is specified, the third column should be left empty. In a tabulated text file, just press the Tab key twice from column 2 to leave column 3 empty. Column 4 Optional comment.
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1. Open the KwrStartDocument.CATPart document. 2. Click the icon. The f(x) dialog box is displayed.
3. Click Import.... A file selection dialog box is displayed. 4. Select the ExCompanyFile0.xls file (Windows only) or the TxCompanyFile0.txt file, then click Open. The list of parameters to be imported into the KwrStartDocument.CATPart document is displayed.
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5. Click OK to import the parameters from the input file into the KwrStartDocument.CATPart document. The imported parameters are now displayed in the parameter list of the f(x) dialog box and in the specification tree.
6. Click OK to terminate the dialog.
Creating Points, Lines... as Parameters
The scenario below explains how to determine the position of the inertia axis of a pad. To do so, start from a pad, then: ) 1. Create a line by using either method ('datum' or 2. Use the inertiaAxis line constructor to specify that this line is to be the inertia axis of the pad. 3. Retrieve the coordinate of the point located at the intersection of the inertia axis and the pad extrusion plane.
To create elements such as Points, Lines, Curves, Surfaces, Planes or Circles and use them in knowledgeware relations, you can: • Create these elements as 'Isolate' elements in the Generative Shape Design workbench. 'Isolate' elements also called Datum are elements that have no link to the other entities that were used to create them. For information on 'Datum' type elements, see the Generative Shape Design User's Guide. Create these elements by using the f(x) capabilities and select the right type of element in the New parameter of type list.
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1. Access the Part Design workbench, create any sketch in the yz plane, then extrude this sketch to create a pad. If need be, refer to the Part Design User's Guide. 2. Create a line intended to be used as an inertia axis afterwards. 3. To do so, click the Formulas icon , select the Line item in New Parameter of type, then click New Parameter of type. 4. Click the Formulas icon. In the parameter list, select the line you have just created (Geometrical Set.1 Line.1).
5. Click Add Formula and add the formula below in the editor: Geometrical Set.1 Line.1 = inertiaAxis(3,PartBody) The inertiaAxis function is accessible through the Line constructors. The axis number 3 is the one which is in the extrusion direction (normal to yz). Click OK in the Formulas dialog box. The inertia axis is displayed in the geometry area. 6. Back to . Create three length type parameters: X, Y and Z.
7. Retrieve the coordinates of the point located at the intersection of the inertia axis and the 'yz plane'. To do so, create the formulas below: X=intersect(Geometrical Set.1 plane').coord(1) Y=intersect(Geometrical Set.1 plane').coord(2) Z=intersect(Geometrical Set.1 plane').coord(3) Line.1, 'yz Line.1, 'yz Line.1, 'yz
8. You get the intersect function from the Wireframe constructors and the point.coord method from the Measures item of the dictionary. 9. Check the value displayed in the specification tree as well as in the Formulas dialog box. The KwoGettingStarted.CATPart document used as a sample for the Product Engineering Optimizer User's Guide illustrates this scenario.
Applying Ranges to Parameters by Using a Rule
This task explains how to apply ranges to parameters by using a rule.
1. Open the KwrRangesParameters.CATPart. 2. Click the icon and select Real in the scrolling list to create two parameters of Real type: Real.1 and Real.2. 3. Select Real.1 and right-click the field next to the Edit name or value of the
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current parameter box. 4. Select Add Range The Range of Real.1 dialog box opens.
5. Specify the Minimum and the Maximum bounds (-5 and 5 for example), and click OK twice. 6. Access the Knowledge Advisor workbench and click the Rule icon ( Rule editor opens. 7. Enter the following rule: Real.2 =Real.1 .InferiorRange and click OK: Real.2 value changes to -5. ). The
8. Double-click the rule under the Relations node and replace the existing script with Real.2 =Real.1 .SuperiorRange and click OK: Real.2 value changes to 5.
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Creating an Associative Link Between Measures and Parameters
This scenario explains how to create a persistent and associative link between a measure created using the Measure Item or Measure Between command and a parameter. • Measure Item allows you to get the length of a curve (edge, line, curve), radius or angle depending on the parameter magnitude. Measure Between allows you to get the minimal distance or angle between two elements, depending on the parameter magnitude.
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This link can be created only if the Keep measure option is checked in the Measure Item and Measure Between dialog boxes (if not the result is copied as a simple value.) • No formula is created when using the Measure Item or the Measure Between commands. The icon located on the right of the editor field is a measure between or item icon. Note that you will be able to edit the measure.
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The parameters located below the Parameters node are directly linked to the measures. You can invert the sign of the parameter using the Invert value command in the Measure Item or Measure Between window. The sign concerns only the valuated parameters and not the parameter of the measure.
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To have an associative link, you must make an associative measure. If you select the Picking point mode and the Measure between function, the measure will not be associative. As a result, there will be no associative geometry. When a measure is not associative, the value is displayed in the value field. Even in the case of an associative measure, if you only want to get the result of the measure, uncheck the Keep measure check box.
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To create a "smart" customization, click the Customize... button in the Measure Item dialog box to see the properties the system can detect for the various types of item you can select.
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1. Open the KwrPlaneWing.CATPart file. The following image is displayed.
Using the Measure Item... command
2. Add a parameter of Length type. o Click the Formula icon ( o ). The Formulas dialog box is displayed.
In the New parameter of type scrolling list, select Length and click the New parameter of type button. Length.1 is displayed in the Edit name or value of the current parameter field. Right-click the value field of Length.1 and select the Measure Item... command. The Measure Item dialog box is displayed.
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Make sure the Keep measure option is checked in the Measure Item dialog box. In the specification tree, expand the Sketch.1 node, and select Spline.2. The selected item is highlighted in the geometry and its measure is displayed in green.
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Click OK in the Measure Item dialog box and OK in the Formulas dialog box. A new parameter is added below the Parameters node and below the Measure node. The Length.1 parameter is now linked to the result of the measure.
Using the Measure Between... command
1. Add a parameter of Angle type. o Click the Formula icon ( ). The Formulas dialog box is displayed.
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In the New parameter of type scrolling list, select Angle and click the New parameter of type button. Angle.1 is displayed in the Edit name or value of the current parameter field. Right-click the value field of Angle.1 and select the Measure Between... command. The Measure Between dialog box is displayed.
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In the Selection 2 mode scrolling list, select the Edge only option. In the specification tree, select Plane xy then select the geometry as shown below.
The selected items are highlighted in the geometry and the measure is displayed in green.
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Click OK in the Measure Between dialog box and OK in the Formulas dialog box. An angle parameter is added below the Parameters node and the measure is displayed below the Measure node.
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Click here to display the result sample.
2.
Note that: • • if several characteristics of the measure are computed and have the same magnitude, the system will choose the most convenient according to predefined rules. To remove the link to the measure, right-click the measure item in the specification tree and select the measure object->Remove the link with measure command.
Publishing Parameters
This scenario explains how to publish parameters. The scenario described below is divided into the following steps: • Add parameters to the Screw.2 document and publish its Diameter, Depth, and Volume parameters. Repeat the same operations with the second CATPart file. Create a CATProduct file and import Screw.2.
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In the context of the Bolt product, insert the Nut part that imports the Depth and the Diameter parameters by selecting the publication MyDepth and MyDiameter of Screw.2. In the context of the bolt, replace Screw.2 (KwrScrew.CATPart) by Screw.2 (KwrScrew2.CATPart) that doesn't have the same structure as the first one but owns the same publications. Both the parameters and the check are recomputed.
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A publication has a name and references a geometry or parameters inside the product (or one of its subproducts). The publication of parameters should be used when: • Defining an import of parameters between two parts (similar to the import of geometry). Defining relations at the assembly level between parameters (similar to constraints).
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Before you start, make sure that the Keep link with selected object check box is checked (Tools->Options->Infrastructure->Part Infrastructure->General). 1. Open the KwrScrew.CATPart document. The following image is displayed.
2. Add parameters to the part. icon. The Formula Editor opens. In the New parameter of type scrolling Click the list, select Volume and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the
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parameter: MyVolume. Click Apply and click the Add Formula button. The Formula Editor opens. o Enter the following formula by using the Dictionary: smartVolume(PartBody Click OK, and Yes. o Pad.1 ) + smartVolume(PartBody Pad.2 ) .
In the New parameter of type scrolling list, select Length and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: MyDepth. Click Apply and click the Add Formula button. Enter the following formula: MyDepth=PartBody Pad.2 FirstLimit Length and click OK.
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In the New parameter of type scrolling list, select Length and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: MyDiameter. Click Apply and click the Add Formula button. Enter the following formula: MyDiameter=PartBody twice. Sketch.2 Radius.2 Radius * 2. Click OK
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3. Publish the MyVolume, MyDepth, and MyDiameter parameters.
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To do so, select the Tools>Publication command and select the MyVolume, MyDepth, and MyDiameter parameters in the specifications tree. Click OK. The published parameters appear in the specifications tree below the Publication node. Close the file.
4. Open the KwrScrew2.CATPart and repeat the steps listed above (steps 1 to 3 included). The part should be identical to the one below. Close the file.
5. Create a CATProduct file. Select the Insert->Existing Component... command and click the root of the specifications tree. The File selection box is displayed. Select the KwrScrew.CATPart file and click Open. The screw is imported. 6. Select the Insert->Existing Component... command, select the Kwrnut.CATPart file and
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click Open. The nut part is inserted.
7. Double-click the inner circle of the nut, the Hole Definition window is displayed. o Right-click the Diameter field and select the Edit formula... command. The Formula Editor opens. Select MyDiameter in the screw publications. The formula should be as follows: PartBody o Hole.1 Diameter=`External Parameters
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MyDiameter`. Click O
Right-click the Depth field and select the Edit formula... command. The Formula Editor opens. Select MyDepth in the screw publications. The formula should be as follows: PartBody Parameters Hole.1 HoleLimit.1 Depth=`External
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MyDepth`. Click OK twice.
8. Double-click, then right-click the Screw.2 component in the specifications tree and select the Components->Replace Component... command. The File Selection window opens. Select the KwrScrew2.CATPart file and click Open. 9. Click Yes when prompted to replace all instances with the same reference as the selected product. Update the nut part: the parameters are recomputed.
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Activating and Deactivating a Component
This task explains how to activate and deactivate a component. In the scenario described below, the CATProduct file contains two CATPart files that you will activate and deactivate alternatively after creating user parameters and a rule based on these parameters. Note that: • Relations located at the product level are not integrated to the
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product update. If your relation drives the parameters of a Part, create the relation at the Part level. Parameters driven by rules are designed to enable you to control components activities at assembly level.
When working in a Japanese environment, remember to check the Surrounded by the Symbol' option (Tools->Options->General->Parameters and Measure->Knowledge tab).
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1. Open the KwrSyringe.CATProduct file and save the following files in the same directory (SyringePiston.CATPart, HollowSyringePiston.CATPart, and SyringeContainer.CATPart): This file contains a syringe made up of three different parts: A barrel, and two different plungers. 2. Create a multiple value parameter of string type. • • Click the icon. The Formulas Editor opens.
Select String in the scrolling list with Multiple Values. Click the New Parameter of type button. The Value List dialog box opens. Enter two different values, Hollow and Full, and click OK. Edit the name of the new parameter (SyringeType in this scenario) in the Edit Name or value of the current parameter and click OK. The new parameter is displayed under the Parameters node of the Specification tree.
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3. Access the Knowledge Advisor workbench and click the Rule icon to create a rule. The script of this rule will allow you to enable or disable one of the plungers. 4. Enter the code below in the Rule Editor, and click OK. if (SyringeType == "Hollow") { `S3\Component Activation State` `S2\Component Activation State` } else { `S2\Component Activation State` `S3\Component Activation State` }
= false = true
= false = true
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Note that Japanese users should enter the following rule.
6. Double-click the SyringeType parameter under the Parameters node and select Hollow in the Edit Parameter window. The SyringeBarrel CATPart and the HollowSyringePlunger CATPart are displayed.
7. Double-click the SyringeType parameter and select "Full" in the Edit Parameter window. The SyringeBarrel CATPart and the SyringePlunger
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CATPart are displayed.
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Creating an External Parameter
This tasks shows how to create an external parameter. • Make sure you have checked: o the Parameters and the External References check boxes below the Display in Specification tree settings in the Tools->Options->Infrastructure-> Part Infrastructure->Display dialog box, as well as the With Formula and With Value check boxes below the Parameter Tree View settings in the Tools->Options->General->Parameters and Measure dialog box.
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Open the DeactivatingExternalParameter.CATProduct file.
Note that the external parameters created at a product level are not integrated to the update process.
1. Expand the Part1_External_Parameter(Part1.1)\Part1_External_P arameter document, right-click the Line_Length parameter located below the Parameters node in the specification tree, and select the Copy command. 2. Double-click, then right-click Part2_External_Parameter (Part2.1)\Part2_External_Parameter and select the Paste Special command. In the Paste Special dialog box, select As Result With Link and click OK to validate. The External Parameters node is added to the specification tree and the Line_Length parameter is displayed.
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Deactivating and Re-activating External Parameters
This tasks shows how to deactivate, re-activate and synchronize external parameters. In the scenario described below, you: • • • • Create an external parameter Deactivate the external parameter Modify the parameter pointed by the external parameter Re-activate the external parameter
Until now, external parameters (external references) could be: • • synchronized (if their values were different from the values of the pointed parameter). isolated (external parameters become simple parameters) .
Now you can deactivate and re-activate external parameters. It means that when the external reference is deactivated, it cannot be synchronized with the pointed value, but it keeps its last value (the value cannot be changed any longer). The external parameter can also be reactivated: Its native behavior is then restored. Note that: • • •
A deactivated external parameter will only lose the ability to be synchronized and will keep its last value. A deactivated external parameter can be re-activated using its contextual sub-menu. The Activate, Deactivate, Synchronize, and Isolate commands can also be accessed from the Links dialog box (Edit->Links.) Make sure you have checked: o the Parameters and the External References check boxes below the Display in Specification tree settings in the Tools->Options->Infrastructure-> Part Infrastructure->Display dialog box. as well as the With Formula and With Value check boxes below the Parameter Tree View settings in the Tools->Options->General->Parameters and Measure dialog box,
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Open the DeactivatingExternalParameter.CATProduct file.
Creating the external parameter
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1. Expand the Part1_External_Parameter(Part1.1)\Part1_External_P arameter document, right-click the Line_Length parameter located below the Parameters node in the specification tree, and select the Copy command. 2. Double-click, then right-click Part2_External_Parameter (Part2.1)\Part2_External_Parameter, and select the Paste Special command. In the Paste Special dialog box, select As Result With Link and click OK to validate. The External Parameters node is added to the specification tree and the Line_Length parameter is displayed.
Deactivating the external parameter
3. Right-click this external parameter and select the Part2_External_Parameter\External Parameters\Line_Length object-> Deactivate command. A mask ( ) indicating that the paramete is deactivated is displayed next to the parameter name.
4. Double-click Part1_External_Parameter, right-click Line_Length twice in Part1_External_Parameter and select the Line_Length object->Formula->Edit... command. Modifying the parameter pointed by the external parameter
5. In the Formula Editor, modify the formula so that it matches the following formula: Line_Length=Length(PartBody\Line.1)*2. Click OK when done. The Line_Length parameter value updated in Part1_External_Parameter. Note that it is not updated in Part2_External_Parameter since th external parameter is deactivated. Re-activating the external parameter
6. Go back to the external parameter you've created, right-click it and select the Part2_External_Parameter\External Parameters\Line_Length object->Activate command. A mask ( ) indicating that the parameter is deactivated is displayed next to the parameter name. 7. Right-click it and select the Part2_External_Parameter\External Parameters\Line_Length object->Synchronize command. The parameter is updated and a mask ( ) indicating that the parameter is deactivated is displayed next to the parameter name.
Getting Familiar with the Parameters Explorer
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Contrary to the parameters created using the Formulas editor, the parameters created using the Parameters Explorer display below the feature selected in the specification tree.
icon in the standard tool The Parameters Explorer dialog box is displayed when you click the bar. This dialog box allows you to add parameters to features. It is made up of the following fields: • • • • • Feature Parameters Parameter Properties Ranges
Feature
This field indicates the item selected in the specification tree to which the parameter will be added.
Parameters
This field enables you to create the parameters that will be added to the feature that you selected in the specification tree. To know more about this field, see Getting Familiar With the f(x) Dialog Box.
Parameter
The Value field enables you to assign a value to the created parameter.
Properties
The Local Name field enables you to modify the name of the parameter that you created. The Name field indicates the way the parameter will be displayed in the editors. The Comment field enables you
Ranges
The Inf. Range check box, if checked, enables you to add
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an inferior range to the parameter.
to add comments to the parameter.
The Sup. Range check box, if checked, enables you to add an inferior range to the parameter. The Constant check box, if checked, enables you to lock the parameter. In this case, the parameter cannot be modified. The Hidden check box, if checked, enables you to decide if you want the parameter to be displayed or not.
Adding a Parameter to a Feature
This task explains how to add two parameters to a circular pattern feature. One parameter is a multiple value string, the other is a mass with upper and lower bounds. 1. Open the KwrBallBearing1.CATPart document. 2. In the specification tree, select the root feature, then select the Start->Knowledgeware->Knowledge Advisor command to access the Knowledge Advisor workbench. 3. In the specification tree, select the CircPattern.1 feature. 4. Click the Parameters Explorer displayed: icon, the dialog box below is
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5. In the New Parameter of Type list, select the String type, then in the opposite field ('With'), select the Multiple Values item. Click New Parameter of Type. 6. In the <Value list dialog box: a) enter the Type1 string, then press Enter b) enter the Type2 string, then press Enter c) click OK to go back to the Parameter Explorer dialog box. 7. If need be, rename the created parameter in the Local Name field and add a comment. 8. In the New Parameter of Type list, select the Mass type, then in the opposite field ('With'), select the Single Value item. Click New Parameter of Type. The MASS.1 name is displayed by default in the Properties and a default value of 0kg is assigned to the created parameter. 9. Modify these values as indicated on the figure below:
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10. Click OK. Both parameters are displayed in the specification tree right below the CircPatter.1 feature. Parameters added by using the Parameters Explorer are displayed right below the feature they are assigned. 11.
Adding a Parameter to an Edge
This task explains how to add parameters to an edge by using the Parameters Explorer. Note that this new function is designed to work on edges, faces and vertex.
1. Open the KwrSupport.CATPart file. The following image is displayed.
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2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 3. Click the Add Parameters on Geometry icon ( of Pad.2. ) and select the upper edge
The Parameter Explorer dialog box opens. 4. In the New Parameter of type scrolling list, select the Length parameter type, and click the New parameter of type button. 5. In the Local Name field, enter the name of the parameter. For the purpose of this scenario, enter Extract_Length, and click OK to validate. A new Extract feature is created and the parameter you just created is added to this feature.
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Parameters added by using the Parameters Explorer are displayed right below the feature they are assigned.
Locking and Unlocking a Parameter
This task explains how to lock and unlock parameters: 2 new commands are now available in the Knowledge toolbar: the Lock selected parameters... and the Unlock selected parameters... commands. 1. Open the KwrLockingUnlockingParameters.CATPart file. 2. Expand the Parameters node and click the f1 parameter. 3. In the Knowledge toolbar, click the Lock selected parameters... icon ( ) to lock this parameter. The parameter is locked (a lock is displayed next to the parameter in the specification tree.) 4. To unlock the parameter, select the f1 parameter in the specification tree and click the Unlock selected parameters... icon ( toolbar. Note that: ) in the Knowledge
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The Lock selected parameters... and Unlock selected parameters... commands enable the multiselection of parameters or features.
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The parameter contextual menu can be used to lock or unlock the parameter.
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The Lock selected parameters... and Unlock selected parameters... commands are recursive: If you select a feature, the parameters located below this feature are locked or unlocked. Parameters that do not have a 3D representation can be locked and unlocked. o o o Open the Formulas Editor to access the parameter. Select the parameter in the Parameters list In the Edit name or value of the current parameter value field, access the contextual menu and select the Lock/Unlock command. (click the graphic opposite to enlarge it.)
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Constraints can be locked and unlocked. o Select the constraint in the specification tree and click the Lock selected parameters... )/Unlock selected parameters A lock is displayed next to the constraint in the ( ) icon, or Sketcher. Locked constraints Right-click the constraint in the display in orange. specification tree and select the Lock the parameter/Unlock the parameter command. (
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Creating Sets of Parameters
This task explains how to create sets of parameters. You can create sets of parameters below the Parameters node of the specification tree. Using this capability enables you to regroup parameters by categories. 1. Check at least the Parameters and Relations options of the Display tab in the Tools->Options...->Infrastructure->Part Infrastructure settings. 2. Open any document containing at least one parameter or create a document and add a parameter to it (otherwise, you won't have the Parameters node displayed in the specification tree). 3. Click the icon, then select the Parameters node in the specification tree. The Parameters.1 (or Parameters.n) parameter set is added to the specification tree right below the Parameters node. 4. Click the icon to add a new parameter in the created parameter set. The Parameter Explorer dialog box is displayed. In the specification tree, select the Parameter Set you want to add a parameter to. The name of the parameter set is displayed in the Feature field of the Parameter Explorer dialog box. 5. Fill in the other fields of the Parameter Explorer dialog box. If need be, see Adding a Parameter to a Feature. 6. After you have finished specifying the new parameter, click OK in the Parameter Explorer dialog box. In the specification tree, you can expand the feature which represents the parameter set. A new parameter has been added below the parameter set.
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Parameters belonging to a parameter set can be reordered by using the Reorder... command from the contextual menu.
Working with Formulas
Working with Formulas
Select the Formula icon to specify relations between parameters.
Introducing Formulas Getting Familiar With the f(x) Dialog Box Using the Dictionary Creating a Formula Creating Formulas based on Publications Specifying a Measure in a Formula Using Geometry to Create a Formula Referring to External Parameters in a Formula Using the Equivalent Dimensions Feature
Introducing Formulas
Formulas are features used to define or constrain a parameter. A formula is a relation: the left part of the relation is the parameter to be constrained, the right part is a statement. Once it has been created, a formula can be manipulated like any other feature from its contextual menu. The formula language uses operators and functions of all types whereby you can perform operations on parameters.
Displaying Formulas in the Specification Tree
Formulas are relations and as such they can be displayed below the Relations node provided you check the 'Relations' box below the 'Specification tree' settings in the Tools->Options>Infrastructure-> Part Infrastructure->Display dialog box. In addition, formulas can also be displayed below the Parameters node provided you check: • the 'Parameters' box below the 'Specification tree' settings in the Tools>Options->Infrastructure-> Part Infrastructure->Display dialog box • as well as the 'With Formula' box below the Parameter Tree View settings in the Tools->Options->General->Parameters and Measure dialog box
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The Activity Parameter
A formula is a feature which is assigned a parameter called the activity. The activity value is a boolean. If the activity is set to true, the parameter value cannot be calculated from the formula. If a formula is created for a parameter which is not already constrained by another formula, the activity of the new formula is set to true by default. A parameter can be constrained by several formulas, but only one formula can be active at a time. Before activating a formula on a given parameter, you must deactivate the other formulas defined on the same parameter. Activity value Relation icon in the specification tree false true
Importing Formulas
Parameters as well as the associated formulas can be imported from an external file. Refer to Introducing Parameters and Importing Parameters for more information on how to import formulas.
Getting Familiar With the f(x) Dialog Box
The f(x) dialog box is displayed when you click the box allows you to: • Display the list of parameters • • Create parameters and formulas Import external files. icon in the standard tool bar. This dialog
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The parameter list
Basically, the parameter list displays the parameters related to the feature selected either in the specification tree or in the geometry area. If no feature has been selected, all the document parameters are displayed. The dialog box being open, you can select a given feature either in the tree or in the geometry area and display its related parameters. You can restrict the list of displayed parameters by using the Filter Name and Filter Type capabilities as well as the Incremental check box.
The Filter Name filter
This filter allows you to narrow the list of displayed parameters by specifying a substring. If you specify *Limit* as filter, only the parameter with Limit as sub-string will be displayed, for example: PartBody PartBody PartBody PartBody Pad.1 Pad.1 Hole.1 Hole.1 FirstLimit SecondLimit HoleLimit.1 HoleLimit.1 Length Length Depth Angle
The Filter Type filter
This filter allows you to restrict the list of parameters by specifying a type. Selecting User parameters will display only the parameters created by the New Parameter of type button.
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Selecting Hidden parameters will display only the list of parameters which have been declared as hidden by using the Hide command from the value field contextual menu. The Hide command is only available for user parameters.
The Incremental check box
Selecting a feature in the specification tree or in the geometry area is displayed in the editor only the first level of features right below the selected feature. The parameter list on figure above displays all the parameters related to the Pad.1 and Hole.1 features. Selecting Pad.1 in the tree (Incremental unchecked) will display the parameters below: PartBody PartBody PartBody Pad.1 Pad.1 Sketch.1 FirstLimit SecondLimit Radius.3 Length Length Radius
Checking Incremental restricts the list of parameters to the one below: PartBody PartBody Pad.1 Pad.1 FirstLimit SecondLimit Length Length
The 'Edit name of value of the current parameter' field
This field displays the parameter which has been selected in the parameter list. The value field on the right-hand side is grayed out when the parameter is constrained by a formula, a design table or any type of relations. Right-clicking this value field provides you with a number of commands whereby you can refine the parameter definition.
The New Parameter of type button
This button allows you to create a user parameter. This user parameter can be assigned a single value or multiple values (akin to the enum idea).
The Delete Parameter button
This capability operates only for user parameters.
The Add Formula button
When you create a formula, you specify that a parameter, whatever its type, is to be constrained by a relation. Clicking the Add Formula button displays the Formula editor. The formula which is created is displayed in the parameters list as well as its activity. To know more about the Dictionary available in the Formula editor, see Using the Dictionary.
The Delete Formula button
When a parameter which is constrained by a formula is selected in the parameter list, clicking Delete Formula removes the formula.
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The Import button
This capability allows you to import parameters and parameter values from a text file or from an Excel file (Windows).
Using the Dictionary
Using the Dictionary
The Dictionary allows you to access the functions, operators and feature attributes that can be used in relations. It can be accessed from the Formula Editor, the Rule Editor, the Check Editor, and from the Action Editor.
Packages displayed in the left part of the browser are those you selected from the Tools->Options ->General->Parameters and Measure->Language tab. Keywords Point Constructors Line Constructors Direction Constructors Messages and macros Measures Part Measures Object Design tables Law Circle Constructors Electrical Functions Attribute Surface Constructors Plane Constructors Math Operators Search Function String Space Analysis List Wireframe Constructors Analysis Operators
Constants
The following constants are specified or recognized by CATIA when programming rules and checks. As a result, they can be used anywhere in a relation in place of the actual values. • • • • false - one of the two values that a parameter of type Boolean can have true - one of the two values that a parameter of type Boolean can have PI - 3.14159265358979323846 - The ratio of the circumference of a circle to its diameter. E - The base of natural logarithm - The constant e is approximately 2.718282.
Electrical User Functions
About the Electrical User Functions...
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User Tasks • • • • • • Elec_DistanceCommon DistanceWireProduct ListAllOuterLayerObjects ListDirectlyCoveredObjects ListDirectlyOuterLayerObjects VisualMode
To be able to use these functions, you need to activate the ElectricalMeasure package. To do so: 1. Select Tools -> Options... -> General -> Parameters and Measures and go to the Language tab. 2. Choose the ElectricalMeasure package and click the right arrow: 3. Click OK to validate.
Elec_DistanceCommon
Syntax Elec_DistanceCommon(Wire1: Wire, Wire2: Wire):Length Returns the common length of the two wires given as input arguments. The type of Wire1 and Wire2 is ElecWire. Example 1 The Elec_DistanceCommon user function can be used in Knowledge Expert to find all the couples of wires in the session that have a common length greater than a given value. Example 2 In Knowledge Advisor, it can be used to define a rule giving the common length of two specific wires sharing properties. Applying the rule displays the following message if the condition is met: Example 3 Still in Knowledge Advisor, to verify that two wires selected in the specification tree have a common length, the following action can be defined: then ran: select two wires in the specification tree and click OK to validate. The following message displays:
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DistanceWireProduct
Syntax DistanceWireProduct(Wire1: Wire, Object: Product):Length Returns the minimum length between a wire and a product in session. The product must contain at least one part. Example 1 The DistanceWireProduct user function can be used with the f(x) command to display the distance between a wire and a component in the session. This formula returns the following value: Example 2 The DistanceWireProduct user function can be used in Knowledge Expert to find all the wires in the session that have a minimum distance to defined components smaller than a critical value chosen by the user. The components can be defined as heat-resistant. Properties have been added to the product: and to the wires: A check is defined as follows: Updating the session displays green/red light on the check: A report is generated showing the check result: some wires verify the condition, other not. Example 3 The DistanceWireProduct user function can be used in Knowledge Advisor to define a rule that displays a warning message if a minimum distance between a wire and an object is smaller than a critical value chosen by the user. Running this rule displays the following message: Example 4 Still in Knowledge Advisor, an action can be defined using the DistanceWireProduct user function, to know the distance between a wire and an object selected in the specification tree: Run the action using the Action.1 contextual menu:
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User Tasks select a wire and a product in the specification tree then validate. This message displays:
ListAllOuterLayerObjects
Syntax
ListAllOuterLayerObjects (ElecBundleSegmentExtremity:Feature,Offset:Real,ListOfAllCoveringProducts(Protections/Supports):out List):Boolean Returns an ordered list of protective coverings and supports that cover the bundle segment at the point of interest. The point of interest is defined by specifying from which end of the bundle segment and entering an offset in mm. Example A check (in KWE advanced language) to determine the protective coverings and supports at 150 mm from end 1 (Extremity 1) of the bundle segment is written as follows:
ListDirectlyCoveredObjects
Syntax ListDirectlyCoveredObjects((Protection/Support):Feature, ListOfCoveredProducts(BundleSegments/Protections/Supports): out List):Boolean Returns the list of bundle segments, protective coverings and/or supports directly under the component (protective covering or support) you want to analyze. If the component you want to analyze is not a protective covering or a support, the list returned will be empty. Example
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Tape A is placed directly over the bundle segment Corrugated tubes B and C are linked to the bundle segment, and corrugated tube B covers tube C Standard support D is linked to the bundle segment.
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knowledgewareAdvisor A check (in KWE advanced language) to determine the list of bundle segments, protective coverings and supports under corrugated tube C is written as follows:
Running this check returns: • • The name of the component analyzed, in our case, corrugated tube C The number of objects covered by corrugated tube C:
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Followed by the name of this component: the bundle segment.
ListDirectlyOuterLayerObjects
Syntax ListDirectlyOuterLayerObjects ((BundleSegment/Protection/Support):Feature, ListOfCoveringProducts(Protections/Supports): out List):Boolean Returns the list of outer layers of protective coverings and/or supports directly over the component (bundle segment, protective covering or support) you want to analyze. If the component you want to analyze is not a bundle segment, protective covering or a support, the list returned will be empty. Example
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Tape A is placed directly over the bundle segment Corrugated tubes B and C are linked to the bundle segment, and corrugated tube B covers tube C
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User Tasks • Standard support D is linked to the bundle segment
A check (in KWE advanced language) to determine the list of outer layers that directly cover the bundle segment in the example is written as follows:
Running this check returns: • • The name of the component analyzed, in our case, the bundle segment. The number of outer layers over the bundle segment:
Only 3 are found because corrugated tube B does not directly cover the bundle segment since it covers corrugated tube C. • Followed by the names of these components:
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•
VisualMode
Syntax VisualMode (BundleSegment: Feature, Visualization Mode (LIGHT/FULL): String): Boolean Description This function is useful to minimize the size of the harness in LIGHT mode. It simplifies the visualization, the curve and the diameter only are represented, the rib being deleted. This function is only available for bundle segments belonging to multi-branchable documents. Example Create a rule in Knowledge Expert:
Running this rule displays the harness in LIGHT mode:
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The rule is reversible: you can load a harness in LIGHT mode and reload the geometry by applying the rule with the FULL parameter:
The harness is displayed in FULL mode: the rib is recreated:
Working in LIGHT mode allows you to modify the route and route wires but the split, transfer and add branch point commands are not supported. To know more about these commands, refer to Electrical Harness Installation - Working with
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Creating a Formula
This task explains how to create a formula specifying that the external radius of a hollow cylinder is twice its internal diameter. Note that the radius of a sketch can be defined by a formula provided it is declared as a constraint. Make sure the Relations option is active in the Tools->Options...>Infrastructure->Part Infrastructure->Display tab. 1. Open the KwrStartDocument.CATPart document. icon to display the f(x) dialog box. Make sure that the 2. Click the Incremental box is unchecked. Method 1 o Double-click the PartBody Sketch.1 Radius.3 Radius parameter in the parameter list. The Formula Editor is displayed. Enter the PartBody Hole.1 HoleLimit.1 Depth*2 relation in the formula field. Go to Tips and Techniques for information on how to manipulate parameters and formulas. Click OK in the Formula Editor.
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Method 2 o Select the PartBody parameter list. Sketch.1 Radius.1 Radius in the
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Click Add Formula. The Formula Editor is displayed. Enter the PartBody Hole.1 HoleLimit.1 Depth*2 relation in the formula field. Go to Tips and Techniques for information on how to manipulate parameters and formulas. Click OK in the Formulas Editor.
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3. Click Apply to update the document. 4. Click OK to close the dialog box.
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Creating Formulas based on Publications
This task explains how to create a formula based on publications in a CATProduct file.
1. Open the Screw1.CATPart document. 2. Add a Volume parameter to the part. o icon. The Formula Editor opens. In the New parameter Click the of type scrolling list, select Volume and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: ScrewVolume1. Click Apply and click the Add Formula button. The Formula Editor opens. Enter the following formula by using the Dictionary to access the smartVolume operator: ScrewVolume1=smartVolume(PartBody times. Pad.1). Click OK three
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3. Create another Volume parameter called ScrewVolume2 based on Pad.2. 4. Create another Volume parameter called Volume_Total. Click OK when done to exit the Formula editor. 5. Access the Tools->Publication menu, and select the 3 parameters that display below the Parameters node. Assign them new names (see graphic below):
6. Click OK when done. The parameters, the formulas, and the publications are created (see graphic below).
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7. Save your file and close it. 8. Open the Screw2.CATPart document. Repeat the above steps (2 to 7).
9. Create a new product (File->New menu). Click OK when done. 10. Select the Insert->Existing Component... command to insert Screw1.CATPart into the product. 11. In the File Selection window, select the Screw1.CATPart file that you have just saved. Click Open. 12. Create a formula that will compute the volume of the screw. o Click the Root product and click the icon. The Formula Editor
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opens. o Enter the following formula into the editor by selecting the publications in the specification tree:
o o Click OK when done. The screw volume is displayed below the parameters node.
13. Double-click screw.1 in the specification tree, right-click it, and select the Components>Replace Component command. 14. In the File Selection window, select the screw2.CATPart file that you have just saved and click Open. 15. Click OK in the Impacts On Replace window. The new screw is inserted into the product and its volume is computed.
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Specifying a Measure in a Formula
The purpose of this task is to explain how to specify that the value of a Length type parameter is equal to the curvilign abcissa of a point located on a curve. Measures, i.e. values captured from the geometry area can be used in formulas. Here are some examples of measures that can be used in formulas: • • • Distance between two points. Total length of a curve. Length of a curve segment - between a point and the origin or between a point and the curve extremity. Length of a curve segment - between two points. Area of an extruded surface.
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1. Check the Load extended language libraries box in the Tools>Options->General->Parameters and Measure->language tab. 2. Open the KwrMeasure.CATPart document. The whole document has been created using the Generative Shape Design product. The Extrude.1 and Extrude.2 surfaces are extruded from the Spline.1 and Spline.2 curves. The point whose abscissa is to be measured is Point.5. The origin of the curve where Point.5 is located on is Point.8
3. Click the Formula icon. The f(x) dialog box is displayed. 4. Create the CurveLengthFromOrigin parameter.
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Select the Length item with Single Value in the New Parameter of type list, then click New Parameter of type. The new parameter appears in Edit name or value of the current parameter. Replace the Length.1 name with CurveLengthFromOrigin, and click Apply.
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5. Specify that the value of CurveLengthFromOrigin is the abscissa of Point.5: 4. a. Select the CurveLengthFromOrigin parameter in the parameters list, then click Add Formula. The Formula editor is displayed. b. Select the Measures item from the Dictionary list. c. In the list of measures, double-click the length(Curve,Point,Boolean) item. The length function is added to the Formula Editor.
d. Fill in the Formula editor field as indicated below. 1. The three arguments are: a curve to be selected from the geometry area, a point to be selected from the geometry area and a boolean. 2. Position the cursor where the first argument is intended to be typed. Then double-click the Spline.2 feature in the specification tree. The curve argument is added to the length definition. 3. Position the cursor where the second argument is intended to be typed. Then double-click the Point.5 feature in the specification tree. The point argument is added to the length definition. 4. Type a boolean for the third argument: True if the length is to be calculated from the origin, False if the length is to be calculated from the curve end.
5. Click OK to confirm the formula definition. You are
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back to the Formulas dialog box. The CurveLengthFromOrigin formula and value(47.5mm) are added to the parameter list. e. Click OK to add the parameter as well as its formula to the document.
Using Geometry to Create a Formula
This task explains how to use geometry to create a formula. Before performing this scenario, make sure you have checked the Keep link with selected object option (Tools->Options-> Infrastructure->Part Infrastructure->General tab.) 1. Create a Product and add 2 parts to this product. 2. From the Start->Shape menu, access the Generative Shape Design workbench. Select the first part. 3. Add a line to the part. 4. Select the second part and add a Length parameter to the part as well as a formula that will be based on the line. o Click the icon. The Formula Editor opens. In the New parameter of type scrolling list, select Legnth and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: LineLength. Click Apply and click the Add Formula button. The Formula Editor opens. Enter the following formula by using the Dictionary to access the length(Curve,...) operator: LineLength=length(). Position the cursor between the parenthesis and double-click the Line in the geometry or in the specification tree. The External parameter selection window is displayed. Select Line.1 and click OK. The formula is displayed as follows: LineLength=length(`External References\Line.1` ) Click OK when done. Click Yes in the Automatic update window.
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5.
Refering to External Parameters in a Formula
This scenario shows how to use external parameters in a formula. In a formula, you can use parameters defined in external documents. This works between any types of document. For example, in a CATPart document, you can specify a formula referring to parameters defined in a CATDrafting document. External parameters can also be used when working within an assembly. Prior to performing this scenario, make sure that the Keep link with selected object option is checked (Tools->Options...->Infrastructure->Part Infrastructure->General).
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1. Open the KwrStartDocument.CATPart document as well as the KwrImportParameter.CATPart document. Select the Window->Tile Vertically command from the standard menu bar. Both documents are displayed. 2. Make active the KwrImportParameter document. Click the icon to display the f(x) dialog box. 3. Create a parameter of Length type and click the Add Formula button. The formula editor is displayed. 4. In the KwrStartDocument specification tree, select the Hole.1 feature. The External parameter selection dialog box is displayed.
5. In the External parameter selection dialog box, select the Diameter object in the external parameter list. Then click OK. The Length.1 definition is carried forward to the formula editor. (Click the picture below to enlarge it.)
6. Complete the formula definition as indicated below: Length.1 = Diameter*0.45 7. Click OK in the formula editor. You are back to the Formulas dialog box. In the parameter list, the Length.1 parameter value is modified according to the formula specified. In the KwrImportParameter specification tree, the External Parameters node is added. Expand this node to display the Diameter parameter.
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8. Click OK to add the formula to the KwrImportParameter.CATPart document and exit the dialog. 9. Select the Edit->Links command from the standard menu bar. The displayed dialog box confirms that there is a link between the KwrImportParameter KwrStartDocument Length.1 object and the PartBody Hole.1 Diameter object.
10. Click Isolate in the Links dialog box, then click OK. In the KwrImportParameter.CATPart specification tree, the External Parameters node can no longer be expanded and the Diameter parameter is added below the Parameters node.
11. Select the Edit->Links command from the standard menu bar. A message box informs you that the active document has no external links.
12.
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Using the Equivalent Dimensions Feature
This scenario explains how to use the Equivalent Dimensions Feature. The scenario described below is divided into the following steps: • • you apply constraints to an existing sketch. you use the Equivalent Dimensions feature to create a list of Length type parameters that will have the same value.
To know more about the Equivalent Dimensions feature, see Getting Familiar with the Equivalent Dimensions Interface. 1. Open the KwrEquivalentDimensions.CATPart. The following image is displayed:
2. In the specification tree, expand the PartBody node and double-click Sketch.1 to access the sketcher. 3. Double-click the Constraint icon ( graphic below). ) to constraint some lines of the sketch (see
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4. In the Knowledge toolbar, click the Equivalent Dimensions icon ( Equivalent Dimensions Edition window is displayed.
). The
5. Click the Edit List... button. In the opening window, use the arrow key to select the following parameters and click OK when done. o o o Length.34 Length.36 Length.37
6. In the Equivalent Dimensions Edition window, set the value to 150mm and click OK. 7. Exit the Sketcher. The sketch is modified accordingly and the EquivalentDimensions.1 feature is displayed below the Relations node.
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8. Double-click Value=150mm twice in the specification tree. The Edit Parameter window is displayed. 9. Enter 140mm and click OK.
Associating URLs and Comments with Parameters or Relations
Associating URLs & Comments with Features
Link Bar 2
Assigning a Comment to a Knowledge Feature
This tasks shows how to add comments to parameters and formulas using the URLs & Comment toolbox as well as the Properties dialog box.
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You can now edit the text that is displayed in the contextual bubbles when dragging your mouse over a relation or a parameter so that you can assign a text to a particular feature. There are 2 ways to edit the text that is displayed in the contextual bubbles: 1. Select the feature to which you want to add a comment. 2. Click the Comment & URLs icon ( ). 3. Enter the text you want to display in the Comment field. 4. Click OK when done. - Or 1. Right-click the relation in the specificatio n tree. 2. Select the Properties command. 3. Enter the comment in the Comment field of the Properties dialog box. Note that:
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• •
if you want the value of the parameter/formula to display, the "\V" combination should be used (see example below). if no comment is added to the feature, the default name of the feature will be displayed.
1. Open the KwrComment.CATPart file. This file contains 3 Length type parameters and a formula that computes the length of a line. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 3. Click the Length.1 parameter in the specification tree and click the Comment & URLs icon ( ).
4. In the Comment field, enter Length.1 is equal to Length.2: \V. Click OK when done. 5. Right-click Formula.1 in the specification tree, and select the Properties command. 6. In the Comment field of the Properties dialog box, enter the following text: Formula that computes the length of the line. 7. Drag your cursor over Length.1 and Formula.1: The bubbles text is modified (see picture below.)
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Working with Design Tables
Working with Design Tables
Select the Design Table icon to create a design table. Introducing Design Tables Getting Familiar with the Design Table Dialog
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User Tasks Box Creating a Design Table from Current Parameters Values Creating a Design Table from a Pre-Existing File Interactively Adding a Row To the Design Table External File Controlling Design Tables Synchronization Storing a Design Table in a Power Copy If you are already familiar with CATIA and only need a quick access to information, see the CATIA Knowledgeware Infrastructure - Tips and Techniques - Summary.
Introducing Design Tables
A design table: • provides you with a means to create and manage component families. These components can be for example mechanical parts just differing in their parameter values. is a tool mainly intended to ease the definition of mechanical parts. It is provided to all CATIA users. But you will make the best use of it in a Knowledge Advisor application. A design table can be created from a CATIA document, the document data is then exported to the design table. It can also be applied to a document, the document data is then imported from the design table. is designed to drive the parameters of a CATIA document from external values. These values are stored in the form of a table either in a Microsoft Excel file on Windows or in a tabulated text file. When using a design table the trick is to associate the right document parameters with the right table parameters. The design table columns may not all correspond to your document parameters and you may decide to apply only part of the design table values to your document. By creating associations, you declare what document parameters you want to link with what table columns. • becomes a more powerful tool when it is used with the Knowledge Advisor. You are provided with functions to read the design table parameters. These design table functions can be used when programming your checks and rules. Using these functions spares you all the association operations. To know more, click here.
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Example
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knowledgewareAdvisor Screws are a good example of mechanical parts that can be described by a design table. To simplify, imagine they are all described by four parameters: the head width, the head height, the body width and the body height. The sets of four parameter values that can be assigned to a screw can be easily regrouped in a design table. This design table has as many columns as screw parameters and as many rows as sets of parameter values. In a design table, a set of parameter values is called a configuration and it is registered in a row. Design Table Formats • • • The Excel Sheet Format (under Windows) The Tabulated Text File Format The CATIA Design Table
Design Table Status
Design Tables Formats
The Excel Sheet Format (under Windows)
The values mentioned in the sheet cells have to be expressed in appropriate units. Otherwise, the right values won't be associated with the document parameters. Only Excel sheets created with Excel 97 and subsequent versions are supported.
If no unit is mentioned within a cell: • the unit taken into account is the one mentioned in the first row • and if no unit is specified in the first row, the unit taken into account is the relevant SI unit.
Here is an example of an Excel sheet: When a configuration which contains empty cells is selected, the parameters associated with the empty cells are not modified. This property enables you to modify parameters but only under certain conditions.
column name
column unit
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Within a given column, you can change the units.
Units can be specified in cells. No unit = SI
Note that it is highly recommended to choose the General format and not the Cells format in Excel.
The Tabulated Text File Format
Here is an example of a tabulated file format. You can use your favorite text editor to create this design table. Use the Tab key to skip from one column to the other. Unit rules are the same as for the Excel sheets.
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Under UNIX, it is possible to change the default design table editor. To do so, type: export CATTextEditorDT=... (indicate the path of the editor.)
The CATIA Design Table
Once it has been read and processed by CATIA, the design table looks something like this: No units in column Check box to modify the activity
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Displays the design table raw Values with units data.
Duplicates the design table external data into the CATIA document. Check this box whenever you intend to re-access your design table on another platform.
Design Tables Status:
Design tables can have different statuses: Synchronized: The Design Table is copied into the model ("Duplicate data in CATIA model" option checked) and the data stored in the model are synchronized with the content of the file. Not synchronized: The Design Table is copied into the model ("Duplicate data in CATIA model" option checked) and the data stored in the model are synchronized with the content of the file. (The .xls or .txt file was modified outside CATIA.) Inactive: The Design Table is deactivated. The associated parameters are not driven by the design table any longer. Broken: The Design Table is functionally KO because it cannot be used to valuate the associated parameters (data cannot be accessed because the file is lost or there are 2 columns with the same name ...). Light Broken: The filter is not compatible with the current configuration, or if the current configuration value does not correspond to one of the rows of the file.
Getting Familiar with the Design Table Dialog Box
Here is the dialog box sequence you get onscreen when you click the standard toolbar. icon in the
Creation of a design table
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"Create a design table from a pre-existing file" check box Check this option whenever you want to create a design table from the values of an external file. In this case, the created design table is made up of: • either only the columns whose name is a document parameter name. If the external file contains a "Length" column but no such "Length" parameter is defined in the document, the "Length" column will not appear in the created design table. This is the "automatic" association process. • or only the columns that have been associated one-by-one with a document parameter. If the external file contains a "Length" column but no so-called parameter in the document, you can choose to associate the "Length" column of the external with a parameter of the same type (a sketch radius for example).
"Create a design table with current parameter values" check box Check this option whenever you want to create a design table from a subset of the document parameters. You just have to select among all the document parameters the ones you want to be included as columns in the design table. In this case, the created design table only contains a single row. The Orientation check boxes These options allow you to choose the design table orientation. A vertical orientation is recommended when the design table contains many parameters.
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User Tasks The sheet index You can specify an Excel or Lotus sheet number. The Destination field All knowledgeware relations such as design tables, rules, checks or formulas, are created by default below the Relations node. Creating a relation below a given feature may help you organize your document. To specify a destination, select the default destination in the Destination field, then click the feature intended to be the new destination either in the specification tree or in the geometry area.
Selection of the parameters to insert
This dialog box pops up when you check the "Create a design table with current parameter values" check box.
There are two ways to restrict the list of parameters to be displayed in the 'Parameters to insert' list. You can use the: 1. Filter Name field Use the * character to specify any string to be included in a parameter name. Specifying *Len* will display in the "Parameters to insert" part of the dialog box all the parameters having the Len substring in their name. 2. and the Filter Type field. When you click OK in the dialog box above, the "Select the pathname of the file to be created" window is displayed.
Selection of the file to be created
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Use this dialog box to specify the .xls (Windows) or .txt file to be created. Specify the .xls extension when filling out the 'File name' field. Then click Open to display the design table dialog box. When working in a french environment, make sure that the decimal numbers contained in the text file linked to the design table are not written with a comma "," but with a decimal point. (This way you will be able to move to an english environment easily.)
Design table dialog box
The 'Configurations' tab
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User Tasks The current configuration as well as its number (< configuration number >) are highlighted. To change the current configuration, you just have to click the new configuration in the design table. A single row design table is created when you generate a design table with the current parameter values. • The Filter The filter is a means to help you query for a configuration meeting specific criteria. Click the "Edit... " button to display the "Design Table Request Editor". See Using the Dictionary for information on how to use the syntax provided by the dictionary. In a query, you can specify a condition referring to the design table parameters as well as the parameters external to the design table. • The "Activity" check box A design table is created active by default. The activity check box provides you with a way to deactivate the design table to be created. The "Edit table..." push button Click this button to display the edit table to be created. Depending on whether you have selected a .xls extension or not, you will launch a Microsoft Excel application or your default text editor for a .txt file. The "Duplicate data in CATIA model" check box Check this box whenever you intend to reuse your document on an operating system different from the one used to create the design table. That way, your design table data will be duplicated into your document.
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The "Associations" tab
This tab provides you with a way to associate the document parameters with the columns of the external design table. The left part of the dialog box allows you to associate parameters with the design table columns while the right part displays the list of associated parameters.
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The "Create parameters..." push button When a parameter is referred to in the design table but has not been created in the document, clicking this button allows you to create a parameter in the document and associate it with the right column of the design table. The "Rename associated parameters" push button If a parameter does not have the same name as the column it is associated with, you can rename this parameter so that it has the same name as the column. Clicking the "Rename associated parameters" push button displays a dialog box which asks you whether you want to rename all the parameters or only a few of them.
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Creating a Design Table from the Current Parameters Values
A design table is a feature that you create from your document parameters or from external data. No matter the existence of external data, you must create the design table in CATIA. There are two ways to create a design table: • • From the current parameter values From a pre-existing file.
The scenario described below explains how to proceed in the first case. The design table creation process includes the following steps:
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a. Create a table from the document parameters. b. Select the parameters to add to the design table. c. Specify a file to contain the generated design table. d. Edit the generated CATIA design table. e. Apply the design table to your document. For information on how to use the different dialog boxes related to the design table, see The Design Table Dialog. 1. Open the KwrStartDocument.CATPart document. 2. Click the Design Table icon in the standard toolbar. The Creation of a Design Table dialog box is displayed. See The Design Table Dialog for further information. 3. If need be replace the default name and comment for the design table. 4. Check the Create a design table with current parameter values option. 5. Click OK. The Select parameters to insert dialog box is displayed. 6. In the Parameters to insert list, select the PartBody Pad.1 FirstLimit Length and the
PartBody Pad.1 SecondLimit Length items. Then click the right arrow to add both items to the Inserted parameters list. 7. Click OK. A file selection box is displayed. 8. Specify the pathname of the design table to be created. Click OK in the file selection dialog box. The design table feature is added to the specification tree and a dialog box displays the newly created design table. This design table contains only one configuration. By default it is active. If the file specified already exists, the Creation of a Design Table dialog box is re-displayed as well as a message box asking you whether you want to overwrite the existing file. 9. Click Edit table... to start an Excel application (under Windows) or open the text editor under Unix. Replace the PartBody value with 80mm. Pad.1 FirstLimit Length parameter
10. Save your Excel or .txt file and close your application. Some information messages are displayed in a dialog box warning you about events related to the design table. Click Close. 11. Click Apply into the CATIA design table dialog, the document is updated as well as the CATIA design table. Click OK to exit the dialog and add the design table to the document.
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Creating a Design Table from a Pre-existing File
A design table is a feature that you create using your document parameters or external data. No matter the existence of external data, the design table must created in CATIA. There are two ways to create a design table: • • Using the current parameter values Using a pre-existing file
The scenario below describes how to proceed in the second case. Here are the main steps to follow: a. Select the pre-existing file containing the raw data. b. Create the associations between the document parameters and the external table columns. You can choose to create these associations automatically. c. Edit the generated CATIA design table. d. Select a configuration in the generated design table. You can modify the default configuration proposed by CATIA. e. Apply the design table feature to your document. For information on how to use the different dialog boxes related to the design table, see The Design Table Dialog. It is now possible to select a Design Table external file from a VPDM (ENOVIA LCA, ...). To do so, make sure you have enabled the desired environment in the Document Environments field (Tools->Options>General->Document.) Your documents will be accessible via the Document Chooser. 1. Open the KwrStartDocument.CATPart document. 2. Click the Design Table icon ( ) in the standard toolbar. The Creation of a Design Table dialog box is displayed. Enter a name (DesignTable1 for example) and a comment. 3. Check the Create a design table from a pre-existing file option. Click OK. 4. Select the KwrBallBearing.xls file, and click Open. A dialog box asks you whether you want to perform automatic associations between the design table columns and the document parameters which have the same name. 5. Click Yes. The Material parameter is the only one which is common to the document parameters and to the external design table. A multi-row design table is created. The '<' and '>' symbols denote the current configuration. 6. Select the configuration you want to apply to the document (line 4 for
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example). Click Apply. The Iron parameter value is displayed in the specification tree. 7. Click OK to end the design table creation.
The scenario below illustrates how to create a design table by associating one by one the document parameters with the input file columns. 1. Open the KwrStartDocument.CATPart document. Design Table icon in the standard toolbar. 2. Click the The "Creation of a Design Table" dialog box is displayed. Enter a name (DesignTable2 for example) and a comment. 3. Check the Create a design table from a pre-existing file option. Click OK. A file selection window is displayed. 4. Select the KwrBallBearing.xls file. Click Open. The Automatic associations dialog box is displayed. 5. Click No. The design table dialog box informs you that there is no associations between parameters and columns. Now, you have to associate one by one the document parameters with the design table columns. 6. Click the Associations option. The table design dialog box now displays side by side the document parameter list and the input file columns. 7. In the Parameters list, select the PartBody Hole.1 Diameter item. In the Columns list, select the d1 parameter. Then click Associate. A parameter couple is now displayed in the Associations between parameters and columns list. 8. Repeat the same operation for the Material parameter. Selecting a parameter or an association in the list highlights the corresponding values in the geometry area. The parameter list can be filtered: o By clicking on a feature (either in the specification tree or in the geometry area). All the parameter values of the selected feature (and children) are highlighted in the geometry area. The parameter list displays only the parameters of the selected features (and children). By specifying a string in the Filter Name field. For example, typing *ength* enables you to display all Length parameters By specifying a type in the Filter Type field.
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The Create parameters... button allows you to create automatically parameters and associations for items of the Columns list. The Rename associated parameters button replaces the parameter name with the
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column name. 9. Click OK to end the DesignTable2 creation dialog. The DesignTable2 feature is added as a relation to the specification tree. Double-click DesignTable2 in the specification to edit the table. By default, the configuration 1 is applied to the document. A new material (Aluminum) is applied to the document and the hole diameter is modified.You can select another configuration and apply it to your document.
Interactively Adding a Row To a Design Table External File
The task described below explains how to add a row to a design table external file. The scenario is divided into the following steps: • • • • You open the CATPart file and inserts the design table You deactivate the design table and creates a new configuration You add the configuration to the design table external file You activate the design table and implements the new configuration
This new function enables you to add a contextual menu on design table feature (in the tree) which appears only: • • • If the design table is deactivated If the design table external file exists and is read/write If at least one parameter is associated.
The behavior of this command is to add a row at the end of the design table file with associated parameters values. For not associated columns, an empty cell is added. To perform this scenario, you will need the following files: KwrAddARow.CATPart KwrAddARow.xls Note that this task can only be performed in an english environment.
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Prior to performing this scenario, make sure the With value and With formula options are checked in the Tools->Options->General->Parameters and Measure->Knowledge tab. 1. Open the KwrAddARow.CATPart file. The following image is displayed.
2. Click the Design Table icon (
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3. Click the Create a design table from a pre-existing file radio button and click OK. 4. In the opening File Selection window, select the KwrAddARow.xls file and click Open. 5. Click Yes in the Automatic associations window: The design table opens. Click OK to close it. 6. Click the Measure update icon to update Formula.1. 7. Under the Design Tables node, double-click Configuration=1. The Edit Parameter dialog box is displayed. 8. Click the Design table icon in the Edit Parameter dialog box: The Design Table window is displayed. 9. In the dialog box, select the second configuration (line 2), click Apply, and OK twice. 10. Right-click Formula.1 in the specification tree and select the Local Update command. 11. In the Specification tree, right-click DesignTable.1 and select the DesignTable.1 object->Deactivate command. The design table is deactivated. 12. Modify the spline: • Double-click Point.1 twice in the specification tree or in the Geometry. Enter the coordinates indicated below into the Point Definition dialog box.
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Modify the coordinates of X Point.2 and Point.3 (see Y table Z opposite) Click OK when done.
Point 1 0 0 0
Point 2 100 100 -100
Point 3 50 50 -226
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13. Add the new configuration to the design table. To do so, right-click DesignTable.1 in the specification tree and select the DesignTable.1 object>Add row with current values command.
14. Right-click DesignTable.1 and select the DesignTable.1 object->Activate command. 15. Double-click Configuration=1 under DesignTable.1 and click the Design Table icon ( ).
16. In the DesignTable.1 window select the configuration that you have just added and click Apply and OK twice. The spline is updated accordingly.
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Controlling Design Tables Synchronization
This topic aims at providing you with short examples when working with design tables in the following modes: • • • Automatic Synchronization At Load Interactive Synchronization At Load Manual Synchronization
Automatic Synchronization At Load
When loading a model containing user design tables, if the design table files have been modified and the external file data is contained in the model, the design table will be synchronized automatically if this radio button is checked. 1. Open the KwrBallBearing1.CATPart file. The following image is displayed.
2. Click the Design Table icon ( is displayed.
). The Creation of a Design Table dialog box
3. Click the Create a design table from a pre-existing file option and click OK. The File Selection dialog box opens. 4. Select the KwrBearingDesignTable.xls file and click Open. Click Yes when prompted to associate the columns of the tables with the parameters. 5. Click OK to apply the default configuration. 6. Save your file and close it. 7. Open the KwrBearingDesignTable.xls file. Change the material of row 2 to Gold. Save your file and close it. 8. Go back to Catia. Open the part: The Part is updated accordingly to your changes.
Interactive Synchronization At Load
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When loading a model containing user design tables whose external source file was deleted, this option enables you to select a new source file or to save the data contained in the design tables in a new file. 1. From the Tools->Options... menu, select General->Parameters and Measure and check the Interactive Synchronization At Load option in the Knowledge tab. 2. Open the KwrBallBearing1.CATPart file. The following image is displayed.
3. Click the Design Table icon ( is displayed.
). The Creation of a Design Table dialog box
4. Click the Create a design table from a pre-existing file option and click OK. The File Selection dialog box opens. 5. Select the KwrBearingDesignTable.xls file and click Open. Click Yes when asked if you want to associate the columns of the tables with the parameters. 6. Click OK to apply the default configuration. 7. Save your file and close it. 8. Go to the directory containing the KwrBearingDesignTable.xls file and delete it. 9. Go back to Catia. Open the KwrBallBearing1.CATPart file: A dialog box is displayed asking you if you want to select a new file. Click the Select button and select a new Excel file.
Manual Synchronization
When loading a model containing user design tables, if the design table files have been modified and the external file data is contained in the model, the design table will be synchronized if this option is checked. To synchronize both files, right-click the design table in the specification tree and select the DesignTable object->Synchronize command or the Edit->Links command. 1. From the Tools->Options... menu, select General->Parameters and Measure and check the Manual Synchronization At Load in the Knowledge tab. 2. Open the KwrBallBearing2.CATPart file. This file already contains a design table whose values are identical to those contained in the
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KwrBearingDesignTable.xls file (Note that the KwrBearingDesignTable.xls file and the KwrBallBearing2.CATPart file should be located in the same directory.)
3. Select the Edit->Links command to edit the Excel file path and select the appropriate KwrBearingDesignTable.xls file. Save the file and close it. 4. Open the KwrBearingDesignTable.xls file and modify the material values for example. Close the file. 5. Go back to CATIA. Open the KwrBallBearing2.CATPart file. 6. Select the Edit->Links command and click the Synchronize button to synchronize both files. If the Duplicate data in CATIA model option is checked, and if you choose another design table file without using the Edit Table command in the CATIA session, the following message is displayed whatever the settings:
If the Duplicate data in CATIA model option is unchecked, the synchronization occurs automatically.
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Storing a Design Table in a Power Copy
This task shows how to store a design table in a power copy for later use. In this scenario, you want to instantiate the inner and the outer cages of a ball bearing in a different context. To do so, you create a power copy only containing the outer and the inner cages of an already existing ball bearing. This scenario is divided into the following steps: • Inserting the Design Table into the CATPart file • • Creating the Power Copy Instantiating the Power Copy containing the Design Table
To perform this scenario, the Product Knowledge Template license is required. To perform this scenario, you will need the following files: • • KwrBallBearing1.CATPart KwrBearingDesignTable.xls
To store a design table in a Power Copy, do not forget to select the parameters pointed by the design table. 1. Open the KwrBallBearing1.CATPart file. The following image is displayed.
Inserting the Design Table into the CATPart file
2. Click the Design Table icon ( ) in the Standard toolbar. The Creation of a Design Table dialog box is displayed. 3. Check the Create a design table from a pre-existing file radio button and
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click OK. The File Selection dialog box is displayed. 4. Select the KwrBearingDesignTable.xls and click Open. 5. Click Yes when asked for automatic associations and click OK. The Design table is displayed below the Relations node.
Creating the Power Copy
6. From the Start->Knowledgeware menu, access the Product Knowledge Template workbench (if need be) and click the Create a PowerCopy icon. The Power Copy Definition dialog box is displayed. 7. In the Specification tree, select the following items: o o o o o o o o o DesignTable.1 Shaft.1 Shaft.2 Shaft.3 Sketch.1 Sketch.2 Sketch.3 the Material Parameter. Click OK when done. The Power Copy is displayed below the PowerCopy node in the specification tree.
8. Save your file and close it.
Instantiating the Power Copy
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9. From the File->New menu, select Part in the List of Types and click OK. 10. If need be, from the Start->Knowledgeware menu, access the Product Knowledge Template workbench and click the Instantiate From Document icon. The File Selection dialog box is displayed. 11. Select the KwrBallBearing1.CATPart file and click Open. The Insert Object dialog box is displayed. 12. Select the yz plane in the specification tree and click OK. The Design Table is instantiated
Creating and Using a Knowledge Advisor Law
The scenario which is developed below illustrates how to create a Knowledge Advisor law, then use a combination of a Generative Shape Design law and a Knowledge Advisor law in the same relation. • The Evaluate method is to be used to calculate a parameter value when this parameter is defined by a Generative Shape Design law. Note that the result you obtain on completion of this task depends on the initial lines. You can replay the scenario with different lines and see how it affects the result.
•
•
•
A Knowledge Advisor law is a relation whereby a parameter is defined with respect to another. Both parameters involved in a law are called formal parameters. Formal parameters and laws are specifically designed to be used in the creation of shape design parallel curves. A Generative Shape Design law can be used in a Knowledge Advisor law. Laws only specify a relation between one parameter and another single parameter.
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1. From the Start->Shape menu, access the Generative Shape Design workbench. 2. Define a working support using the Work on Support icon ( ).
3. Select the zx plane, for example, and click OK in the updated Work on Support dialog box without modifying any other parameter. 4. Click the Line icon ( 5. ). The Line dialog box is displayed.
Right-click in the Point 1 field, and choose the Create point command.
6. The Point Definition dialog box is displayed, the Point type and Plane fields being automatically filled. 7. Create a point at H:0mm and V:0mm, and click OK.
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8. Repeat the operation, right-click the Point 2 field from the Line dialog box to create another point at H:100mm and V:0mm, then click OK in the Point Definition dialog box. 9. Click OK in the Line dialog box to create the line. icon. If need be, use the 10. Access the Knowledge Advisor workbench and click the Tools->Customize command to access the icon. A dialog box similar to the one below is displayed. This editor is similar to the other relation editors. If need be, replace the default values specified in the dialog box fields.
11. Click OK. The law editor is displayed. The right-hand part allows you to create the parameters to be used in the law. The left-hand part is the law edition box. 12. Click the New Parameter of type button to create two real type parameters FormalReal.1 and FormalReal.2, then enter the law below into the edition window: FormalReal.1 = 5*sin(5*PI*1rad*FormalReal.2)+ 10
13. Click OK to add the law to the document. The Law.1 feature is added to the specification tree right below the Relations node.
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14. Select your document root feature and re-access the Generative Shape Design workbench. icon to create a curve parallel to the line created at the very beginning of the 15. Click the scenario. The Parallel Curve Definition dialog box is displayed. 16. Select the line that you previously created as the reference Curve.
Note that only positive laws, i.e. with positive values only, can be used when creating parallel curves (positive is to be understood as "strictly positive"). 18. Click the Law ... button. The Law Definition dialog box is displayed. 19. Click the Advanced Law type, click Law.1 in the specification tree and click Close.
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20. Click OK. A curve parallel to the selected one is created, taking the law into account.
The KwrCreatingaLaw.CATPart sample illustrates this scenario.
Using the Knowledge Inspector
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The Knowledge Inspector allows you to query a design to determine and preview the results of changing any parameters without committing themselves to actually changing the design. This "what if" analysis provides immediate feedback that helps you experiment and refine designs. While it is important to determine what happens when one or more parameters are changed, it is equally significant for you to see how a design can be changed to achieve a desired result. The Knowledge Inspector supports this by allowing you to query "how to" make a particular change. In short, the Knowledge Inspector is a tool designed to study impacts and dependencies. What if (impacts) Helps you understand to what extent changing any parameter of your design (such as material, pressure, or a dimensional parameter) changes the operation or design of the product on which you are working. Can be used to examine interactions of parameters with each other and with the rules that make up the product's specifications. A "Geometric Update" option enables you to visualize the result of your modification in the geometry area. How To Helps you determine how your design can be changed to achieve a (dependencies) desired result.
You shouldn't use the
capabilities with the Knowledge Inspector.
The 'What If' Mode
This task explains how to use the 'What If' mode. 1. Open the KwrFormula1.CATPart document and access the Knowledge Advisor workbench. 2. Click the Knowledge Inspector icon or select the Knowledge Inspector from the standard tool bar. The "Knowledge Inspector" dialog box is displayed. Check the 'What If' option. 3. Select the KwrStartDocument PartBody Pad.1 this stage, don't modify its value in the Equals field). FirstLimit Length parameter (at
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4. Click Apply. The following list of parameters and parameter values is displayed in the Then area.
5. The first line describes the parameter which has just been selected. The other lines describe the impacted parameters. 6. Use the Equals field to replace the KwrStartDocument PartBody Pad.1 FirstLimit Length parameter value with 60mm. Click Apply. In the Then area, the parameter values are updated as follows:
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7. The InitialValue column shows the initial parameter values (when you open the Knowledge Inspector). The OldValue column shows the parameter values resulting from the previous 'What if' operation. The Var (variations) columns show comparison operators between values located in adjacent columns. 8. Check the Geometric Update option to display in the geometry area the modifications resulting from the 'What If' operation. Click Apply to update the document in the geometry area. 9. Click OK to apply the values resulting from the current 'What If' operation to your document. Otherwise, click Cancel>. Note that: • Using the buttons reloads in the 'Then' area the previous or next values in the history of the 'What if" operations. Checking the Show All Parameters option displays all the document parameters. An f letter in the Dvn column indicates that the parameter is constrained by a formula. Selecting a parameter in the Then area while the Show All Parameters is checked, highlights the selected parameter in the parameter list above.
•
•
Modifying a parameter value does not imply that the values of the impacted parameters are automatically updated by a 'What If' operation. For example, if a parameter is constrained by a formula such as: if Parameter1 > A then Parameter2 = B replacing the Parameter1 value with a value greater than A won't modify Parameter2 if Parameter2 was previously set to B.
The 'How To' Mode
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This task explains how to use the 'How To' mode. 1. Open the KwrFormula1.CATPart document. 2. Click the Knowledge Inspector icon in the standard toolbar. The Knowledge Inspector dialog box is displayed. Check the 'How To' option. By default, only the parameters which are constrained by a formula are displayed. 3. If need be, check the Show All Parameters to display all the document parameters. 4. Select the KwrStartDocument PartBody Hole.1 Diameter parameter (assuming that you would like to have this parameter modified). 5. Click Apply or Enter. The list of parameters to be modified in order to change the Hole.1 Diameter parameter is displayed in the 'Use' area. FirstLimit Length parameter.
6. Select the Pad.1
7. Check the What If option. 8. Modify the FirstLimit Length parameter in 'What If' mode.
9. Click OK to apply the parameter modification to your document.
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Note that: • Checking the Show All Parameters option displays all the document parameters. An f letter in the Dvn column indicates that the parameter is constrained by a formula. • Selecting a parameter in the 'Use' area while the Show All Parameters is checked, highlights the selected parameter in the parameter list above.
Working with the Rule Feature
Working with the Rule Feature
Select the Rule icon to create a rule, write its code, test its syntax and apply it to your document. A rule is a set of instructions, generally based on conditional statements, whereby the relationship between parameters is controlled. In addition, depending on the context described by the rule instructions, actions can be executed: • To set a value or a formula to parameters, including feature activity • • • To display information windows To launch Visual Basic macros stored in external files or in the V5 document. To affect points, curves and surfaces and thus allow contextual and automatic topological changes
In the specification tree, the rule is displayed as a relation that can be activated or deactivated. Like any feature, a rule can be manipulated from its contextual menu.
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knowledgewareAdvisor A rule is executed when one of its input parameters has changed or when one of its input features has changed and if you require the update of the rule. The consequence is that it is impossible for you to completely control when the rule is to be fired. As a result, rules should only manipulate parameters and features and should be used to control the status of a design (change of parameters and geometry).
If you want to control when the action takes place, you should use the Reaction feature. Creating a Rule Using the Rule Editor Using Rules and Checks in a Power Copy Using the Dictionary
Creating a Rule
The task described below explains how to create a rule which retrieves the abscissa of a point and, depending on the coordinate value, displays a message or another. This scenario uses two special functions allowing you to retrieve the coordinates of a point. These functions can be accessed from the Measures item of the Dictionary. To find out more about the Dictionary, see the Using the Dictionary. 1. Open the KwrMeasure.CATPart document. The whole document has been created using the Generative Shape Design product. The extruded surfaces are extruded from the Spline.1 and Spline.2 curves. The point whose coordinates are to be retrieved and tested is Point.5.
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2. 3. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. editor to create three Length type parameters: Point5X, Point5Y 4. Use the and Point5Z. icon. In the first dialog box which is displayed, enter a rule name 5. Click the (MeasureRule for example). If need be, replace the default comments. If you want to add the rule to be created to a specific relation set, specify a destination. To do so, see Creating Sets of Relations. 6. Click OK. The Rule Editor is displayed. 7. Enter the rule below in the edition window.
if Geometrical Set.1
Point.5.coord(1) > 0mm
Message("Point.5 abscissa is positive") else { Geometrical Set.1 Point.5.coord(Point5X, Point5Y, Point5Z)
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Message("Point.5 abscissa is: # ", Point5X) } 8. In the rule above, you can retrieve the Point.5 definition (Geometrical Set.1 Point.5) by double-clicking the feature in the specification tree. 9. Click OK. The message "Point.5 abscissa is: 0mm" is displayed. 10. Edit the Point.5 feature (double-click the object in the specification tree for example) and replace the Point.5 X value with 10 mm. The rule is in a to-beupdated status. See Updating Measures for information on relations to be updated. 11. Re-access the Knowledge Advisor workbench, then click the message box informs you that "Point.5 abscissa is positive"). icon. A
To find out more about the Rule Editor, see Using the Rule Editor.
Using Rules and Checks in a Power Copy
This task explains how to use rules and checks in a Power Copy. Rules and checks as well as other relations can be applied to a document by retrieving them from another document provided they have been stored in a power copy. For further information on the power copy mechanism, see the Generative Shape Design User's Guide.
1. Open the KwrMeasurePCopy.CATPart document. If need be, access the Generative Shape Design workbench. 2. In the standard menu bar, select the Insert->Knowledge Templates>PowerCopy... command. The Power Copy definition window is displayed. 3. In the specification tree, select the Rule.1 and Check.1 relations. Both relations are carried forward onto the Power Copy definition window. Click OK in the Power Copy creation window. Save and close your document. 4. Open the KwrSplineInPcopy1.CATPart document and access the Generative Shape Design workbench. 5. Select the Insert->Instantiate From Document... command from the standard menu bar. The Select PowerCopy dialog box is displayed. Select the document which contains the power copy storing the Rule.1 and Check.1 relations and click Open. The Insert Object dialog box is displayed. 6. Select the Spline.1 feature either in the specification tree or in the geometry area. Click OK. A message box launched by the check is displayed informing you that the Spline Length is < 100mm. Both relations are carried forward to the specification tree and the check icon is red. The rule has not been fired. 7. Open the KwrSplineInPcopy2.CATPart document and repeat the same operation (from step 5). An information box displays the Spline Length
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indicating that Rule.1 is fired. This time, the check icon is green is the specification tree.
Rules and checks can be stored in catalogs and instantiated later in a document. See Instantiating Knowledgeware Relations from a Catalog
Using the Rule Editor
The Rule Editor is intended to help you key in the check body using the Dictionary. It is made up of:
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In the Rule Editor, you can: • Restrict the list of parameters displayed in the dictionary: in the specification tree, simple click the feature you want to display the parameters. If the 'Incremental' option is selected, only the first level of parameters right below the selected feature are displayed, otherwise, all the parameters at all levels are displayed. Suppose your document contains a Geometrical Set feature which itself is made up of several Shape Design points. When the 'Incremental' box is unchecked, selecting the Geometrical Set feature in the specification will display all the parameters related to the points (the parameters which defines the coordinates are included in the list). When the 'Incremental' box is checked, selecting the Geometrical Set feature displays only the first level of parameters below the Geometrical Set (the point coordinates are not displayed). Insert the feature definition in a rule: in the specification tree, double click the feature you want to insert the definition. Check whether the rule syntax is correct: click Apply. Erase the contents of the edition window: click the Add the rule to the document: click OK. To find out more about the items displayed in the Dictionary, see Using the Dictionary or select one of the items and press the F1 key in Catia. To find out more about rules, see Creating a Rule. icon.
• • • •
Handling Errors
This task explains how to handle features that are in error. In the scenario described below, you are going to open a .CATPart file that is made up of 2 lines and a datum point. This point will be the intersection of the lines if they intersect, or the origin if they do not. To do so, you are going to create a rule. The use of geometrical operators to value geometry in relations may lead to update errors in the created features. If you value a datum point with the result of the intersection of 2 lines, these 2 lines may not intersect and the point is therefore in error. The Do not catch evaluation errors option which is available by selecting the relation in the specification tree and selecting the Properties command enables you: • • • To create features in error To know (through an error message) if a feature is in error and To make changes (or not) in case of errors.
Note that this error handling is only available for GSD features.
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1. Open the KwrErrorHandling.CATPart file. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. ) to create a rule that will react to the fact that the 3. Click the Rule icon ( datum point is the intersection of the 2 lines if they intersect or the origin if they do not. 4. In the Rule Editor, enter the following body: let x(Point) x =intersect(`Geometrical Set.1 Set.1 Line.2` ) if (x.Error==true) `Geometrical Set.1 else `Geometrical Set.1 Note that Japanese users should enter the following rule body: Point.5` = point(0mm,0mm,0mm) Point.5` = x Line.1` ,`Geometrical
5. Click OK when done. The intersect operator launches an error message if the intersection is empty.
6. Right-click the rule in the specification tree and select the Properties command. 7. Check the Do not catch evaluation errors check box and click OK when done. This way, the evaluation of the rule will be forced even if an update error occurs.
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Working with the Check Feature
Working with the Check Feature
Select the Check icon to create a check, write its code, tests its syntax and apply it to your document. A check is a set of statements intended to inform you if certain conditions are fulfilled or not. A check does not modify the document it is applied to. A check is a feature. In the document specification tree, it is displayed as a relation that can be activated and deactivated. Like any feature, a check can be manipulated from its contextual menu. Creating a Check Using the Check Editor Performing a Global Analysis of Checks Using the Check Analysis Tool Using Rules and Checks in a Power Copy Customizing Check Reports Using the Dictionary
Creating a Check
This task explains how to create a check.
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1. Open the KwrFormula0.CATPart document, select the root item in the specification tree and access the Knowledge Advisor workbench. 2. Click the Check icon . The first Check Editor dialog box is displayed.
3. Replace the default name with Cylinder_Check. If needed, add some comments to the Description field. If you want to add the check to be created to a specific relation set, specify a destination. To do so, see Creating Sets of Relations. By default, the check is created right below the Relations node. 4. Click OK. The Check Editor is displayed.
5. Select a type of check. Enter the message you want to be displayed in the information or warning box in case the check is not verified. 6. Enter the check statements in the edition window. You can simply Copy/Paste the following statements into the edition window:
Relations
Formula.1
Activity == false
7. Click Apply to test your check syntax. If the information message is displayed, the check syntax is correct. 8. Click OK to add Cylinder_Check to the relations node in the specification tree. A red icon is displayed in the specification tree meaning that the check is not valid. 9. Deactivate Formula.1, the check icon turns to green in the specification tree. Three parameters related to a check are displayed in the "Formulas" dialog box: • • • The activity The severity The result
When you select the result parameter, the icon indicating whether the check is valid or not is displayed opposite the value field. Double-clicking this icon opens the check editor. To find out more about the Check Editor, see Using the Check Editor.
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To find out more about the Check Editor, see Using the Check Editor.
Performing a Global Analysis of Checks
Performing a Global Analysis of Checks
This task explains how to perform an analysis of Knowledge Expert and Knowledge Advisor Checks. The scenario is divided into 2 major steps: • • parameters, formulas and checks are created, the checks analysis is run and the checks that failed are corrected.
To find out more about the Global Analysis tool and the Check Report, see Using the Check Analysis Tool and Customizing Check Reports. • For the check report to be correctly generated, go to Tools->Options->General>Parameters and Measure ->Report Generation, and select: - The Input XSL file under Input XSL. (An XSL file is provided by default. Click here to get a description of the generated XML file.) - The parameters you want to appear in the report under Report Content. - The Output directory under Output Directory. 1. Open the KwrCheckAnalysis.CATPart file. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 2. Create a parameter of Length type and assign it a formula. Click the icon. The formula editor opens.
o o
Select Length in the scrolling list to define the type of the parameter, click the New parameter of type button, change the name of the parameter (Length in this scenario), and click the Add Formula button. The Formula Editor opens.
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o
Under Dictionary, select Measures, and doubleclick distance(Body,Body). Position the cursor before the coma and double-click Point.1 in the specification tree or in the geometrical area. Position the cursor after the coma and doubleclick Point.2 in the specification tree. Click OK.
3. Create a parameter of Volume type and assign it a formula. o Click the o icon. The formula editor opens.
Select Volume in the scrolling list to define the type of the parameter, click the New parameter of type button, change the name of the parameter (Volume in this scenario), and click the Add formula button. Under Dictionary, select Part Measures, and double-click smartVolume. Position the cursor between the parentheses and select PartBody in the specification tree. Click OK.
o
The parameters and the associated formulas are created
), change the 4. Access the Knowledge Advisor workbench, click the Check icon ( name of the check (Length in this scenario), and click OK. The Check Editor opens. 5. Enter the following script in the editor, then click Apply and OK. Length > 150mm
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The Knowledge Advisor Check is created.
6. Access the Knowledge Expert workbench, click the Expert Check icon, and change the name of the check (HoleCheck in this scenario). The Expert Rule Editor opens. 7. In the Condition tab, enter the following script: H:Hole Editor H.Diameter > 15mm
8. Click the Correction tab, select VB Script in the scrolling list and enter the following script in the editor: Dim aHole as Hole Set aHole = H.parent.Item(H.Name) Dim diam As Length Set diam = aHole.Diameter diam.Value = 16 MsgBox("Correction performed on "&H.Name) 9. In the Correction Comment field of the Correction tab, enter the following string, and click OK: Holes diameter should be greater than 15mm. 10. Select the Rule Base under the Relations node and click the Expert Check icon, change the name of the check (DraftandHole in this scenario), and click OK. The Expert Check Editor opens. 11. In the Condition tab, enter the following script, then click Apply and OK. H:Hole ; D:Draft Editor D.Activity AND H.Diameter > 12mm
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The checks are created (click the graphic opposite to enlarge it).
12. Click the
icon in the toolbar. The Global Analysis Tool opens.
13. Click the icon to update the status of the checks. The Checks lights turn to red in the specification tree. icon. An xml page opens indicating the items that failed. To find out 14. Click the more about this report, see Customizing Check Reports. icon to launch the correction method specified when creating the Expert 15. Click the check (See step 9). The checks have been corrected. Only the Advisor check (Length) could not be corrected: The value of the Length parameter is 100.175 mm (as indicated in the report) whereas it should be superior to 150mm (as indicated in the body of the check). 16. To correct the check, modify the value of the Length parameter. • • Double-click Point.1 in the geometrical area. The Point definition window opens. In the H: field, change the value of the point to 150mm. Click OK. The light of the check turns to green indicating that the check is passed.
Using the Check Analysis Tool
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knowledgewareAdvisor The Global Analysis Tool is designed to manage Expert and Advisor checks wherever they may be located in the specification tree. It helps you understand the validation status of your design and allows navigation by checks or violations and highlights failed components. You can: • Access information concerning failing items • • Gather information concerning objects and checks Perform automatic corrections if need be.
The Global Analysis tool can be accessed at the session level by clicking the icon in the toolbar. This icon provides you with a simple Checks status: All the checks are updated and could be fired successfully. The checks need to be updated. All the checks are updated and at least one of them is incorrect.
Check Analysis Tool Window
Click the
icon in the toolbar to access the Check analysis window.
Filter section This option enables you to apply a filter to the checks or to the items that failed.
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Check
Only the Expert and Advisor checks that failed when updating the check report are displayed.
Failure
All the items that failed when updating the check report are displayed.
Help section To display the help section associated with each item of the list, double-click the desired item. The following view is displayed: The check and the items that it controls are displayed in the view as well as its current status. The items entered when creating the check are displayed: • Associated comments • • • • • Type Attributes Variables Name Owner of the check...
In the graphic above, the selected check is TestHole, it checks the holes of the CATPart file (3 of them do not pass the check because their diameters is not superior to 15mm), and the attributes are displayed corresponding to the data entered when creating the check.
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Note that it is also possible to select the items associated with the check. To do so, double-click the desired item in the view: The Help section shows the information concerning this item (see graphic opposite.)
Toolbar Click this icon to generate the customizable check report. To find out more about the check report, see Customizing Check Reports. Click this icon to solve the checks created in your document. Click this icon to launch the correction method specified in the Check Editor when creating the check. For an example, see Performing a Global Analysis of Checks. Click here to display the URL associated with the object, or to assign an URL to an object. To know more, see Associating URLs and Comments with Parameters or Relations.
Introducing the Default Check Report
The default check report presents the Expert and Advisor checks that failed. This window lists the checks that failed and presents a percentage of the failed items per Expert Check.
Advisor Checks report
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The Advisor checks window lists the Advisor checks that failed and shows the following elements: - the body of the check (Length>150mm here) - the item(s) on which the check operates (here, the Length formula).
Expert Checks report
The Advisor checks window lists the Expert checks that failed and shows the following elements: - the Input items checked by the check operation. - the item(s) that failed (here Hole.1, Hole.2, and Hole.3).
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Remember that this report should not be used to generate macros or other files. It is provided as information only.
Customizing Check Reports
The reports generated by the Global Check Analysis Editor can be customized. You can choose to display a xml or a html report.
Displaying a HTML report
To generate a html report when performing the check analysis, go to Tools>Options->General->Parameters and Measure and select the Report generation tab. Select Html in the Select Configuration of the check report area. In this case, only the Check Advisor, the Check expert and the Passed objects options are available in the Report content area. You can specify the output directory containing the generated HTML report in the Select output directory field. Select Html if you use a Netscape browser.
Displaying a XML report
To display a XML report when performing the check analysis, go to Tools->Options>General->Parameters and Measure and select the Report generation tab. Select Xml in the Select Configuration of the Check Report area. The following window opens:
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The Report generation tab is made up of 4 different fields: The Input XSL, the Report Content, the Select output directory, and the HTML options fields. Input XSL field This field enables you to select the XSL style sheet that will be applied to the generated XML report. The StyleSheet.xsl file is the default XSL file, but you can use your own template. Report content field Failed Checks All Checks Check advisor If checked, the generated report will contain information about the failed checks only. If checked, the generated report will contain information about all the checks contained in the document. If checked, the generated report will contain information about all the Knowledge Advisor checks contained in the document. Parameters information Check expert If checked, the generated report will contain information about the parameters of the Advisor checks. If checked, the generated report will contain information about all the Knowledge Expert checks contained in the document. Passed objects If checked, the generated report will contain information about the objects that passed the Expert checks as well
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as information about the parameters of these objects (diameter, depth, pitch,...). Objects information If checked, the generated report will contain information about all the objects contained in the Expert checks as well as information about the parameters of these objects (diameter, depth, pitch,...).
Output directory field This field enables you to select the output directory containing the generated XML report. HTML options field This option is available for Windows only. It enables you to define if the report will be opened in a CATIA session (in this case, the check box should be checked) or if it will be opened in an Internet Explorer session (in this case, the check box should remain unchecked.) Note that it is highly recommended not to use this report as a basis for macros or for other applications. It is only provided for information purposes.
Using the Check Editor
The Check Editor is intended to help you enter the check body using the Dictionary. It is made up of 3 different areas:
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Three different types of checks can be used: • • • The silent checks The information checks The warning checks
Depending on the type of check and the result of the check, you will be warned as follows: Check verified Relation icon in the specification tree Silent check Information check Warning check Check not verified
no message displayed no message displayed
no message displayed
no message displayed the message specified at check creation is displayed in an information box the message specified at check creation is displayed in a warning box.
In the Check Editor, you can: • Restrict the list of parameters displayed in the dictionary: To do so, go to the specification tree, simple click the feature you want to display the parameters for. If the 'Incremental' option is selected, only the first level of parameters located right below the selected feature are displayed. If not, all the parameters at all levels are displayed. Insert the feature definition in a check: To do so, go to the specification tree, and double-click the feature you want to insert the definition for. Check whether the check syntax is correct by clicking Apply. Erase the contents of the edition window by clicking the Add the check to the document by clicking OK. To find out more about the Dictionary, see Using the Dictionary. To find out more about checks, see Creating a Check. icon.
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Using the Action Feature
This task explains how to use an action.
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The scenario described below is made up of 3 major steps: • You first create a pad containing an action. • • You store this action in a catalog You then import the action stored in the catalog into another CATPart product.
It is highly recommended to be familiar with the Part Design workbench to perform this scenario. 1. Access the Part Design workbench and create a Pad or open the KwrAction.CATPart file. 2. Create a parameter of volume type and assign it a formula. Click the icon, select Volume in the scrolling list, click the New Parameter of type button and rename the Parameter (V in this scenario).
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Click the Add formula button. The formula editor opens. Under Dictionary, select Part Measures, and double-click smartVolume. Position the cursor between the parentheses and select PartBody. Click OK, Yes (when prompted for an automatic update) and OK.
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) to 3. Access the Knowledge Advisor workbench and click the Action icon ( create an action. The Action editor opens. Enter the following script and click OK: Inputs B: Body field Editor B.Query("Pad","").Compute("+","Solid","smartVolume(x)",V) Message("Total volume of the pads under this body : #",V) • The action created above searches for the pads contained in the selected body and computes the volume of these pads.
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• • •
To find out more about Query and Compute, click here. To see the created .CATPart file, click here. Note that the arguments types must be written in English.
4. Save your file and store the created action in a catalog. • From the Start menu, select Infrastructure->Catalog Editor. The catalog editor opens.
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), or select the Insert -> Add Family... Click the Add Family icon ( commands from the main menu to display the Component Family Definition dialog box. Indicate the name of the family (ComponentFamily.2 in this scenario), and click OK. Double-click the ComponentFamily.2 family in the catalog structure ), or select the Insert -> Add and click the Add component icon ( Component... command to display the Description Definition dialog box.
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Click the Select external feature button. Go back to the geometry, select the Action.1 feature in the specification tree and click OK. Save your catalog. The action contained in your .CATPart file is now stored in the catalog you have just created.
5. Open the KwrReceiveAction.CATPart file.
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6. Click the Catalog icon ( ) to import the action stored in the catalog. Click the Browse ), select another catalog icon your catalog, and click Open. Double-click ComponentFamily.2, and double-click Action.1. The Insert object dialog box opens. (Click the graphic opposite to enlarge it.)
7. Select PartBody: the imported action displays the volume of the pads contained in this body. (Click the graphic opposite to enlarge it.) 8. Select Body.2: the imported action displays the volume of the pads contained in this body.
Working with the Reaction Feature
Working with the Reaction Feature
Click the Reactions icon to create a script specifying how to change some feature attributes when an event occurs. The reaction is a feature that reacts to events on its source(s) by triggering an action. It is designed to cope with the rules and the behaviors limitations and to create more associative and reactive design. A reaction is a feature that reacts to events
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User Tasks The source can be: • A selected feature (or a list of features) • A parameter (result of a test) Events can be: • General events on objects (creation, deletion, update, drag and drop, attribute changes) and parameter value changes. • Insert/Replace component • Object Drag and Drop
A reaction is similar to a rule in the fact that: • It is stored in the model. • It reacts to changes and can trigger modifications. • It also references other objects and parameters in the document and supports the replace mechanism. But • • Reaction features provide a better control over when the action has to be fired. Reactions enable you to perform more complex actions. Since you have better control when the action is triggered, and as you're not constrained by the update mechanism limitations, you can use all the power of any Visual Basic API (in CATIA but also in other automation applications...), and a Visual Basic macro can be called with arguments from an action. Reactions can be written to customize the update mechanism (to optimize user features, for example). Reactions can react to user actions (instantiation of a user defined feature), insertion of a component in an assembly, modification of a parameter... Reactions can be stored in the model and can be integrated in the definition of a power copy or user feature.
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The reaction feature is not integrated to the update contrary to the rule. If a reaction is launched when updating the document, it may impact the document.
Link Bar 3
Using the Reaction Feature Window
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You can access the Reaction window by clicking the Advisor workbench.
icon in the Knowledge
The Reaction window is made up of 3 major fields: The Source Type field, the Source field and the Action field.
Source Type
• Selection enables you to manually select one or more items in the specification tree or in the geometrical area. These items will be displayed in the Sources field. Owner enables you to link the action with a feature of the geometry or of the specification tree (see Using the Knowledge Advisor Reaction Feature: DragAndDrop Event where the reaction feature is linked with a Hole, for example). To link the reaction with an object of the geometry, click the Destination field and select an object in the specification tree or in the geometry.
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Sources Field
A reaction is a feature that reacts to events (see Available events below) on an object called the source and that triggers an action. The Sources field displays the selected items with which the reaction will be linked (only available if the Selection Source type is selected.)
Available events
The events available in this scrolling list depend on the source type selected in the Source type field. The reaction will be fired when one of the events detailed below happens. Available Events AttributeModification Explanation The reaction is fired because of a change in an attribute state. Only available if the Selection option is selected.
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BeforeUpdate DragAndDrop Insert Inserted Instantiation Remove Update ValueChange
The reaction is fired before a feature is updated. The reaction is fired after a feature is dragged and dropped. The reaction is fired when a feature is inserted. The reaction is fired after a feature is inserted. The reaction is fired when a User feature is instantiated. The reaction is fired when a feature is removed. The reaction is fired right after a feature is updated. The reaction is fired because of a parameter value change. Only available if the Selection option is selected.
FileContentModification The reaction is fired each time the file associated with the design table is modified.
Action Field
The action is triggered by a reaction that reacts to events on an object. This field enables you to select the language in which you want to write the action (VB or the Knowledge Advisor language) and to edit the action.
Edit action button
Click this button to access the Action Editor.
Action Editor
The action editor displayed depends on the language selected in the Action field. If Knowledgeware action is selected, the window below is displayed.
The Edition pane enables you to enter the body of the action.
The Dictionary is divided into 2 or 3 panes depending on the selected category: - The left-hand one displays the categories that can be used in an action. - The middle one lists the
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objects belonging to the selected category. - The right-hand one displays the members of the selected category.
If VB action is selected, the window below is displayed. - The Name field enables you to enter a name for the VB script. - The Comment field enables you to enter a comment associated with the VB script. - The Editor enables you to enter the VB script. - The Insert object resolution button enables you to select an object in the specification tree or in the geometry and to automatically add its resolution to the script. (Click the graphic opposite to enlarge it.)
Creating a Reaction: DragAndDrop Event Creating a Reaction: Insert Event Creating a Reaction: Inserted Event Creating a Reaction: Remove Event Creating a Reaction: AttributeModification Event Creating a Reaction: BeforeUpdate Event Creating a Reaction: ValueChange Event Using a Reaction with a User Feature: Instantiation Event Using a Reaction with a Document Template: Instantiation Event Creating a Reaction: Update Event Creating a Reaction: File Content Modification Event
Creating a Reaction Event
Creating a Reaction: DragAndDrop Event
This task explains how to use the DragAndDrop event in a reaction feature. In the scenario below, you are going to drag and drop a hole, which fires a
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reaction. a) The following information are displayed in a VB box when the rule is fired: • The type of feature. • Its name as well as its initial diameter.
b) You are prompted to click OK to convert the hole into a counterbored one or to click Cancel to skip the conversion. Note that this task could be carried out in the past by using the Behavior feature which has been replaced with the Reaction feature. For more information about Reaction features, see Working with the Reaction Feature. 1. Create .CATPart file and a pad with a hole or open the KwrReactionPad.CATPart file. 2. Access the Knowledge Advisor workbench and click the Reaction icon ( ) to create a reaction. The reaction dialog box opens. o In the Source type field, select Owner for the Reaction to be applied to the hole selected in the Destination area (see below). In the Available events list, select DragAndDrop for the reaction to occur when the hole is dragged and dropped. In the Action field, select VB action, to write the action in VB. Click the Destination area in the Reaction dialog box and select Hole.1 in the specification tree.
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3. Click the Edit Action... button, paste the following script in the editor, and click OK twice:
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Set H = DroppedFeature.Parent.Item(DroppedFeature.Name) Dim FeatureType, FeatureName, HoleType FeatureType = TypeName(H) FeatureName = H.Name HoleType = H.Type Str1 = "The feature to be dropped" Str2 = Str1 & vbCrLf & "is a " & FeatureType & " type feature" Str3 = Str2 & vbCrLf & "Its name is '" & FeatureName & "'" Str4 = Str3 & vbCrLf & "Its initial diameter is "_ & H.Diameter.Value & vbCrLf Str5=Str4 & vbCrLf &_ "Unless you click Cancel, it will be converted into a counterbored hole" Dim MyBox MyBox = MsgBox (Str5,1) if MyBox = 1 then H.Type = 2 H.HeadDiameter.Value = 20.0 H.Diameter.Value = 10.0 End If 4. Access the Part Design workbench. In the geometry, select the hole and drag and drop it. The following dialog box appears:
5. Click OK. The hole is converted into a counterbored hole (see graphic below).
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To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: AttributeModification Event
This task explains how to use the AttributeModification event in a reaction feature. In the scenario below, you are going to create a reaction based on the activity (activated or deactivated) of a point. If the point is activated, a message box is displayed. This reaction is designed to react to attributes modification (color, state, name, thickness...). Note that attribute modification events are not available for all features. If it is the case with the feature you have selected, select the attribute in the Select a source... window and use the ValueChange event. The reaction will be launched when the attribute is modified.
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1. Open the KwrAttributeModificationEvent.CATPart file. This file contains a point that is deactivated. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( dialog box opens. ) to create a reaction. The reaction o In the Source type field, select Selection and select Point.1 in the specification tree. In the Available events scrolling list, select AttributeModification. In the AttributesLabel scrolling list, select Activity for the reaction to be launched when the point is activated or deactivated. In the Action field, select VB action and enter the following text into the editor: MsgBox "Point.1 activated" Click OK when done. The reaction is created and is displayed below the Relations node in the specification tree.
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3. Double-click Point.1 in the geometry to access the Generative Shape Design workbench. 4. Right-click Point.1 and select the Point.1 object->Activate command. A dialog box is displayed indicating that Point.1 is activated. 5. Click OK. Point.1 is activated. To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: Insert Event
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This task explains how to use the Insert event in a reaction feature. In the scenario below, you are going to insert an element into the CATProduct document, which displays a message. 1. Open the KwrSyringeAssembly.CATProduct file. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( reaction dialog box opens. ) to create a reaction. The
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In the Source type field, select Selection for the Reaction to be applied to the element you select and select the syringe in the specification tree). In the Available events list, select Insert for the reaction to occur when an item is inserted into the CATProduct. In the Action field, select Knowledgeware action and enter the following message: Message("An element was added to your document"). This message will be displayed each time you insert a new component into the CATProduct. Click OK. A reaction is added to the Relations node in the specification
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3. Double-click the root of the specification tree, select the Insert->Existing Component... command and click the root of the specification tree. The File selection dialog box opens. 4. Select the KwrSyringePiston.CATPart file and click Open. 5. The new element is inserted and the reaction is fired. The following message is displayed:
To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: Inserted Event
This task explains how to use the Inserted event in a reaction feature. In the scenario below, you are going to insert an element into the CATProduct document, which displays a message.
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1. Create a CATProduct file called Container.CATProduct and insert the KwrSyringeContainer.CATPart file by using the Insert->Existing Component... command. Save your file and close it. 2. Create a CATProduct file called Plunger.CATProduct, rename the root of the specification tree to Plunger, and insert the KwrSyringePiston.CATPart file by using the Insert->Existing Component... command. Close the file. 3. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( dialog box opens. ) to create a reaction. The reaction
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In the Source type field, select Selection for the Reaction to be applied to the element you select (plunger in this example). In the Available events list, select Inserted if you want the action to be launched when the Plunger is inserted into the CATProduct. In the Action field, select Knowledgeware action and enter the following message: Message("Plunger inserted"). This message will be displayed after the plunger is inserted. Click OK. A reaction is added to the Relations node in the specification tree. Save the file and close it.
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4. Save the file and close it. 5. Open the Container.CATProduct file, select the Insert->Existing Component... command. The File Selection dialog box opens. Select the Plunger.CATProduct file and click Open. The message specified step 3 is
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displayed.
To find out more about the Reaction feature window, see Using the Reaction Feature Window.
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Creating a Reaction: Remove Event
This task explains how to use the Remove event in a reaction feature. In the scenario below, you are going to remove an element from the CATProduct document, which displays a message. 1. Open the KwrSyringeAssembly2.CATProduct file. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( dialog box opens. ) to create a reaction. The reaction
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In the Source type field, select Selection for the Reaction to be applied to the element you select (Syringe in this example). In the Available events list, select Remove for the reaction to occur after an item is removed from the CATProduct. In the Action field, select Knowledgewar e action and enter the following message: Message("An element was removed from your document"): This message will be displayed when you remove a component from the CATProduct. Click OK. A reaction is added to the Relations node in the
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3. Double-click the root of the specification tree, right-click the Syringe piston in the specification tree, and select Delete. The following message is displayed.
To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: ValueChange Event
This task explains how to use the ValueChange event associated with the reaction feature. The CATPart file contains a cable going through 3 points. You want the cable length to be optimized each time you modify the cable length. The scenario is divided into 3 parts: • • • you create an optimization you create a reaction you modify the cable length value
1. Open the KwrEventValueChange.CATPart file: It contains 3 points and a
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spline (called cable in this scenario).
2. From the Start->Knowledgeware menu, access the Product Engineering Optimizer workbench and click the Optimize icon ( window opens. 3. Enter the following data in the Optimization window: Problem tab Optimization type Optimized parameter Free parameters Minimization distance Geometrical Set.1 Algorithm Termination criteria Point.3 Z ). The Optimization
Simulated AnnealingConvergence speed Maximum number of updates: 100 Consecutive updates without improvements: 20 Maximum time (minutes): 5
Constraints tab New constraint `Geometrical Set.1 Point.3 Z` - max (Geometrical Set.1 Point.2 ,Geometrical Set.1 Point.1 <= 0mm 4. Click OK in the opening dialog box, click Run optimization. Z Z)
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5. Select an output file and click Save. 6. Click OK once the optimization process is over. 7. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( ). The Reaction dialog box opens. • In the Source type field, select Selection and select the CableLength parameter in the specification tree for the Reaction to be applied to the CableLength parameter. In the Available events list, select ValueChange. In the Action field, select VB action.
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8. Click the Edit action... button, paste the following script in the editor, and click OK twice: Dim partDocument1 As Document Set partDocument1 = CATIA.ActiveDocument Dim part1 As Part Set part1 = partDocument1.Part Dim relations1 As Relations Set relations1 = part1.Relations Dim optimizations1 As Optimizations Set optimizations1 = relations1.Optimizations Dim anyObject1 As Optimization Set anyObject1 = optimizations1.Item("Optimization.1") anyObject1.Run False
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The reaction is added to the specification tree.
9. Double-click twice the CableLength=400mm parameter and change its value to 600mm: The optimization is launched (the RealLength and the distance parameters have changed) and the geometry is changed accordingly. To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: BeforeUpdate Event
This task explains how to use the BeforeUpdate event in a reaction feature. In the scenario below, you are going to optimize the position of a point each time you modify the length of the cable (spline). You create your geometry and insert all the components in a User Feature (UDF). This UDF contains the geometry of a cable going through 3 points: • The two points located at both extremities are to be specified in input. The coordinate of the third point is optimized in order to reach a target length for the cable.
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This target parameter is a published parameter of the UDF. The optimization is launched by using a VBMacro with argument, called in a Reaction to the "Before Update" event of the UDF. This scenario requires the Product Engineering Optimizer product.
1. Open the KwrEvent_BeforeUpdate.CATPart file: It contains 3 points and a spline (called cable in this scenario).
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2. From the Start->Knowledgeware menu, access the Product Engineering Optimizer workbench and click the Optimize icon ( Optimization window opens. 3. Enter the following data in the Optimization window: Problem tab Optimization type Optimized parameter Free parameters Minimization distance Geometrical Set.1 Algorithm Termination criteria Point.3 Z ). The
Simulated AnnealingConvergence speed Maximum number of updates: 100 Consecutive updates without improvements: 20 Maximum time (minutes): 5
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New constraint
Geometrical Set.1 Point.3 Z` - max (Geometrical Set.1 Point.2 ,Geometrical Set.1 Point.1 <= 0mm Z) Z)
4. Click OK in the opening dialog box, click Run optimization. 5. Select an output file and click Save. 6. Click OK once the optimization process is over. 7. From the Start->Knowledgeware menu, access the Knowledge Advisor ). The Script Editor workbench and click the Macros with argument icon ( opens. Enter the following data in the editor and click OK: Argument Script body optim optim.Run false
8. Click the Reaction icon (
). The Reaction dialog box opens. • • In the Source type field, select Owner. In the Available events list, select BeforeUpdate. In the Action field, select Knowledgeware action.
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9. Click the Edit action... button, paste the following script in the editor, and click OK twice: if (CableLength <= distance (Geometrical Set.1 Point.1
,Geometrical Set.1 Point.2 )) Message ("Incompatible inputs: cable length is less than distance between points!") else { `VB Script.1` .Run(Relations Optimizations.1 Optimization.1 )
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10. Double-click the root of the specification tree and select the Insert>UserFeature->UserFeature Creation... command. The User Feature Definition window opens. 11. In the Name field, enter the name of the UDF: Cable1 in this scenario. 12. Select the Spline, Point3, Reaction.1, VB Script.1, Optimization.1, the 4 formulas, and the parameters: they are displayed in the User Feature definition window (see below.)
Note that the UDF becomes the owner of the reaction. This reaction will be fired before the update of the UDF instance. 13. Click the Parameters tab, select CableLength, click the Published name check box and click OK. 14. Save the file and close it. 15. Create a new .CATPart file, access the Generative Shape Design workbench, and create 3 points. 16. Select the Insert->Instantiate From Document... command. The File Selection window opens. Select the KwrEvent_BeforeUpdate.CATPart file you just saved and click the Open button. 17. The Insert object dialog box opens. Select Point.1 and Point.2 in the geometry or in the specification tree and click OK. The cable (UDF) is instantiated and the optimization is launched before the update. 18. Repeat steps 14 and 15: select Point.2 and Point.3 when instantiating the UDF: the cable lengths are optimized.
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19. Double-click the CableLength=400mm parameter and change its value to 200mm. This cable length is optimized once again just before the update. To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: File Content Modification Event
This task explains how to use the FileContentModification event associated with the reaction feature. This event launches a reaction each time the file associated with the design table is modified. 1. Open the KwrBallBearing1.CATPart file. The following picture is displayed.
2. Click the Design Table icon ( is displayed.
). The Creation of a Design Table dialog box
3. Click the Create a design table from a pre-existing file option and click OK. The File Selection dialog box opens. 4. Select the KwrBearingDesignTable.xls file and click Open. Click Yes when asked if you want to associate the columns of the tables with the parameters. 5. Click OK to apply the default configuration. 6. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( opens. ). The Reaction dialog box • In the Source type field, select Selection and select the DesignTable.1 in the specification tree for the Reaction to be applied to the design
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table. • In the Available events list, select FileContentModification. In the Action field, select Knowledgeware action and enter the following message: Message("The design table was modified"). Click OK when done. The Reaction feature is added to the Relations node.
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7. Double-click DesignTable.1 in the specification tree. The Design Table window is displayed. 8. Click the Edit table... button and change the material of row 2 to Gold. Save your file and close it. The reaction is launched and the message is displayed.
To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: Update Event
This task explains how to use the Update event associated with the reaction feature. The CATPart file contains a rulebase that is updated each time a modification is made. 1. Open the KwrEvent_Update.CATPart: It contains a part with holes and a rulebase made up of 2 checks.
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2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( ). The Reaction dialog box opens. • In the Source type field, select Selection and select the RuleBase in the specification tree for the Reaction to be applied to the rulebase. In the Available events list, select Update. In the Action field, select Knowledgeware action and enter the following message: Message("Rulebase updated").
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3. Double-click the CATKWECheck.1. The Check Editor opens. Modify the check: (H Diameter == 20mm) and click OK 4. Right-click the rulebase and select the Rulebase object->Manual Complete Solve command. The reaction is fired and the following message is displayed:
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To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Using a Reaction with a User Feature: Instantiation Event
This task explains how to use a reaction in a User Defined Feature. The scenario described below is divided into two major steps: • In the first step, you first create a formula that returns the length of the line, you create a reaction that will add items of length type to a list when the document is instantiated and then you create a UDF containing the line, the reaction and the formula. In the second step, you open a second document, you create a rule based on a list that will display the total length, and then you instantiate the UDF that you previously created in this document.
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A basic understanding of the Part Design workbench and of Product Knowledge Template is required to perform this scenario. Note that the Instantiation event is available for User Features only. It cannot be used with Power Copies. 1. Open the KwrUDFandReaction.CATPart file. 2. Create a parameter of Length type and assign it a formula. • icon, select Length in the New Parameter of Click the Type scrolling list, click the New Parameter of type button, and click the Add Formula button. In the Dictionary, click Measures, and double-click length
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(Curve,): Length. • Position the cursor between the parentheses and double-click Line.1 in the specification tree. Click OK, Yes, and OK. (Length.1=length(Geometrical Set.1 3. Access the Knowledge Advisor workbench, click the List icon ) to ( create a list, and click OK. An empty list appears under the Parameters node. Line.1)).
4. Click the Reaction ( o o o
) icon. The Reaction editor opens:
In the Source type list, select Owner. In the Available events, select Instantiation. In the Action area, select Knowledgeware action and click the Edit action button. The Action editor opens. Click the list in the specification tree and, in the Dictionary pane select List, and in the Member pane, double-click List.AddItem. Position the cursor between the parentheses and enter Length.1 before the comma, and 0 after the coma. Click OK twice. The Reaction feature is created.
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5. Access the Part Design workbench and select the Insert->UserFeature>UserFeature creation command. The Userfeature Definition window opens: in the Definition tab, enter the name of the User Feature (UserFeature1 in this scenario) and select the Line, the Reaction, and the Length parameter in the specification tree. Click OK. The UserFeature1 is created and displayed under the Knowledge Templates node.
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6. Save your file, close it, and open the KwrUDFandReaction2.CATPart file This is the file into which you will instantiate the UDF you previously created. 7. Access the Knowledge Advisor workbench, and click the list icon ( create an empty list and click OK. ) to
8. Create a parameter of Length type (called Length.1 in this scenario) and apply a formula to it. icon, select Length in the scrolling list, click the New Click the Parameter of type button, and click the Add Formula button. Select the list in the specification tree, in the Dictionary pane select List, and in the Member pane, double-click List.sum. Click OK three times. ), click OK, enter the following script in the Rule
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9. Click the Rule icon ( Editor, and click OK:
Message("Total Length : #",Length.1 ) 10. The total length is displayed: 0mm. 11. Access the Part Design workbench and select the Insert->Instantiate from Document command. 12. Select the file you created (from step 1 to step 5, KwrUDFandReaction.CATPart in this scenario) and click Open. The Insert Object window opens: • • • Select Point.1 in the specification tree or in the geometry. Select Point.2 in the specification tree or in the geometry. Select List.1 in the specification tree and click OK. The rule is fired and the Total Length is displayed.
Creating a Loop in a Reaction
This task explains how to create a loop in a reaction. In the scenario described below, you are going to: • • • Create 3 points that are inserted into a list Create a formula that will automatically fill in the list Create a reaction that will set the Z coordinate of the points to
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• •
20mm if this value is inferior to 20mm. Create a reaction that will set the Y coordinate of the points to 40mm if this value is inferior to 40mm. Update the Part
It is now possible to create the While and the For constructs. To know more, see Using the Knowledge Advisor Language. 1. Create a Part containing 3 points. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 3. Click the List icon ( 4. ) to create the list that will contain the created points.
Add a formula to fill in the list. o Click the Formula Editor icon. The Formula Editor is displayed. In the specification tree, select List.1 and click the Add formula button. List.1=PartBody.Query("Point",""). Click OK twice when done. Note that Japanese users should enter the following formula.
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6. Click the Reaction icon (
). The Reaction dialog box opens. • In the Source type field, select Selection and select the list in the specification tree for the Reaction to be applied when the list is modified. In the Select a source... dialog box, select List.1 and click OK. In the Available events list, select ValueChange.
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In the Action field, select Knowledgeware action and enter the following message action body.
let x(Point) for x inside parameter { if (x.GetAttributeReal("Z") < 0.02) x.SetAttributeReal("Z",0.02) } • Click OK when done. The Reaction feature is added to the Relations node.
7. Click the Reaction icon (
). The Reaction dialog box opens. • In the Source type field, select Selection and select the list in the specification tree for the Reaction to be applied when the list is modified. In the Select a source... dialog box, select List.1 and click OK. In the Available events list, select ValueChange.
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In the Action field, select Knowledgeware action and enter the following message action body. let i = 1 let x(Point) for i while i<=parameter.Size() { x = parameter.GetItem(i) if (x.GetAttributeReal("Y") < 0.04)
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x.SetAttributeReal("Y",0.04) } • Click OK when done. The Reaction feature is added to the Relations node.
8. Create a new point with the following coordinates: X: 36mm Y: 12mm Z: 0mm 9. Update the Part twice: The Y and Z coordinates are set to 40 and 20 mm. Click here to display the result sample. To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Launching a VB Macro with Arguments
The task below illustrates how to add arguments to a macro. Macros with arguments are features that can be: • • • stored in CATPart or CATProduct documents, stored in catalogs. Double-click them in the catalog to run them, called from a rule (VBScriptRun) or a reaction. In this case, arguments are passed from the rule.
icon enables you to access the macro editor. In addition to the usual The 'edit and run' capabilities, this editor allows you to: • specify arguments • carry forward a feature definition to the editor just by selecting the feature either in the tree or in the geometry area.
Note that the VB macro with arguments functionality is intended to help you write macros. It is not intended to find the code of other objects: Only the
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objects that were correctly integrated to the macros are supported. 1. Click the icon. The script editor is displayed.
2. Copy/paste the script below into the editor:
Dim oActiveDoc As Document Set oActiveDoc = CATIA.ActiveDocument
If (InStr(oActiveDoc.Name,".CATPart")) <> 0 Then
Dim oParams As Parameters Set oParams = oActiveDoc.Part.Parameters
Dim strParam1 As StrParam Set strParam1 = oParams.CreateString("FirstName", "")
Dim strParam2 As StrParam Set strParam2 = oParams.CreateString("LastName", "")
strParam1.Value = fname strParam2.value = lname
Else MsgBox "The active document must be a CATPart" End If
End Sub
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3. Enter the fname and lname arguments in the field located between the parentheses. The arguments must always be separated by a comma. 4. Click OK to add the macro to the document. A 'VB Scripts' sub-node is added to the specification tree below the Relations node. A VB Script object is added below this sub node. 5. Double-click the VB Script object. The Script Editor is displayed. The Insert Object Resolution button allows you to retrieve a feature definition. The VB Script.2 macro of the KwrObject.CATPart sample illustrates how to use this capability. 6. Click Run script.... The Select Inputs for Script Arguments is displayed. 7. If need be, select fname in the argument list, then enter a string into the value field (no quotation marks). Then select lname and enter the lname value. 8. Click OK to run the script. The two string type parameters are added to the document. Their values are those you have just specified. Note that the VB script features with arguments are provided with a contextual menu enabling the user to launch the script.
Working with Relations
Working with Relations
Relations located at a product level are not integrated to the product update process. If your relation drives parameters located at a Part level, create the relation at the Part level.
Select the Add Set of Relations icon to regroup relations into categories. Select the Measure Update icon to perform the update of relations using measures. Creating Sets of Relations Using Relations based on Publications at the Product Level Activating and Deactivating a Component Instantiating Relations from a Catalog Updating Relations Using Measures Controlling Relations Update
Creating Sets of Relations
This task explains how to create sets of relations below the Relations node of the specification tree.
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Using this capability enables you to regroup relations into categories. When you create a relation, you are prompted to enter a destination. i.e. a feature you add the new relation to. Formulas, design tables, rules and checks can all be created into relation sets. When no relation set has been created, the destination field of the relation editor is by default initialized to the Relations node. 1. Create a Part and from the Start->Knowledgeware menu, access the Knowledge Advisor workbench. icon and click the Relations node, the Relations.1 (or 2. Click the Relations.n) relation set is added to the specification tree right below the Relations node. 3. Click the Rule or the Check creation icon. The first dialog box displayed is similar to the one displayed when you create a relation right below the Relations node except that you must specify a destination. To do so, select the value specified in the Destination field of the relation editor, then select the Relation Set you want to add a relation to. This results in a modification of the destination path in the relation editor (partname partname Relations.n is replaced with Relations Relations.n).
4. Click OK to display the next dialog box and enter the relation body. 5. After you have finished specifying the new relation, click OK in the editor dialog box. In the specification tree, you can expand the feature which represents the relation set. A new relation has been added below this relation set.
Using Relations based on Publications at the Product Level
This scenario explains how to use relations based on publications at the product level. The scenario described below is divided into the following steps: • Add a parameter to the KwrScrew.CATPart called Screw_Volume, add a formula to calculate the volume of the screw and publish the Screw_Volume parameter. Add a parameter to the KwrScrew1.CATPart called Screw_Volume, add a formula to calculate the volume of the screw and publish the Screw_Volume parameter. Create a CATProduct file called Bolt and import the KwrScrew.CATPart Import KwrNut.CATPart. In the context of the Bolt product, create a formula calculating the bolt volume based
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on the screw and the nut publications. • In the context of the bolt, replace KwrScrew.CATPart by KwrScrew1.CATPart. The volume is recomputed.
Before you start, make sure that the Keep link with selected object check box is checked (Tools->Options->Infrastructure->Part Infrastructure->General). Note that this function can be used with: • • • • • Design Tables Formulas Rules and Checks Set of Equations The optimization
1. Open the KwrNewScrew.CATPart document. The following image is displayed.
2. Add a Volume parameter to the part. Click the icon. The Formula Editor opens. In the New parameter of type scrolling list, select Real and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: Screw_Volume. Click Apply and click the Add Formula button. The Formula Editor opens. Enter the following formula by using the Dictionary:
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Screw_Volume=smartVolume(PartBody Pad.2 ). Click OK three times. 3. Publish the Screw_Volume parameter. To do so, select the Tools>Publication command and click the Screw_Volume parameter under the Parameters node in the specification tree. Click OK. The published parameter appears in the specifications tree below the Publication node. Save your file and close it.
Pad.1)+smartVolume(PartBody
4. Open the KwrNewScrew1.CATPart and repeat the steps listed above (steps 1 to 3 included). The part should be identical to the one below. Save your file and close it.
5. Create a CATProduct file named KwrBolt.CATProduct. 6. Click the Root product and select the Insert->Existing Component... command. The File selection box is displayed. Select the KwrNewScrew.CATPart file and click Open. The screw is
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imported. 7. Select the Insert->Existing Component... command, select the KwrNewnut.CATPart file and click Open. The nut part is inserted.
8. Add a Bolt_Volume parameter to the product to compute the volume of the bolt.
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icon. The Formula Editor opens. In the New param Click the Root product and click the of type scrolling list, select Real and click the New parameter of type button.
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In the Edit name or value of the current parameter field, enter the name of the paramet Bolt_Volume. Click Apply and click the Add Formula button. The Formula Editor opens.
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Enter the following formula by using the Dictionary and by clicking the published parameters i specification tree: Bolt_Volume=`..!screw.2!Screw_Volume` +`..!Nut!Nut_Volume` Click OK, and OK. The Bolt volume is displayed
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9. Replace the screw to compute a new volume: Double-click, then right-click the Screw.2 component in the specification tree and select the Components->Replace Component... command. The File Selection window opens. Select the KwrNewScrew1.CATPart file and click Open. 10. Click Yes and OK in the Impacts on Replace window. The new screw is inserted and the bolt volume is updated.
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Activating and Deactivating a Component
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This task explains how to activate and deactivate a component. In the scenario described below, the CATProduct file contains two CATPart files that you will activate and deactivate alternatively after creating user parameters and a rule based on these parameters. Note that: • • Relations located at the product level are not integrated to the product update. If your relation drives the parameters of a Part, create the relation at the Part level. Parameters driven by rules are designed to enable you to control components activities at assembly level.
When working in a Japanese environment, remember to check the Surrounded by the Symbol' option (Tools->Options->General->Parameters and Measure->Knowledge tab).
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1. Open the KwrSyringe.CATProduct file and save the following files in the same directory (SyringePiston.CATPart, HollowSyringePiston.CATPart, and SyringeContainer.CATPart): This file contains a syringe made up of three different parts: A barrel, and two different plungers. 2. Create a multiple value parameter of string type. • • Click the icon. The Formulas Editor opens.
Select String in the scrolling list with Multiple Values. Click the New Parameter of type button. The Value List dialog box opens. Enter two different values, Hollow and Full, and click OK. Edit the name of the new parameter (SyringeType in this scenario) in the Edit Name or value of the current parameter and click OK. The new parameter is displayed under the Parameters node of the Specification tree.
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3. Access the Knowledge Advisor workbench and click the Rule icon to create a rule. The script of this rule will allow you to enable or disable one of the plungers. 4. Enter the code below in the Rule Editor, and click OK. if (SyringeType == "Hollow") { `S3\Component Activation State` `S2\Component Activation State` } else { `S2\Component Activation State` `S3\Component Activation State` }
= false = true
= false = true
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Note that Japanese users should enter the following rule.
6. Double-click the SyringeType parameter under the Parameters node and select Hollow in the Edit Parameter window. The SyringeBarrel CATPart and the HollowSyringePlunger CATPart are displayed.
7. Double-click the SyringeType parameter and select "Full" in the Edit Parameter window. The SyringeBarrel CATPart and the SyringePlunger
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CATPart are displayed.
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Instantiating Relations from a Catalog
The scenario developed below explains how to instantiate a check stored in a catalog into a CATPart document. Formulas, rules and checks can be stored in a catalog. They can then be reused in a document by using an instantiation mechanism. For more information about catalogs, see the Infrastructure User's Guide. 1. Open the Formula_005_Start.CATPart file. 2. In the Tools toolbar, click the icon. The catalog browser is displayed.
3. Click the icon to open the CatalogFormula.catalog catalog. The catalog browser looks something like the one below (you may need to expand the Knowledge node to display the three relations Formula.1, Check.1, Check.2 what you see in the left-hand part of the Catalog Browser depends on the last interactions you have carried out with this dialog box).
4. Double-click the Check.1 object. The dialog box below is displayed.
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5. Rename the Check.1 check by using the Name field. Enter HeightCheck for example. 6. The 'Hauteur' input is highlighted. In the part specification tree, select the "Hauteur" parameter. The Rayon input is now highlighted. In the specification tree, select the "Rayon" parameter. Click OK and Close. The HeightCheck is added to the specification tree and, depending on the values assigned to the Height (Hauteur) and Radius (Rayon) parameters, a message can be displayed. 7. Double-click the HeightCheck relation twice in the specification tree. The relation below is displayed in the check editor: Hauteur >= Rayon. The relations of a catalog must be instantiated one-by-one in a document.
Updating Relations Using Measures
This task explains how to update relations using measures. A relation using measures is to be updated when the opposite the relation in the specification tree. Example MeasureRule requires an update symbol is displayed
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MeasureRule does not need to be updated
To update the rules: • Click the icon. To do this you must be in the Knowledge Advisor workbench. -or• Select the Measure Update command from the Relations node contextual menu. You can do this in any workbench.
All the document relations are then updated.
Controlling Relations Update
This topic provides you with 2 short examples showing you how to work with relations in Synchronous and in Update relation at global update command modes. • • In the first example, you update a formula. In the second example, you update an equation.
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For a given relation, it is possible to determine that it only executes in Synchronous mode using the Edit->Properties command. Its evaluation can then be launched manually. The Synchronous mode enables you to create synchronous relations, that is to say relations that will be immediately updated if one of their parameters is modified. Relations based on parameters are the only ones that can be synchronous.
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For a given relation, it is also possible to decide that its evaluation will be launched when the part is updated (Update relation at global update command). The relations can be asynchronous for 2 reasons: o You want the relation to be asynchronous o The relation contains geometry.
It is possible to change the update mode of a relation after it is created. • Right-click the relation in the specification tree and select the
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Properties command. Check the Synchronous or the Update relation at global update command check box.
To know more about the Synchronous or the Update relation at global update command options, see the description of the Knowledge tab in the Infrastructure User's Guide.
Updating a Formula
In this example, the document contains 2 parameters of Length type: • Length.1 is valuated by you. Length.2 is valuated by a formula computing the distance between 2 points + Length.1.
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1. Open the KwrUpdatingaFormula.CATPart file. The following image is displayed.
2. Expand the Relations node (if need be), right-click Formula.1 and select the Properties command. 3. In the Properties window, uncheck the Update relation at global update command check box. Click OK to validate.
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4. Double-click Length.1. The Edit parameter window is displayed. Enter 50 in the value field. Click OK to validate. The value of Length.2 is updated automatically and an update icon is displayed indicating that it will also be updated at the global update. 5. Right-click Formula.1 and select the Properties command. 6. In the Properties window, uncheck the Synchronous check box and check the Update relation at global update command check box. Click OK to validate. 7. Double-click Point.2 in the specification tree or in the geometry. 8. Enter the following values in the Point Definition window and click OK when done:
The Formula is not updated and an update icon is displayed next to the formula. 9. Right-click Formula.1 and select the Local Update command. The formula and Length.2 are updated.
Updating an Equation
In this example, you change 3 parameters, a, b and c before solving the equation. If you use the Synchronous mode, an error is displayed when modifying the parameters values since the update is launched at each modification. To ensure the stability of the equation, the update must be launched after the 3 parameters are changed. Thus you need to select the Update relation at global update command mode. 1. Open the KwrUpdatinganEquation.CATPart file. The following image is displayed: This document contains 4 parameters. x is a parameter valuated by an equation based on the other 3 parameters (a, b, and c).
2. Expand the Relations node (if need be), right-click Equations.2 and select the Properties command. 3. In the Properties window, check the Synchronous check box and uncheck the Update relation at global update command check box. Click OK to validate. 175 4. Double-click a in the specification tree. The Edit Parameter window is displayed. Enter 2 in the value field. A message is displayed indicating that the equation cannot be solved and click OK.
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Working with the List Feature
Working with the List Feature
Select the List icon to create a list of features that will be located under the Parameters node in the specification tree. Clicking this icon opens the List edition window.
List features can be used to manage lists of objects or parameters. These lists can be edited interactively. The List edition window enables you to sort items automatically and to specify the type of objects authorized. The list feature is integrated in the update mechanism, the size of the list is computed automatically (it is provided with functions designed to compute sums, areas, costs...). The list feature can be manipulated through the language to: • Create list • • • • • Copy the content of a list into another one Add and remove elements Get an element Retrieve values from the list Move elements of the list to another position
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Using the List Edition Window
The List Edition window enables you to manage the objects you want to add to the list you are creating. It can be accessed by clicking the List icon ( ).
The window contains four different buttons and is made up of 2 columns. Name Column indicating the name of the list. Enables you to add the items you selected in the specification tree or in the geometry to the list. Enables you to remove items from the list. Enables you to move up items in the list. Enables the user to move down items in the list. The Number of Elements field displays the number of items contained in the list. Value/<Type> Column indicating the value of the list or the associated type.
There are 4 different types of lists: • Not seen lists: These lists are created by CAA users and cannot therefore be modified interactively by the user (they are not displayed). In this case, the buttons of the List dialog box do not display. Read only lists: These lists are created by CAA users and cannot therefore be modified interactively by the user (they are in read only mode). Read/Write lists: These lists are created by CAA users, can be edited by the end user but they cannot be deleted.
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User lists: These lists can be edited and deleted by the end user.
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Like for any other parameter, it is now possible to hide and reorder lists. To do so, rightclick the list and select the Hide or Reorder... commands. When clicking the List icon to create a list, the MultiSelection window now is displayed. To find out more about this window, see the Infrastructure User's Guide. If you select an item in the List, and click another item in the specification tree or in the geometry, and click Add, the List item will be replaced with the one you have just added.
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Creating a List
This task explains how to use the List Feature. In the scenario described below, you are going to manipulate a plane wing to which you will add planes and intersections. You will then create parameters and formulas to calculate the surface of the intersections and will create a list that will compute the total area of the intersect sections. To find out more about the List Edition window, see Using the List Edition Window. To find out more about the List Feature, see Working with the List Feature. 1. Open the KwrPlaneWing.CATPart file. 2. Access the Generative Shape Design workbench. 3. Create three planes. • Click the Plane icon in the tool bar.
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a) The Plane Definition dialog box opens. b) In the Plane type area, enter the yz plane (select it in the geometry or in the specification tree): The yz plane is displayed in the Reference area. c) Indicate the required offset in the Offset field (-50mm for example). Click OK. d) Repeat this operation twice with offsets of -100 and -150mm. (Click the graphic to enlarge it)
4. Add formulas to calculate the intersection surface of the planes with the blend. • • Click the icon. The Formulas Editor opens.
Select Area in the scrolling list and click the New parameter of type button. Change the name of the parameter to Area_Intersect1 and click the Add Formula button. The Formula editor opens. In the Dictionary, select Measures, double-click area(Surface, ...):Area. Position the cursor between the parentheses, select Wireframe constructors in the Dictionary, and double-click intersect(Surface,Surface):Curve. Position the cursor before the coma and select Plane.2 in the specification tree (or in the geometry) then select Blend.1 in the specification tree. Click OK.
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Repeat the above steps for Area_Intersect2 and Area_Intersect3 by selecting Plane.3 and Plane.4.
(Click the graphic to enlarge it)
5. Access the Knowledge Advisor workbench, and click the List icon ( window opens. 6. Select the 3 parameters located under the Parameters node in the specification tree, and click the Add button. Click OK. Rename List.1 to Intersections for example. (Click the graphic to enlarge it)
). The List Edition
7. Click OK. The list is added to the parameters. 8. Add a formula that will compute the area of the 3 planes intersections with the blend. Click the icon. Select Area in the scrolling list, click the New parameter of type button, rename the parameter to Total_Intersection_Areas and click the Add formula button. The Formula editor opens.
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Click the List (Intersections in this scenario) in the specification tree: the name of the list is displayed in the editor. Under Dictionary, select List, and double-click List.Sum(): Real in the Members of List area. Click OK twice.
The area of the 3 planes intersections with the blend is automatically calculated.
(Click the graphic to enlarge it) 9. Edit the list content and re-compute the total area. o Double-click the list (Intersections) in the specification tree: the List edition window opens. Select Area_Intersect3, click the Remove button, and click OK. Right-click the Total_Intersection_Areas parameter and select Local Update. The area of the remaining 2 planes intersections with the blend is automatically calculated. (Click the graphic to enlarge it) Click here to display the result of this scenario.
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Working with the Loop Feature
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Working with the Loop Feature
Select the Loop icon to create a loop. Introducing the Loop Feature Getting Familiar with the Loop Edition Window Creating a Loop Creating a Power Copy containing a Loop Using the Scripting Language Reference
Introducing the Loop Feature
Note that a KWA license is required to execute loops. Loops use the Generative Knowledge language to drive the creation, modification and deletion of a set of features. This functionality enables you to: • • • Select inputs in the definition of the loop Define several contexts in the loop action Include the loop into a Power Copy
It can be accessed by clicking the Loop icon ( • •
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A loop is stored in the resulting model as a feature on its own. A change in its specification will drive the expected modification in the model. A loop can be instantiated through a Power Copy implying a significant simplification of use and re-use.
Getting Familiar with the Loop Edition Window and Menus
• • • The Loop Edition Window The Loop Tools Menu The Loop Contextual Menu
The Loop Edition Window
The Loop Edition window is displayed when you click the Loop icon ( Control Features tool bar. ) in the
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Input(s)
This field enables you to select the features that you want to use in the specification tree or in the geometry. The selected features are those that will be used in the loop body. To deselect items from the Inputs list, click them in the specification tree or in the geometry. The Input Name field enables you to rename the inputs that you selected. In this case, this name will be used in the loop body.
Context
This field enables you to define the application context of the loop. It can be any V5 feature. To select the context, click the Context field once, then click the item in the specification tree.
Iterators
The From ... To fields enable you to define the number of times that the loop will operate. When defining the ranges, you can right-click the From... and the To fields to access the contextual menu. • The Edit formula... command enables you to access the Formulas editor and to create a formula that will apply to the loop operation. To know more, see Creating a Formula. The Add Multiple Values... command enables you to add multiples value. To know more, see Switching between Simple and Multiple Values After Creating a Parameter. The Add Range... command enables you to add a range.
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The Edit Comment... command enables you to add a comment. The Lock... command enables you to lock this parameter. To know more, see Locking and Unlocking a Parameter .
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Note that: • • The step is one in the From... To fields. Both bounds are included when the loop runs.
Editor
The Editor enables you to enter the loop syntax. The language to use in this editor is the scripting language. To find out more about the syntax to be used, see Using the Scripting Language.
The Tools menu
The Tools->Object Browser ... command enables you to access the Object Browser. This browser contains the types and attributes that are part of the scripting syntax. The object browser guides you when writing a script. It allows you to access the keywords, operators and feature attributes that can be used when working with the loop features. The packages displayed in the left part of the browser are those you selected from the Tools->Options... command. To add or remove packages: 1. Select the Tools->Options... command to open the Options window, then select General->Parameters and Measure, and click the Language tab. 2. In the Language field of the Knowledge tab, check Load extended language libraries and select the libraries.
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From this window, you can manipulate the list o objects supported by the script using their attributes... • The left part of the browser displays the available packages.
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The central part displays the list of object belonging to this category.
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The right part displays the attributes allowing you to manipulate these objects any).
... and write loop bodies (see example below): Circle0 isa GSMCircle { CircleType = 0; TypeObject isa GSMCircleCtrRad { Center = object: .. .. .. Construction_Body Support = object:
Point.2;
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.. Construction_Body Radius = 180mm; } StartAngle = -100deg; EndAngle = 100deg; }
Extrude
The Back icon. To return to your last interaction in the wizard. Has no action on the script editor. The Forward icon. To go forward to your next interaction in the wizard when moving through a series of interactions. The Attribute Type icon. This icon is not available in the current version of the product. The Inheritance icon. To return to the root object. The Insert icon. To insert the object name in the script.
The Loop Contextual menu
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knowledgewareAdvisor You can access the Loop contextual menu by right-clicking the loop in the specification tree. • The Definition... command enables you to access the Loop Edition window. The Deactivate... command enables you to deactivate the loop. In this case an icon indicates that the loop is disabled. To enable it, right-click it and select the Loop activate... command. The Hide command enables you to hide the loop. In this case, it will not be displayed in the specification tree. The Reorder... command enables you to reorder the loops.
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Creating a Loop
The task below illustrates how to interactively apply a loop to an existing document.
The KwrLoop1.CATPart is made up of a surface (2) and a solid (1) that symbolizes a hole. This hole is inserted into a User Feature (UDF) for a later instantiation. The User Feature (UDF) has 3 different inputs (a point, an axis and a surface). 2 parameters of the User Feature (UDF) are published (3). • • Clearance=4mm Diameter=8mm
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The KwrLoop2.CATPart is made up of a surface (1) and of 12 points (3) inserted into a list. The Line.7 is the instantiation axis (2).
The aim of this scenario is to instantiate as many holes as existing points. It is divided into the following steps: • You create a loop. • • You instantiate the User Feature (UDF) from the existing .CATPart file. You valuate the required inputs to instantiate the holes.
To create a loop, you have to: 1. Declare input data 2. Define the context 3. Specify iterators 4. Write the body of the action script Before creating a loop in a CATPart document, make sure that the Manual input option is unchecked in the Part Number field of the Tools->Options...>Infrastructure->Product Structure->Product Structure tab. To perform this scenario, you will need the following files: • • KwrLoop1.CATPart KwrLoop2.CATPart
1. Open the KwrLoop2.CATPart
Creating a Loop
2. From the Start->Knowledgeware menu, access the Knowledge Advisor
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workbench. 3. Click the Loop icon ( window is displayed. ) in the Control Features bar. The Loop Edition
4. In the specification tree, select the inputs of the loop. o Expand the Parameters node and select the List_Extract list. In the Input name field, enter the name of the list: PointsList. Expand the Surface node and select the Revolute.1 feature. In the Input name field, enter the name of the list: SurfRef. Expand the Result_Body node and select the Line.9 feature. In the Input name field, enter the name of the list: LineAxis. Note that the name indicated in the Input name field is the one that will be used in the loop body. 5. Select the context, that is to say, in this scenario, the feature that will contain the instantiated holes. o o Click the Context field. Click Result_PartBody in the specification tree.
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6. Indicate the number of holes that you want to instantiate into the surface. o o In the From field, indicate 1. Right-click the To... field and select the Edit formula... command. The Formula Editor is displayed. In the specification tree, click ListSize=12. Click OK when done. The number of instantiated holes is now valuated by a formula based on the list, that is to say on the number of points contained in the list.
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7. Enter the following action script into the Editor. o Use the import keyword to indicate the path of the file containing the User Feature (UDF) to be instantiated. To indicate the path of the file, it is recommended to use the Insert File Path command available in the contextual
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menu to import KwrLoop1.CATPart. (1) o o UDF_$i$ is the name that will be attributed to each instance of the hole. At each iteration, $i$ is replaced with the current iterator. (2)
8. • • • Clearance_Hole_UDF is the name assigned to the User Feature (UDF) in the KwrLoop1.CATPart file. (2)
Position is a point and is also the first input that needs to be valuated when instantiating the holes. PointsList is the name of the List. (3) Clearance_Surface is the second input required and defined when creating the User Feature (UDF) and SurfRef is the revolute into which the holes will be instantiated. (3) Axis is the third input required and defined when creating the User Feature (UDF) and LineAxis is Line.9, that is to say the instantiation axis. (3)
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To find out more about the syntax to be used (;, {}, $i$) in the loop body, see Using the Scripting Language. Click OK when done. The 12 holes are instantiated. (See picture below.)
Creating a Power Copy Containing a Loop
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This task illustrates how to interactively apply a loop to an existing document. In this scenario, you are going to make holes in a pad. To do so, you are going to: • • • Create a loop referencing the inputs of an existing User Feature (UDF) used to make holes in a pad. Save the loop in a Power Copy. Instantiate the Power Copy into an existing document and creates the holes.
To perform the scenario, you will need the following files: The KwrLoop1.CATPart is made up of a surface (2) and a solid (1) that symbolizes a hole. This hole is inserted into a User Feature (UDF) named Clearance_Hole_UDF for a later instantiation. The User Feature (UDF) has 3 different inputs (a point, an axis and a surface). 2 parameters of the User Feature (UDF) are published (3): • • Clearance=4mm Diameter=8mm
The KwrLoop3.CATPart file is made up of a pad and a surface and of 24 points (1) inserted into a list. Line.2 is the instantiation axis (2). This .CATPart file is the one that will contain the loop contained in the Power Copy that will be instantiated into KwrLoop4.CATPart.
The KwrLoop4.CATPart is made up of a pad and a surface (3) and of 17 points (2) inserted into a list. Line.1 is the instantiation axis (1). It will contain the instantiated loop and the holes.
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Before creating a loop in a CATPart document, make sure that the Manual input option is unchecked in the Part Number field of the Tools->Options...>Infrastructure->Product Structure->Product Structure tab. To create a loop, you have to: 1. Declare input data 2. Define the context 3. Specify iterators 4. Write the body of the action script Creating the loop referencing the user feature (UDF) 1. Open the KwrLoop3.CATPart. The following image is displayed.
2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 3. Click the Loop icon ( is displayed. ) in the Control Features bar. The Loop Edition window
4. In the specification tree, select the inputs of the loop. o Expand the Parameters node and click the Lists_PointRef list. In the Input Name field, enter the name of the list: PointsList. Expand the Geometrical Set.1 node and select the Clearance_Surface feature. In the Input name field, enter the name of the feature: SurfRef. Expand the Holes_Points node and select the Line.2 feature. In the Input name field, enter the name of the line: LineAxis. Note that the name indicated in the Input name field is the one that will be used in the loop body. 5. Select the context, that is to say, in this scenario, the feature that will contain the instantiated holes.
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Click the Context field. Click ResultBody in the specification tree.
6. Indicate the number of holes that you want to instantiate into the surface. o o In the From field, indicate 1. (1 corresponds to Extract.1.) Right-click the To... field and select the Edit formula... command. The Formula Editor is displayed. In the specification tree, click ListSize=24. Click OK when done. The number of instantiated holes is now valuated by a formula based on the list, that is to say on the number of points contained in the list.
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7. Enter the following action script into the Editor. o Use the import keyword to indicate the path of the file containing the User Feature (UDF) to be instantiated (KwrLoop1.CATPart) . To indicate the path of the file, it is recommended to use the Insert File Path command available in the contextual menu to import KwrLoop1.CATPart. (1) UDF_$i$ is the name that will be attributed to each instance of the hole. (2) Clearance_Hole_UDF is the name assigned to the User Feature (UDF) in the KwrLoop1.CATPart file. (2)
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Position is a point and also the first input that needs to be valuated
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when instantiating the holes. PointsList[$i$] is the name of the List. [$i$] corresponds to the nth item of the list. In this case, nth is equal to 24, the number of holes to be instantiated (3). o Clearance_Surface is the second input required and defined when creating the User Feature (UDF) and SurfRef is the revolute into which the holes will be instantiated. (4) Axis is the third input required and defined when creating the User Feature (UDF) and LineAxis is Line.9, that is to say the instantiation axis. (5) Clearance is one of the published parameters of the User Feature (UDF). It is used in the action script because you want the value of the published parameter to be modified. (6)
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To find out more about the syntax to be used (;, {}, $i$) in the loop body, see Using the Scripting Language. 8. Click OK when done. The holes are instantiated (see graphic below.) 9. Click the Update icon ( ) to update the document.
10. Right-click the loop and use the Properties command to rename the loop into Loop_Holes. Click OK when done. 11. In the specification tree, right-click the loop (located below the Relations node) and select the Loop_Holes object->Deactivate command. Saving the loop in a Power Copy 12. Click the root of the specification tree, and from the Start->Mechanical Design menu, access the Part Design workbench. 13. From the Insert->Advanced Replication Tools menu, select the PowerCopy Creation... command. The Power Copy Definition window is displayed. 14. In the specification tree, select the items making up the Power Copy: o o Formula.1 Loop_Holes
Note that the Power Copy will need the following inputs at instantiation time: o o o o o ListSize Line.2 Clearance_Surface List_PointsRef ResultBody
15. Click OK when done. The Power Copy is created and is displayed below the 193 Power Copy node in the specification tree. 16. Save your file and close it.
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Using the Scripting Language
Using the Scripting Language
Introducing the Scripting Language The Scripting Language is a declarative way of generating V5 Features. It allows you to: • Describe objects using a very simple script language. • Use 3D geometric features (sketches, parts, ...). • Use parameters on features including formulas. • Use related positioning & orientation constraints. • Generate the corresponding V5 models (features, documents, User Features,...) Enter the body of their loops in the Loop Edition window in Knowledge Advisor.
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Action Script Structure Object Properties Operators Keywords Variables Comments Limitations Using the Get... Commands
Action Script Structure
An action script is written in text format and is organized in blocks consisting of related sets of statements. A block consists in an instruction designed to create an object followed by a set of statements surrounded by braces ({ }). Statement blocks can be nested and the most enclosing one within a script corresponds to the document creation. A document is made up of a hierarchy containing objects, their properties and the features they own. An action script reflects this object hierarchy.
Example
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In the script opposite, the inputs and the published parameters (2) of the instantiated UDF "Hole_UDF" (1) are nested between braces {}.
Object Properties
• • • An object is created by default with some property values. These properties are defined or re-defined within the braces just following the object declaration (isa keyword). Unless otherwise specified, the units are IS units. When defining properties, the semicolon ; is a terminator (see example below). The properties might be object attributes (1), attributes needed to define a type displayed in the Object browser (2) or aggregated objects (3).
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In the script above, the properties are the inputs of an instantiated UDF.
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In the script above, the properties are the attributes required to create a point to point line.
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In the script above, the Pad object is aggregated below the OpenBodyFeature object.
Keywords
• • • • • isa keyword context keyword from keyword import Keyword publish keyword
isa Keyword
Definition
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knowledgewareAdvisor Enables you to create a typed object or instantiate an object. Syntax • or • where: • • • ObjectName is the name of the object to be created. ObjectType is the type of the object to be created. InstanceName is the name of the object to be instantiated. ObjectName isa InstanceName ObjectName isa ObjectType
Example import "E: GPS.CATPart"; myGps isa CATPart { myPart isa Part { PartB isa BodyFeature { S0 isa Sketch.0 {} //Instance name pad0 isa Pad("S0") //Object type } } }
context Keyword
Definition Enables you to define in which part of the specification tree the object will be created. The context keyword may be of use in 2 different cases: • It can indicate a context "Mypart.CATPart" document to be used. In MyPart isa Part { } this case, the "..." are used.
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It can reference an object contained in the document. In this case the path needs to be specified (between `...`).
context `My.CATPart CC isa Cylinder { }
MyPart
PartBody`
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or • context `My.CATPart MyPart PartBody`
from Keyword
Definition Allows you to copy a document from an existing document without maintaining any link. Syntax DocumentName isa DocumentType from FilePath where: DocumentType is either CATProduct, CATPart or model. FilePath is the full path of the initial document. To enter a file path you can: Use the Insert File Path command from the contextual menu Example See Defining the Context
import Keyword
Definition Specifies a document file (.CATPart or .CATProduct) containing definitions to be reused or redefined in the document to be generated. All the features and feature values in the imported file become available to the document to be generated. Importing a document is: • Of interest whenever you want to retrieve a consistent set of definitions from an already existing document (for a UDF definition for example.) • Required whenever you need to create a feature from a sketch (the script language does not allow you to specify a sketch).
Syntax There are 2 ways to specify the file path:
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knowledgewareAdvisor • import "File path"; : Indicate the path of the file to be imported: import "E: users kwecx Models PartImport.CATPart" ;. Note that you should enclose the path within quotation marks and end the import statement with a semicolon (;). import "File Name"; : Indicate only the name of the file to be imported if this file is located in the same directory as the document containing the loop: import "PartImport.CATPart";. Note that: You should enclose the document name within quotation marks and end the import statement with a semicolon (;). The file to be imported should be located in the same directory as the document containing the loop. The document containing the loop should be saved.
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To specify a file to be imported, you can use the 'Insert File Path' command from the contextual menu. Selecting this command displays a file selection window. Quotation marks are automatically included but not the semicolon. Example
publish Keyword
Definition Enables you to assign an object a name that will be used in the script. Syntax publish "!xxx" as yyy ; Where: • xxx is the name of the object to be published. To select this object, it is highly recommended to use the contextual menu.
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Example Publi isa CATProduct { Publi isa Product { P isa Product { P1 isa Part { PartBody isa Feature { Pa isa Pad{} } } publish "Publi/P/!Selection_RSur:(Face:(Brp:(Pa;2);None:());Pa)" as mypadface; /*publishes the face of a pad under the name "mypadface"*/ } Q isa Product { Q1 isa Part { PartBody isa Feature { Cy isa Cylinder{} } } publish "Publi/Q/!Selection_RSur:(Face:(Brp:(Cy;2);None:());Cy)" as mycylinderface; //publishes the face of a cylinder under the name "mycylinderface" } assembly constraints: contact("P } } toto","Q tutu");
Variables
Variables are declared explicitly in your script. These variables are displayed as parameters in the specification tree.
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ALPHA = 45 deg;
Unlike in most script languages, a variable scope is not really determined by where you declare it. From anywhere in your action script, you can access a variable by using the .. .. and ? operators. After the script is finished running, the variable declared in your script still exists as a document parameter.
Operators
Arithmetic operators
+ Addition operator (also concatenates strings) - Subtraction operator * Multiplication operator / Division operator ( ) Parentheses (used to group operands in expressions) = Assignment operator
? (Question Mark in Formulas)
Definition In a formula, specifies that the parameter value to be applied is the first parameter value found when scanning the specification tree from the formula to the top of the specification tree. Sample KwrLoopRelativePath.CATPart
(Relative Path in Formulas)
Definition Defines where the value of a parameter used as an argument in a formula is to be read. A single.. exits the statement block where the formula is defined. The
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User Tasks parameter value applied in the formula is then the one defined in the parent feature scope. Sample KwrLoopRelativePath.CATPart
Using The Get... Commands
The commands described in this section are the ones you can access when using the Loop Editor and right-clicking in the Editor window. When creating a loop containing the path of a feature contained in the specification tree, it is highly recommended to use the Get Feature command to retrieve the internal name of this feature. • • • • • Using Using Using Using the the the the Get Get Get Get Axis Command Edge Command Surface Command Feature Command
Using the Insert File Path Command
The 'Get Axis' Command
This task explains how to create a chamfer by using the Get Axis command. This command enables you to interactively capture the generic name of an axis and to insert it into the script instead of keying it in. 1. Click the Loop icon ( ) and enter 1 in the To field.
2. In the Script Editor, enter the following script and click OK. A pad is created. myChamferDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad { } } } }
3. From the Window menu, select Cascade. 4. Under the P isa Pad block, add F isa Chamfer(){}, position the
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cursor between the parenthesis, then right-click to open the contextual menu and select the Get Axis command, and select an edge in your geometrical surface. The script should be as follows: myChamferDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad { } F isa Chamfer("Edge:(Face:(Brp:(P;0:(Brp:(Sketch.1;2))); None:());Face:(Brp:(P;0:(Brp:(Sketch.1;3)));None:()); None:(Limits1:();Limits2:()))"){} } } } 5. Click the OK button. The chamfer is created.
The "Get Edge" Command
This task explains how to create a chamfer by using the Get Edge command. This command enables you to interactively capture the generic name of an edge and to insert it into the script instead of keying it in. 1. Click the Loop icon ( ) and enter 1 in the To field.
2. In the Script Editor, enter the following script and click OK. A pad is created. myChamferDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad { } } } }
3. Under the P isa Pad block, add F isa Chamfer(){}, position the cursor between the parenthesis, then right-click to open the contextual
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menu and select the Get Edge command, and select an edge in your geometrical surface. The script should be as follows: myChamferDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad {} F isa Chamfer("Edge:(Face:(Brp:(P;0:(Brp:(Sketch.1;2))); None:());Face:(Brp:(P;2);None:());None:(Limits1:();Limits2:()))"){} } } } 4. Click the Generate button. The chamfer is created.
The "Get Surface" Command
This task explains how to create a sketch on an existing face by using The Get Surface command. This command enables you to interactively capture the generic name of a surface and to insert it into the script instead of keying it in. 1. Open the KwrGetSurface.CATPart file. 2. Access the Knowledge Advisor workbench, and click the Loop icon. Enter 1 in the To field 3. Enter the following script: import "f: cube.CATPart"; myFaceDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad{} S isa Sketch.1() 4. Position the cursor between the two parentheses of the last line of the above script, right-click to open the contextual menu and select the Get Surface command. 5. Select the face whose name you want to capture. The full name is inserted at the cursor location. Enter the end of your script. In our example, the final script is as follows: import "f: PktGetSurface.CATPart";
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myFaceDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad{} S isa Sketch.1("Face:(Brp:(P;0:(Brp:(Sketch.1;2)));None:())") { } } } } 6.
The "Get Feature" Command
This task explains how to use the Get Feature command. This command enables you to interactively capture the generic name of a surface and to insert it into the script instead of keying it in. In the task below, you are going to generate a line. 1. Open the KwrGetFeature.CATPart file. 2. Double-click the loop located below the Relations node and insert the following code into the editor: Line_Pt_Pt isa GSMLine { LineType = 0; TypeObject isa GSMLinePtPt { FirstPoint = object: // Using GetFeature to Select the FirstPoint (Point.10) SecondPoint = object: // Using GetFeature to Select the SecondPoint (Point.7) } } 3. 4. Position the cursor after FirstPoint = object: and select the Get Feature command in the contextual menu. 5. Click a point in the geometry (Point.10 for example) and add a semi-colon (;) at the end of the line. 6. Position the cursor after SecondPoint = object: and select the Get Feature command in the contextual menu. 7. Click another point in the geometry (Point.7 for example) and add a
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semi-colon (;) at the end of the line. Your script should now look like the one below:
8. Click OK. A new line is generated. 9.
The 'Insert File Path' Command
This task explains how to use the Insert File Path command. This command is one of the methods you can use to specify a path in a script. When writing a script, you have to specify a file path when you import a file, see the import keyword. 1. Access the Script Editor and enter any instruction requiring a file path specification (import in the example below). 2. Position the cursor where the path is to be specified.
3. Right-click and select the Insert File Path command from the contextual menu.
4. In the dialog box which is displayed, select the appropriate file. Click Open to go back to the script editor. 5. The full path is inserted at the cursor place. Check that the statement is ended by a semi-colon.
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Comments
Multi-line comments (/* ... */) are supported. A single-line comment begins with a pair of forward slashes(//). Note that DBCS characters are not supported as comment.
Example
Sphere1 isa Sphere // Creates a sphere { // Valuates the Radius property Radius = 15.0 ; }
Limitations
You should be aware of some restrictions: • Instances of sketch-based features cannot be moved apart from their prototype. • Any parameter used as an argument in a formula should be preceded by the ? symbol. The syntax X = 2 * Y is invalid and should be replaced with X = 2 * ? Y. Unless a formula-defined parameter has not been initialized with the proper units, the value calculated from the formula is dimensionless. Y = 0 kg ; Y=2*?X; A script error stops the reading and the execution of the loop.
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Declaring Input Data
The Input Data are the data that will be used in the body of the loop and potentially be changed when instantiating the loop. To select them, click them in the specification tree or in the geometry.
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The Input Name field enables you to change the name of the input.
Note that the input can be a list made up of strings. It allows to instantiate features whose types are defined by the list items. To get an example see the following files: • • KwrPartUDFs.CATPart: This file contains the 4 UDFs definitions. KwrInstantiateUDFs.CATPart: This file contains the loop that instantiates the features. The inputs of the loop are made up of 2 lists. The first list contains parameters of String type (the names of the UDFs to be instantiated). The second list contains parameters of Length type (to valuate the UDFs published parameters: PosX).
Defining the Context
To create a loop, you need to define the context, that is to say the object (PartBody, Geometrical set, Pad, Relations, Parameters node or any feature) that will contain the items created by the loop. There are 3 different ways to define the context.
Using the Context field
To define the context of the loop, you may use the Context field of the Loop edition window. To do so, click the Context field, and select an object in the specification tree. In the picture opposite, a pad was selected in the specification tree.
Using an existing Document
It is possible to use an existing .CATPart or .CATProduct document.
Using the context keyword
When creating elements that need to be located in different bodies, you can change the context you defined in the Context field and use the Context keyword to define new contexts in the loop body.
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The action script should not start with the context keyword since the first context is defined in the Context field. Sample: KwrLoopMulticontext.CATPart (to launch the loop, activate the loop.)
Solving a Set of Equations
Solving a Set of Equations
This task explains how to solve a set of equations using the operators and functions of the knowledgeware language. This scenario can be run from any document. • • In a set of equations, the semi-colon (;) is used as a separator. Note that the equations set capabilities require the Knowledge Advisor product.
Note that a KWA license is required to execute loops.
1. Create two real type parameters x and y. Both parameters are intended to be used as variables in a se equations.
icon. In the first dialog box which is displaye 2. Access the Knowledge Advisor workbench. Click the enter the name of the relation, a comment and a destination. Then click OK. The Set Of Equations edi is displayed. 3. Enter the set of equations below into the edition box: y - 2 *sqrt(x) ==2; y - 4 *x*x == 0 Now, your editor looks something like this:
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The value of each parameter is display first in the Unknown parameters field, the in the specification tree (see below).
4. Click here to open the result file. To find out more about the Equations Editor, see Using the Equations Editor.
Using the Equations Editor
In order to improve the use of the Equations solving functions, the Equation Editor was modified. It is made up of two tabs: the Editors tab and the Options tab.
Editors tab
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The Parse arrow is used to identify the variables of the set of constraints. It must be pushed before choosing input and output variables. The left arrow is used to move variables from the Unknown parameters category to the Constant parameters one. The right arrow is used to move variables from the Constant parameters category to the Unknown parameters one. The Switch input/output arrow is used to swap the selected constant and unknown parameters. • • • • • Viewer: enables you to enter the equations that you want to solve. Dictionary: see Using the Rule Editor. Members of Parameters: see Using the Dictionary. Members of All: see Using the Rule Editor. Constant parameters: Constant parameters: The value of constant parameters are set by you and are considered as constants by the solver. This value can be changed directly in the Value column by clicking twice (slowly) in the Value cell. Unknown parameters: The value of unknown parameters will be calculated once the Apply button is pushed.
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Options tab
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Algorithm • Precision: enables you to define the precision of the results (i.e the number of decimal digits after the decimal point.) Use the Gauss method for linear equations: accelerates the solve operation when working with linear equations.
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Termination criteria • Maximal computation time (sec.): enables you to indicate the computation time. If the indicated time is equal to 0, the computation will last until a solution is found. Show 'Stop' dialog: if checked, displays a "Stop" dialog box that will enable you to interrupt the computation.
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Solving a Set of Equations
Using the Knowledge Advisor Language
Using the Knowledge Advisor Language
• Writing Formulas - Rules & Checks - Overview o o o Conditional Statements For Statement While Statement
• • • • • • •
Constants Comments Temporary Variables Units Operators Object Methods Messages and Macros
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Writing Formulas
A formula is a one-line statement that you can write either by typing directly the appropriate syntax in the editor field or by selecting items from the editor dictionary list. The formula syntax is easy to use and learn. The period is generally used as a separator between the whole numbers and the fractional part of a number. Using a comma as a separator in place of the period is not recommended in real values intended to be used directly in relations. Example: Real1 = 2,1 + 5,4 is not allowed whereas Real1 = Real2 + Real3 is allowed regardless of the separator used when valuating Real2 and Real3.
Writing Rules and Checks
Rules and checks are multi-line statements that you can write either by typing directly the appropriate syntax in the editor field or by selecting items from the editor dictionary list. Here is a description of the syntax to be used. The mathematical and trigonometric functions as well as the functions used to manipulate strings are the same as for formulas.
Conditional Statements
Rules
if ... else ... else if Conditionally executes a group of statements, depending on the value of an expression. You can use either block form syntaxes:
if condition statements [else elsestatements ] or
if condition { statements } [else if condition-n [ { elseifstatements } ] ] . . . [else [ { elsestatements } ] ]
You can use the single-line form (first syntax) for short, simple rules. However, the block form (second syntax) provides more structure and
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User Tasks flexibility than the single-line form and is usually easier to read, maintain, and test. The else and else if clauses are both optional. You can have as many else if statements as you want below a block if, but none can appear after the else clause. Block if statements can be nested that is, contained within one another.
Checks
statement1 => statement2 (if statement1 then statement2) Displays a message (if type is Warning or Information) and turns to red in the specification tree each time statement2 is invalid as statement1 is fulfilled. OK => KO KO => KO KO => OK OK => OK
For Statement
Note that the For statement is available for Action and Reaction scripts only. The first type of loop is a loop based on the element of a list. See syntax opposite. Where: • • • X is a variable name (of a given type. It may represent an object or a value). List is a variable name of type List or an expression returning a list. X (like any other variable of the language) can be used in the body. It contains the Nth element of the list. For x inside List { Body }
The body is executed Nth times where N is the number of elements of the list. The second type of loop executes until an expression becomes false. See syntax opposite. Where: • • X is a variable name of integer type. It is incremented at the end of each execution of the body. Predicate is a Boolean expression. The body is executed as long as this expression is true. This For x while predicate { Body }
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expression is evaluated before the body. Note that the second for operator can lead to infinite loops.
While Statement
This loop executes until an expression becomes false. See syntax opposite. Where: • • i is a variable name of integer type. It is incremented at the end of each execution of the body. X is a variable for points. let i = 1 let x(Point) for i while i<=parameter.Size() { x = parameter.GetItem(i) if (x.GetAttributeReal("Y") < 0.04) x.SetAttributeReal("Y",0.04) }
Constants
The following constants are specified or recognized by CATIA when programming rules and checks. As a result, they can be used anywhere in a relation in place of the actual values. • • • false - one of the two values that a parameter of type Boolean can have true - one of the two values that a parameter of type Boolean can have PI - 3.14159265358979323846 - The ratio of the circumference of a circle to its diameter. E - The base of natural logarithm - The constant e is approximately 2.718282.
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Comments
The /* and */ comment characters are supported.
/* Rule created by CRE 05/03/99 */ if PartBody { Sketch.1 Radius.3 Radius > 45mm
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Temporary Variables
Temporary variables can be declared by using the let keyword. A temporary variable does not persist as a parameter after the rule execution is finished.
/*Rule created by CRE 08/23/99*/ let x = 5 mm if PartBody { PartBody } For non digital values, the type has to be indicated: let S(Surface) S= split (...,...) Temporary variables should be declared at the beginning of the rule, before any conditional instruction is specified. let S1(Surface) let S2(Surface) let S3(Surface) S1 = Split ... S2 = ... S3 = ... Hole.1 Activity = false Hole.1 Diameter > x
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Units
Units are all provided in the dictionary. 1. Pay attention to unit consistency when writing a rule or a check. 2. Units are written with an underscore instead of the usual "/" (example N_m2 instead of N/m2).
Operators
Arithmetic operators
+ Addition operator (also concatenates strings) - Subtraction operator * Multiplication operator / Division operator ( ) Parentheses (used to group operands in expressions) = Assignment operator ** Exponentiation operator
Logical Operators
and Logical conjunction on two expressions or Logical disjunction on two expressions
Comparison Operators
<> Not equal to == Equal to >= Greater or equal to <= Less than or equal to < Less than > Greater than
Object Methods
Description
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Attributes
ID Name UserInfoComment Owner NamedURLs
Methods
• List.1 is the name of the list on which the calculation will be performed. PartBody is the body on which the search will be carried out Hole is the Type. x.Diameter>50mm is the expression.
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• •
AbsoluteId Method GetAttributeInteger GetAttributeString ID Method IsOwnedBy Method IsSupporting Method Query Method SetAttributeBoolean SetAttributeString
AttributeType Method GetAttributeBoolean GetAttributeReal HasAttribute IsOwnedByString Method Name Method SetAttributeInteger SetAttributeReal
Example
1. Create a part with several holes. 2. Add a real type parameter ("Real.1" for example) to one of the hole features. To do this, you must use the Knowledge Advisor product. 3. Create the rule below: /* This rule resets the diameter of the hole */ /* which has "Real.1" as its parameter to the Real.1 value */ (for all) H:Hole if H->HasAttribute("Real.1")
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knowledgewareAdvisor H.Diameter = 1mm*(H->GetAttributeReal("Real.1")) You can use all the GetAttributexxx methods in that way. • • Add one or more drafts to the part. You can write the rule below: (for all) Dr:Draft /* Displays the names of the Drafts which have PartBody as their names */
See also: Using the Dictionary
Attributes
Id Defines the feature identifier, i.e. the name primarily assigned to the feature at creation before any renaming has been done. Owner Defines the parent feature. Name Defines the feature name. NamedURLs Describes the URL that the user can add to a relation by clicking the Comment and URLs icon in the Knowledge Advisor workbench. UserInfoComment Describes the comment that the user can add in the Comment and URLs dialog box when adding a URL to a relation in the Knowledge Advisor workbench.
Object Methods
AbsoluteId Method GetAttributeInteger Method HasAttribute Method IsOwnedByString Method SetAttributeBoolean
AttributeType Method GetAttributeReal Method Id Method IsSupporting SetAttributeReal Method
GetAttributeBoolean Method GetAttributeString Method IsOwnedBy Method Name Method SetAttributeInteger Method
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Method
SetAttributeReal Method
SetAttributeString Method
SetAttributeDimension
AbsoluteId Method
Retrieves the path of a feature. Note that this feature is not NLS (it will not be translated into your language and remains in english.)
Syntax
feature.AbsoluteId(): String
Example
String.2=PartBody
Sample
Pad.1.Id() + PartBody
Pad.1.AbsoluteId()
KwrTopology.CATPart
AttributeType Method
Returns the attribute type in the form of a string.
GetAttributeBoolean Method
Returns the value of a boolean type parameter added to a given feature by using the Knowledge Advisor product. parameterName is the name of the boolean type parameter. It should be put between quotation marks (").This method enables you to read: • • •
Syntax
The attributes added to parameters using the Parameters Explorer. The real attributes added to objects. The User Properties of a product.
feature.GetAttributeBoolean(String): Boolean where the argument is name of the attribute.
Example
Message ("The value of the Boolean.1 attribute of # is #", PartBody PartBody Pad.1.Name(), Pad.1.GetAttributeBoolean("Boolean.1"))
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Sample
KwrObject.CATPart
GetAttributeInteger Method
Returns the value of an integer type parameter added to a given feature by using the Knowledge Advisor product. parameterName is the name of the string type parameter. It should be put between quotation marks ("). This method enables you to read: • • •
Syntax
The attributes added to parameters using the Parameters Explorer. The real attributes added to objects. The User Properties of a product.
feature.GetAttributeInteger(String): Integer where String is name of the attribute. This name should be put between doublequotes.
Example
Integer.3=PartBody
Sample
Hole.1 .GetAttributeInteger("Integer.2")
KwrObject.CATPart
GetAttributeReal Method
Returns the value of a real or Length (in m) type parameter added to a given feature by using the Knowledge Advisor product. parameterName is the name of the string type parameter. It should be put between quotation marks ("). This method enables you to read: • • •
Syntax
The attributes added to parameters using the Parameters Explorer. The real attributes added to objects. The User Properties of a product.
feature.GetAttributeReal(String): String where String is name of the attribute. This name should be put between doublequotes.
GetAttributeString Method
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User Tasks Returns the value of a string type parameter added to a given feature by using the Knowledge Advisor product. parameterName is the name of the string type parameter. This method enables you to read: • • •
Syntax
The attributes added to parameters using the Parameters Explorer. The real attributes added to objects. The User Properties of a product.
feature.GetAttributeString(String): String where String is name of the attribute. This name should be put between doublequotes.
Example
String.2 =PartBody
Sample
Pad.1 .GetAttributeString("String.1")
KwrObject.CATPart
HasAttribute Method
Determines whether the attribute specified in the argument belongs to the feature the method is applied to.
Syntax
feature.HasAttribute(String): Boolean where String is name of the attribute. This name should be put between doublequotes.
Example
Boolean.2 = PartBody
Sample
Hole.1.HasAttribute("Real.1")
KwrObject.CATPart
Id Method
Applies to a feature. Retrieves the identifier of a feature.
Syntax
feature.Id(): String 221
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Example
String.2=PartBody Pad.1.Id() + PartBody Pad.1.AbsoluteId()
Sample
KwrTopology.CATPart
IsOwnedBy Method
Determines whether the feature specified in the argument is the parent of the feature the method is applied to. featureName should be put between quotation marks (").
Syntax
feature.IsOwnedBy(): Boolean
Example
Boolean.1=PartBody
Sample
Hole.1.IsOwnedBy(PartBody)
Topology.CATPart
IsOwnedByString Method
Applies to a feature. Determines whether a feature belongs to another. This method returns a string.
Syntax
feature.IsOwnedByString(): Boolean
IsSupporting
Function indicating if the object passed in argument is supported or not.
Example
H:Hole H->IsSupporting("TaperedHole") == true
Name Method
Applies to a feature. Retrieves the name of a feature. Cannot be used to rename a feature.
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Syntax
feature.Name(): String
Example
String.1=PartBody
Sample
Pad.1.Name()
KwrTopology.CATPart
SetAttributeBoolean Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the boolean type parameter whose value is to be modified. It should be put between quotation marks ("). booleanvalue is either TRUE or FALSE.
Syntax
feature.SetAttributeBoolean(String, Boolean): Void where the first argument is name of the attribute while the second is the value to be assigned to it.
Example
if PartBody PartBody
Sample
Pad.1
Boolean.1 <> true
Pad.1.SetAttributeBoolean("Boolean.1", true)
KwrObject.CATPart
SetAttributeReal Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the real type parameter whose value is to be modified. parameterName should be put between quotation marks (").
Syntax
feature.SetAttributeReal(String, Real): Void where String is name of the attribute and Real the value to be assigned to the parameter.
Example
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if PartBody PartBody
Sample
Hole.1
Real.1 <> 3
Hole.1 .SetAttributeReal("Real.1",3)
KwrObject.CATPart
SetAttributeString Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the string type parameter whose value is to be modified. parameterName and stringvalue should be put between quotation marks (").
Syntax
feature.SetAttributeString(String, String): Void where the first argument is name of the attribute while the second is the value to be assigned to it.
Example
if PartBody PartBody
Pad.1.GetAttributeString("String.1") <> "String1" Pad.1 .SetAttributeString("String.1","This is a test")
Another syntax for the same rule is: if PartBody PartBody
Sample
Pad.1
String.1 <> "String1"
Pad.1.SetAttributeString("String.1","This is a test")
KwrObject.CATPart
SetAttributeInteger Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the integer type parameter whose value is to be modified. parameterName should be put between quotation marks (").
Syntax
feature.SetAttributeInteger(String, Integer): Void where the first argument is name of the attribute while the second is the value to be assigned to it.
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Example
if PartBody PartBody
Sample
Hole.1
Integer.1 <> 3
Hole.1 .SetAttributeInteger("Integer.1", 3)
KwrObject.CATPart
SetAttributeDimension Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the parameter whose value is to be modified. parameterName should be put between quotation marks ("). The unit used is the current one.
Syntax
feature.SetAttributeDimension(String, Real, String): Void Type where the first argument is name of the attribute, the second is the value to be assigned to it and the third is the type.
Example
H:Hole H->SetAttributeDimension("Myhole",5,"Length")
Messages and macros
LaunchMacroFromDoc Function Question Function LaunchMacroFromFile Function VBScriptRun Message Function
LaunchMacroFromDoc Function
Executes a macro stored in a document from a rule. A macro is stored in a document when you don't specify any external file before recording it. Warning: It is up to you to check that the macro which is run is not going to cause an infinite loop or result in a system crash.
Syntax
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knowledgewareAdvisor LaunchMacroFromDoc(MacroName)
Example
LaunchMacroFromDoc("Macro1")
Question Function
Displays a message in a dialog box, waits for you to click a button and returns a value indicating which button you clicked (true if Yes was clicked, false if No was clicked)
Syntax
Question(String [# String1 # String2 ..., Param1Name, Param2Name, ...] ): Boolean The Question function takes one required argument and several optional arguments depending on whether parameter values are to be displayed in the message. Arguments String # String1, Param1Name... Description Required. String to be displayed in the dialog box (should be put in quotes). Optional. When parameter values are to be displayed within the message, the arguments should be specified as follows: • one string in quotes including a # symbol wherever a parameter value is to be displayed as many [, parameter name] statements as parameter values declared with a "#" in the message.
•
Use the "|" symbol to insert a carriage return in a prompt.
Example
Boolean2 = Question("SketchRadius is # | Do you want to change this value ?", PartBody Sketch.1 Radius.3 Radius )
Note that you can use the Question function together with the BuildMessageNLS function for your question to display in your language. To
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use this function, use the following syntax: question(BuildMessageNLS ("x","xx",a,b)) • • • x corresponds to the name of the CATXXX.CATNls file where you will find the NLS message (it is the CATXXX name without the CATNls extension). xx corresponds to the key name in this catalog. a and b are the arguments (values that will be replaced in the message)
LaunchMacrofromFile Function
Executes a macro CATScript from a rule. Warning: It is up to you to check that the macro which is run is not going to cause an infinite loop or result in a system crash.
Syntax
LaunchMacroFromFile("MacroName.CATScript" )
Example
LaunchMacroFromFile("Macro1.CATScript")
Run Method
Runs a macro with arguments. Warning: It is up to you to check that the macro which is run is not going to cause an infinite loop or result in a system crash.
Syntax
VB Script.Run(valueOrFeature:ObjectType,...): Void where valueOrFeature is the macro argument name. There can be several arguments.
Example
You must have created the VB Script.1 macro prior to creating the rule below: if PartBody Pad.1.HasAttribute("String.1") == true Pad.1 Pad.1.Name() )
`VB Script.1` .Run(PartBody
.GetAttributeString("String.1"),PartBody
Sample
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knowledgewareAdvisor KwrObject.CATPart
Message Function
Displays a message in an information box. The message can include one or more parameter values.
Syntax
Message(String [# String1 # String2 ..., Param1Name, Param2Name, ...] ) : Void The Message function takes one required argument and several optional arguments depending on whether parameter values are to be displayed in the message. Arguments String # String1, Param1Name... Description Required. String to be displayed in the information box (should be put in quotes). Optional. When parameter values are to be displayed within the message, the arguments should be specified as follows: • one string in quotes including a # symbol wherever a parameter value is to be displayed as many [, parameter name] statements as parameter values declared with a "#" in the message.
•
Use the "|" symbol to insert a carriage return in a message.
Example 1
Message("External radius is: # | Internal Radius is: #", PartBody PartBody Sketch.1 Hole.1 Radius.3 Diameter) Radius,
Example 2
Note that this function can be used along with the buildMessageNLS function Message (BuildMessageNLS("KwrCATCatalog.CATNls","Zero")) Where x,y,z are parameters.
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Note that you can use the Message function together with the BuildMessageNLS function for your question to display in your language. To use this function, use the following syntax: Message(BuildMessageNLS ("x","xx",a,b)) • • • x corresponds to the name of the CATXXX.CATNls file where you will find the NLS message (it is the CATXXX name without the CATNls extension). xx corresponds to the key name in this catalog. a and b are the arguments (values that will be replaced in the message)
Limitations
Parameters and Formulas
• • The output parameter (the one that is valuated) of a formula can not be a publication. The bypass is to use a rule. If you want to edit a formula located in another document (not the UI active one) in the Formula editor, a warning is displayed and the formula editor is grayed out.
Design Tables
When working with design tables in .xls format, the Undo command may not work properly.
Rules
• • Geometrical features valuated by a rule should not be used as the construction support of sub-elements. If you create a rule driving formulas activity, you might encounter update problems.
Sets of Equations
In set of equations, there is no control of units coherence (like in rule, check, formula).
Macros with Arguments
It is not possible to use the InputBox Visual Basic function in the definition of macros with arguments on unix. The SelectElement method on Selection object does not work either (on all Operating Systems).
Loops
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A loop can only generate items in the document it belongs to. So, in the graphic opposite, the loop cannot generate items in Product3. this restriction applies also to assemblies made up of different parts. A loop located in one of the Parts cannot generate items in another Part of the assembly.
Useful Tips
Relations
When using some objects, you need to indicate the destination of the formulas and the rules that valuate the parameters of these objects. If you valuate a time parameter in a kinematic simulation for example, the relation will not be located below the Relations set but in the mechanisms and commands tree of the simulation.
Hiding relations
You can hide a knowledge relation (formula, rule, check, ..) by right-clicking this relation in the specification tree and by selecting the Hide command. • A visual indicator located at the Relations set level indicates that the set contains hidden relations. Note that this indicator is not recursive. If you try to delete a relations set containing hidden relations, a message is displayed asking you if you want to delete the relations set that contains hidden relations. Note that if you try to delete a relations set containing another relations set with hidden relations, the message will be displayed.
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Relations Updates
The evaluation of relations containing measures can be integrated to the Part update only. In a .CATProduct or in a .CATProcess file, to create a parameter
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User Tasks • • which value is the result of a relation containing measures updated when modifying the measure inputs:
1. Create the relation containing the measure at the Part level. 2. Integrate the relation evaluation to the Part update. 3. At the Product or the Process level, create a relation that valuates the parameter by using the result parameter of the relation created at the Part level. To get an example, see KwrUpdate.CATProduct. 4. Perform a local update at the Relations level.
Syntax errors in relations message
When loading a document, the message opposite can appear. It means that during the load, some relations appeared as broken. These relations use functions that are not recognized by the dictionary because the library containing the definition of the function is not still loaded. That's why you are asked if you want to load all the libraries containing functions definition. But loading all libraries may have an impact on performances. So, we recommend you to load only the libraries you are interested by. To do so, select the required libraries in the Language tab (Tools>Options->General>Knowledge->Language.)
Rules
Geometrical Features and Rules
In a rule using features that need the geometry to return the type (such as extrudes), when the feature is deactivated, the type cannot be returned. To solve the problem, use the Set command to indicate the type in the rule. To know more, see the KwrSetType.CATPart file.
Rules and Update Cycle
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This configuration is allowed since a modification of the parameter activity does not impact the formula update. But: • • • In such a case, it is highly recommended to use the reaction feature. If you want to use a rule, do not deactivate and reactivate the activity parameter. When working with a UDF feature, make sure that you have inserted the relation set when defining the UDF.
Parameters
• You can add properties to a .CATPart or a .CATProduct document by using the Properties command from the contextual menu. You just have to click the Define other properties... button in the Product tab then click New parameter of type. The dialog is similar to the f(x) dialog. See the Product Structure User's Guide for more information. The properties you define that way are also displayed in the parameter list of the f(x) dialog box. Parameters belonging to a parameter set can be reordered by using the Reorder... command from the contextual menu. Parameters added by using the Parameters Explorer are displayed right below the feature they are assigned. CATIA users working with non-latin characters should check the Tools>Options>Knowledge->Parameter Names->Surrounded by' option. Otherwise, parameter names should have to be renamed in latin characters when used in formulas. You can specify that a parameter is constant by using the Properties command from the contextual menu. This command also enables you to hide a parameter. When copying parameters sets containing hidden parameters, these parameters are automatically pasted when pasting the parameters sets and appear as hidden parameters. Parameters have 2 different names: The local one and the global one. o The local name is the name attributed to the parameter when it was created in the Formula Editor or in the Parameters Explorer. Note that this name will not be modified if you perform a Reorder using the contextual menu.
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•
•
• •
•
This name can be modified using the Parameters Explorer and the Edit>Properties command. o The global name (name) is the name attributed to the parameter by Knowledge Advisor. It is the path of the parameter + its type. If you select
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the parameter and reorder it, the path contained in the name will be modified. If you double-click the parameter in the specification tree, and enter a new name in the Edit Parameter dialog box, the global name will be changed. If, after renaming the parameter in the Edit Parameter dialog box, you reorder the parameter the path will not appear any more. This name can be modified in the Edit Parameter dialog box. • • When renaming parameters using the Edit->Properties command, do not apply names similar to the parameters types available in the Formula Editor. For example, if you rename a Length parameter into Time, the name will be converted into Time.1. Deleting parameters used in a relation: If you delete a parameter used in a relation, a "clone" parameter will be created. Applying the same formula to several parameters: If you want to apply the same formula to several parameters, use the Equivalent Dimensions feature and value this feature by a formula. To know more, see Using the Equivalent Dimensions Feature.
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•
Formulas
• The Incremental option of the formula editor :The Incremental option allows you to restrict the list of parameters displayed in the dictionary. Select a feature either in the tree or in the geometry area. Only the first level of objects right below the selected feature will be displayed in the dictionary. If the Incremental option is unchecked, all the objects below the selected feature are displayed. The Incremental mode is useful when you work with large documents and when the parameter lists are long. Tips about the formula editor: To help you write a formula, the formula editor provides you with a dictionary. This dictionary exposes the list of parameters and functions you can use to define a formula. Depending on the category of objects to be referred to in the formula, the dictionary is divided into two or three parts. To insert any definition in the formula editor, just double-click the object either in the dictionary or in the tree. If you doubleclick a function in the dictionary, its signature is carried forward to the formula editor. Only the argument definitions are missing.
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Design Tables
• A design table can only be created from non-constrained parameters, i.e.
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knowledgewareAdvisor from parameters which are neither referred to in an active design table nor used in any other active relation. If you keep the Activity option checked for DesignTable0 and you try to create another design table, you will have to select the parameters to add to your second design table among a restricted parameter list. Uncheck the Activity option if you want to deactivate a design table and reuse its parameters in another design table.
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Anytime you modify a design table, the relations that refer to this design table detect the modification and turn to a to-be-updated status.
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As long as a design table is active, the parameters which are declared in it are constrained parameters and you are not allowed to modify them. Double-clicking a design table in the specification tree displays the design table with its set of configurations and allows you to select a new configuration.
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Only parameters which are not already constrained by any other relation or by any other design table can be used to create a design table. If a parameter is already constrained, it does not appear in the Parameters to insert list in the design table dialog box.
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Selecting the parameters to be inserted in a design table The Filter Name and Filter Type filters can be used to restrict the display of a parameter list. If you specify x in the Filter Name field of the Select parameters to insert dialog box, you will display all the parameters with the letter x in their name (xA, xB, xC, xD, xE). If you select the Renamed Parameters in the Filter Type list, you will display all the parameters you have renamed in the Formulas dialog box (yA, xB, xA, yC, xC, yB, yD, xD, yE, xE, TangE). Parameters to be inserted can be multi-selected. You just have to keep on pressing the Ctrl key while you select parameters. If you do this, the group of multi-selected parameters will be carried forward onto the Inserted parameters list in the order in which they are displayed in the initial list. When the design table is created, the rank of the columns fits the rank of the parameters in the Inserted parameters list. If you want to have columns ordered in a given way in the design table, you must insert the parameters one by one.
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Accessing the functions related to the design table Once in the formula (rule or check) editor, select the Design Table item in the dictionary, the list of the methods that can be applied to a design table is displayed. Select a method, then click F1 to display the associated documentation.
Loops
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User Tasks
•
Generic Naming: Generic naming is a CATIA technique which creates a label whenever an element has been selected interactively. This label is a coded description of the selected element. When you specify a fillet to be applied to a face, you must select interactively the face definition but prior to doing this you must of course have generated the face to be filleted. This is why scripts requiring face, point or edge definitions cannot be generated in one shot. You don't have to mind about the generic naming itself as it is automatically captured from the geometry area. The thing you have to mind about is the order your instructions are to be written and executed in the script. Message "property does not exist...": Check in the browser that the attribute name is correct. For attributes of list type (Fillets and Chamfers), check the indexes. The indexes specified must be consecutive from 1 to n without any gaps. Specifying a File Path (2 methods)
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• Syntax
There are 2 ways to specify the file path: • import "File path"; : Indicate the path of the file to be imported: import "E: users kwecx Models PartImport.CATPart" ;. Note that you should enclose the path within quotation marks and end the import statement with a semicolon (;). import "File Name"; : Indicate only the name of the file to be imported if this file is located in the same directory as the document containing the loop: import "PartImport.CATPart";. Note that: o You should enclose the document name within quotation marks and end the import statement with a semicolon (;). The file to be imported should be located in the same directory as the document containing the loop. The document containing the loop should be saved.
•
o
o
To specify a file to be imported, you can use the 'Insert File Path' command from the contextual menu. Selecting this command displays a file selection window. Quotation marks are automatically included but not the semicolon • Importing Sketches: Recommendation
When designing a document to be generated by a script, it is better to group all the required sketches in a single file. That way: • you minimize the overall size of your sketch-related data • no matter the method used to specify the input file, you just have to specify
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the path once • the design of the final document is made easier. You get a global view of the sketches on which the other features rely. Specifying Strings: Recommendation: Double quotation marks as well as single quotation marks of apostrophe type (`) can be used to delimit strings. Single quotations marks (`) must be used to enclose character strings which contain other strings.
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Reactions
There are 2 ways to react to parameter changes using the reaction feature: • Or • Select the feature (that owns the attribute corresponding to your parameter) and react to the Attribute Modification event. Note that this method does not work in all cases. Select the parameter and react to its Value Changed event
Use Cases
Use Cases
Link Bar 5
The Ball Bearing
The Ball Bearing
A bearing is defined by parameters such as its principal dimensions, its basic load ratings, its limiting speeds and its mass. It belongs to a category which corresponds a certain range of its parameter values. In a catalogue, a bearing is referred to by a designation. Bearing types are described by tables which define the bearing parameter values including the designation. The bearing example has been chosen here because the bearing tables given in distributor and retailer catalogues illustrate quite well the design table principles. The bearing itself is a good example of how components within a mechanical part can be constrained by relations. In the scenario below, you start from an existing document inspired by a deep groove ball bearing. This document contains already a number knowledgeware relations, others are added to control the document design.
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Link Bar 4
Before you Start
Here is the data required to perform the scenario. They are all delivered with the Knowledge Advisor product but can be rebuilt from the information given below. See the Infrastructure User's Guide for how to specify the material library settings (you must use the Tools->Options...->Infrastructure->Material Library command from the standard menu bar).
The Initial Document
The initial document is the KwrBallBearing1.CATPart document.
The bearing rings are coaxial shafts created from the Sketch.1 and Sketch.2 features. The balls are shafts created from the Sketch.3 feature.
The Outer Ring
The outer ring is a shaft generated by rotating the Sketch.1 highlighted in figure below around an axis coaxial to V. Note that you must create this axis as a construction element, otherwise CATIA won't let you create the Shaft. The lower part of the sketch is the symmetry of the upper part with respect to the H axis.
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Here are the constraints defined on this sketch: d1 L1 B1 R1 b1 D1 2.1 mm 3 mm 5 mm ring width half height of the non - hollowed inner surface half height of the outer surface
2.759 mm groove radius 0 mm 13 mm ordinate of the groove center external diameter
The Inner Ring
The inner ring is a shaft generated by rotating the Sketch.2 highlighted in figure below around an axis coaxial to V.
Here are the constraints defined on this sketch:
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d2 L2 B2 R2 b2 D2
2.1 mm 3 mm 5 mm
ring width half height of the non - hollowed inner surface half height of the outer surface
2.759 mm groove radius 0 mm 7.1 mm ordinate of the groove center internal diameter
The Balls
A ball is a shaft created by rotating half a circle (sketch.3) around the H axis. The circle must be closed before being rotated.
The parameters of the circular pattern which is created to build the set of balls are constrained by the formulas below: • BallNumber = int(3* D3 / BallRadius) • AngStep = 3.6deg / BallNumber D3 being the abscissa of the ball center.
The Import File
In the scenario, you have to import the text file below which is delivered under the KwrBallBearingImport.txt name.
Temperature 100Kdeg Pressure
Maximum temperature allowed
190N_m2 Maximum pressure allowed L1*D3*B1*0.005 required lubricant volume
LubricantVolume 0mm3
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If you modify this file, pay attention to the column format, use the Tab key to skip from one column to the other.
The Excel Table which Controls the Bearing Design
You must download the KwrBearingDesignTable.xls Excel table in your environment.
The CATScript Macro
The KwrBearing.CATScript macro just creates a circular pad. You can record this macro on your own in the Part Design workbench or use the one supplied with the KnowledgeAdvisor samples. When creating Rule.2 in your own environment, you should replace the pathname given as the argument of the LaunchMacroFromFile function with the pathname corresponding to the file where the macro has been downloaded.
Step-by-Step Procedure
Controlling the Bearing Design with a Design Table
A design table is created from a pre-existing file. The data set contained in this pre-existing file is quite similar to the data set which identifies a bearing in a catalogue. The design table which is created defines a number of configurations. Applying a new configuration results in a bearing modification. 1. Open the KwrBallBearing1.CATPart document. 2. Click the Design Table icon in the standard toolbar.
3. Check the Create a design table from a pre-existing file option. Click OK. 4. Select the KwrBearingDesignTable.xls file and associate automatically the design table columns with the document parameters (i.e. click YES in the "Automatic Associations?" dialog box). 5. In the Design table dialog box, select the configuration 3 (Line 3) and click Apply. Your ball bearing has changed. It is now a bronze bearing with 21 balls. You can tell the difference when you look at the geometry area. The bearing width is also modified. Click OK to exit the Design Table dialog box. 6. Keep your document open and proceed to the next task.
Creating a Check
A combined check using the => syntax is created. This check is intended to display a message whenever the check is not satisfied. 1. Access the Knowledge Advisor workbench
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icon then click OK in the first Check Editor dialog box. The 2. Click the check editor is displayed. 3. In the Check Editor, select the Warning type and enter the string "BallNumber is too small" in the message field. Then enter the D3 >= 6mm => BallNumber > 6 relation in the edition box. 4. Click OK to create your check and exit the editor. At this stage, no particular message is displayed. The check is added to the specification tree with a green icon. For the configuration 3 of the design table, this is the status of the check relations: OK => OK 5. In the specification tree, double-click the design table and select the configuration 1. Click OK. The message "BallNumber is too small" is displayed. For the configuration 1 of the design table, this is the status of the check relations: OK => KO 6. Keep your document open and proceed to the next task
Creating a Multiple Value Parameter
A multiple value parameter is created. Depending on this parameter value, a rule which is created in the next task will display either a message or launch a macro. 1. Click the icon.
2. In the Formulas dialog box, select String in the New Parameter of type list. Select Multiple values in the with list, then click 'New Parameter of type'. 3. In the Value List of String dialog box, enter one-by-one the step1, step2 and step3 values. Click OK. 4. In Edit name or value of the current parameter, replace the String.1 string with Status, then click OK. The Status parameter is added to the specification tree.
Creating a Rule
This task creates a rule which displays a message prompting you to import a file or launches a macro.
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1. In the specification tree, double-click the design table feature and select the configuration 3 in the table which is displayed. You are back to 21 ball bearing. 2. Access the Knowledge Advisor workbench 3. Click the icon.
4. Enter the Rule.2 string in the Name field of the first dialog box. Click OK. 5. Copy/Paste the code below into the rule edition box (modify the macro path):
if Status == "step2" Message("Import the KwrBallBearingImport text file") else if Status == "step3" LaunchMacroFromFile("e:/tmp/KwrBearing.CATScript") 6. Click OK to add the rule to the document and execute it. icon. In the "Formulas" dialog box, select the Status parameter 7. Click the and replace its step1 value with step2. Click OK. A message asks you to import the KwrBallBearingImport text file. 8. Click Import and select the KwrBallBearingImport.txt file. Three parameters are then added to the document. Click OK in the dialog box displaying the parameters and formulas to be imported. 9. Select the Status parameter and replace the step2 value with step3. Click OK. The KwrBearing.CATScript is executed and a circular pad is created.
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System of Three Equations in Three Variables
When designing a product, you may come across a system of equations to be solved. Whatever these equations (linear or not), CATIA provides you with resolution methods. These methods are the Simulated Annealing algorithm and the "SetOfEquations" capability. Can you use either method ? If your set of equations is purely mathematical, the answer is yes. Otherwise, no. The SetOfEquations capability cannot solve systems using CATIA functions such as measures. To solve a system of equations using measures, you must use the Simulated Annealing algorithm. The Simulated Annealing algorithm is provided with the Product Engineering Optimizer product. The set of equations is to be specified as constraints and the variables are to be specified as free parameters. This resolution method is quite good although sometimes a bit long and you can use it to solve a broad range of cases. The trick about this algorithm is to adjust the precision and the other algorithm parameters. The example developed below works well with both methods. Just to illustrate a system that cannot be solved by both methods, you can draw a cube and create two user parameters: CubeSurface (of Area type) and CubeVolume (of Volume type). To calculate CubeSurface and CubeVolume, you can write either: CubeSurface = smartWetarea ( PartBody CubeVolume = smartVolume ( PartBody or CubeVolume = smartVolume ( PartBody Pad.1 ) Pad.1 ) Pad.1 )
Solving the System of Equations by a Simulated Annealing
1. Open a new part document. 2. Create six real type parameters by using the f(x) capabilities. Name these parameters x1, y1, z1 and x2, y2, z2. 3. Access the Product Engineering Optimizer product and click the icon.
4. In the Constraints tab, specify the three constraints (enter the constraints one-by-one) x1 + y1 - z1 == 0 x1*y1 - z1 == 0 sin(x1*1rad)**2 - y1 - 1 == 0 Specify a precision of 0.01 for all three constraints. If need be, see the Product Engineering Optimizer User's Guide. 5. In the Problem tab, specify x1, y1, z1 as free parameters and 1 as Step value for all three parameters. 6. Run the optimization process in Simulated Annealing mode. You can use the default termination criteria. After the process has finished running, the x1, y1 and z1 values are close to the one below:
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x1 = 0.454 y1 = -0.807 z1 = -0.363 Keep your document open and proceed to the next task.
Solving the System of Equations by the "SetOfEquations" Capability
1. Access the Knowledge Advisor workbench, then click the icon. 2. In the "Set of Equations" editor, enter the set of equations below: x2 + y2 == z2 ; x2*y2 == z2; sin(x2*1rad)**2 == y2 +1 Specify x2, y2 and z2 as Unknown parameters by using the Parse arrow button ( ).
3. Click OK. The system of equations is solved. The values below are displayed in the specification tree x2 = 0.448043478 y2 = -0.812335288 z2 = -0.364229828
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The packages listed below are those displayed in the Browser when specifying a loop body. Basic Wireframe Package GSD Shared Package Mechanical Modeler Part Shared Package GSD Package Knowledge Expert Part Design Standard
Basic Wireframe Package
GSMPoint
Definition:
A GSMPoint is a point: • • generated by the Generative Shape Design product available in the BasicWireFrame Package.
To find out more about points, see the Generative Shape Design User's Guide.
Attributes:
PointType A point is defined by its type. The attribute to use is PointType. The syntax to be used is: PointType = i, i corresponding to the type of point that you want to create.
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Please find below a table listing the existing types of points that you can create and the digit to indicate. PlaneType in GSD Coordinates On surface On curve On plane Circle center Plane Type in the Package GSMPointCoord GSMPointOnSurface GSMPointOnCurve GSMPointOnPlane GSMPointCenter 0 1 2 3 4 Corresponding digit
As mentionned above, you may create 5 different point sub-types. Please find below a description of each sub-type, as well as its attributes and the syntax to use.
Coordinates (GSMPointCoord)
The sub-type to be used in this case is GSMPointCoord which enables you to create a coordinate point. The following attributes are available for this sub-type: • RefPoint (Reference point, optional). If specified, x, y, and z are indicated in a mark whose origin is this reference point. X (First coordinate) Y (Second coordinate) Z (Third coordinate)
• • •
These attributes can be combined as follows: Combination • • • • RefPoint (Reference point, optional) X which is defined by the syntax below: X = 10mm; Y which is defined by the syntax below: Y = 10mm; Y which is defined by the syntax below: Z = 10mm;
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On surface (GSMPointOnSurface)
The sub-type to be used in this case is GSMPointOnSurface which creates a point on a plane. The following attributes are available for this sub-type: • Direction: Element taking its orientation as reference direction or a plane taking its normal as reference direction RefPoint: Reference point. By default, the surface middle point is taken as reference. Support: Surface where the point is to be created. Values: Distance along the reference direction used to display a point.
•
• •
These attributes can be combined as follows: Combination • • • Direction which is defined by the syntax below: Direction = object: .. Line.1; Support which is defined by the syntax below: Support= object: .. Extrude.1; Values which is defined by the syntax below: Values = 12mm;
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On curve (GSMPointOnCurve)
The sub-type to be used in this case is GSMPointOnCurve which enables you to create a point on a curve. The following attributes are available for this sub-type: • • • • Boundary: Not available. RefPoint: Reference point. If not specified, it is the extremity of the curve. Support: Curve Values: Distance between the reference point and this point. Combination • • • Refpoint which is defined by the syntax below: RefPoint= object: .. Point.1; Support which is defined by the syntax below: Support = object: .. Line.1; Values which is defined by the syntax below: Values = 12mm;
On plane (GSMPointOnPlane)
The sub-type to be used in this case is GSMPointOnPlane. It creates a point on a plane. The following attributes are available for this sub-type: • • • Direction (optional). When specified, indicates the direction H: Vector. RefPoint: point used to define a reference for computing coordinates in the plane. Support: Plane on which the point will be created.
•
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V: Vector.
The attributes should be used as follows: Combination • • • • • Direction which is defined by the syntax below: Direction = object: .. Line.1; H which is defined by the syntax below: H = 150mm; RefPoint which is defined by the syntax below: RefPoint= object: .. Point.1; Support which is defined by the syntax below: Support = object: 'xy plane' V which is defined by the syntax below: V = 150mm;
Circle Center (GSMPointCenter)
The sub-type to be used in this case is GSMPointCenter which enables you to define the center of a circle. • Curve: circle, circular arc, or ellipse.
This attribute is to be used as follows: Combination • Curve which is defined by the syntax below: Curve = object: .. Extrude.1;
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GSMLine
Definition:
A GSMLine is a line : • • generated by the Generative Shape Design product. available in the BasicWireFrame Package.
To find out more about lines, see the Generative Shape Design User's Guide.
Attributes:
LineType A line is defined by its type. The attribute to be used is LineType. The syntax to be used is: LineType = i, i corresponding to the type of line that you want to create. Please find below an equivalence table listing the existing types of lines that you can create and the digit to indicate. Line Type in GSD Point to Point Point-Direction Angle to Curve Tangent to Curve Normal to surface Line Type in the Package GSMLinePtPt GSMLinePtDir GSMLineAngle GSMLineTangency GSMLineNormal 0 1 2 3 4 Corresponding digit
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Intersection betw. 2 planes
GSMLineBiTangent
5
As mentioned above, you may create 7 different line sub-types. Please find below a description of each sub-type, as well as its attributes and the syntax to use.
Point to Point Line (GSMLinePtpt)
The sub-type to be used in this case is GSMLinePtpt which defines the line extremities. The following attributes are available for this sub-type: • • • • • FirstPoint (feature) SecondPoint (feature) Support (feature) Length1 (length, optional for both combinations) Length2 (length, optional for both combinations)
These attributes can be combined as follows: 1st combination • the FirstPoint which is defined by the syntax below: FirstPoint = object: .. .. theFirstPoint; the SecondPoint which is defined by the syntax below: SecondPoint = object: .. .. theSecondPoint; Length1 which is defined by the syntax below: Length1=200mm; Length2 which is defined by the syntax below: Length2=150mm; • 2nd combination the FirstPoint which is defined by the syntax below: FirstPoint = object: .. .. theFirstPoint; the SecondPoint which is defined by the syntax below: SecondPoint = object: .. .. theSecondPoint; the Support
•
•
• •
•
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Point-Direction (GSMLinePtDir)
The sub-type to be used in this case is GSMLinePtDir which defines the line direction. The following attributes are available for this sub-type: • • • • • • Length1 Length2 Direction Orientation RefPoint Support
These attributes can be combined as follows: Combination • • • • • Length1 which is defined by the syntax below: Length1 = 100mm; Length2 which is defined by the syntax below: Length2 = 10mm; Direction which is defined by the syntax below: Direction = object: .. .. Plane.2; RefPoint which is defined by the syntax below: RefPoint = object: .. .. Point.2; Support which is defined by the syntax below: SecondPoint = object: .. .. 'xy plane';
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Tangent to Curve (GSMLineTangency)
The sub-type to be used in this case is GSMLineTangency. The following attributes are available for this sub-type: • • • • • • Curve: Reference curve used to define the tangency. Length1 Length2 Orientation RefPoint: Reference point used to define the tangency. Support
These attributes can be combined as follows: Combination • • • • • Curve which is defined by the syntax below: Curve = object: .. .. Spline.2; Length1 which is defined by the syntax below: Length1 = 100mm; Length2 which is defined by the syntax below: Length2 = 10mm; RefPoint which is defined by the syntax below: RefPoint = object: .. .. Point.2; Support which is defined by the syntax below: SecondPoint = object: .. .. 'xy plane';
Normal to surface (GSMLineNormal)
The sub-type to be used in this case is GSMLineNormal. The following attributes are available for this sub-type:
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• • •
Orientation RefPoint RefSkin
These attributes can be combined as follows: Combination • • RefPoint which is defined by the syntax below: RefPoint = object: .. .. Point.2; Support which is defined by the syntax below: RefSkin = object: .. .. Extrude.1;
GSMPlane
Definition:
A GSMPlane is a plane: • • generated by the Generative Shape Design product. available in the BasicWireFrame Package.
To find out more about planes, see the Generative Shape Design User's Guide.
Attributes:
PlaneType A plane is defined by its type. The attribute to use is PlaneType. The syntax to be used is: PlaneType = i, i corresponding to the type of plane that you want to create. Please find below a table listing the existing types of planes that you can
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create and the digit to indicate. PlaneType in GSD Equation Through 3 points Through 2 lines Through a point and a line Normal to a curve Tangent to a surface Normal to a plane Plane Type in the Package GSMPlaneEquation GSMPlane3Points GSMPlane2Lines GSMPlane1line1Pt GSMPlane1Curve GSMPlaneTangent GSMPlaneNormal 0 1 2 3 4 5 6 Corresponding digit
As mentionned above, you may create 7 different plane sub-types. Please find below a description of each sub-type, as well as its attributes and the syntax to use.
Equation (GSMPlaneEquation)
The sub-type to be used in this case is GSMPlaneEquation which enables you to create a plane by using an equation. The following attributes are available for this sub-type: • • • • • A (First component of the equation) B (Second component of the equation) C (Third component of the equation) Length RefPoint (point used to position the plane through this point)
These attributes can be combined as follows: 1st Combination • • • • A which is defined by the syntax below: A=31; //A value is required B which is defined by the syntax below: B=-47; //A value is required C which is defined by the syntax below: C=-24; //A value is required Length: enables the user to indicate the required length. It is defined by the syntax below: • • • • 2nd Combination A which is defined by the syntax below: A=31; //A value is required B which is defined by the syntax below: B=-47; //A value is required C which is defined by the syntax below: C=-24; //A value is required RefPoint which is defined by the syntax below: RefPOint = object: .. Point ;
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Length=24mm
Through 3 points (GSMPlane3Points)
The sub-type to be used in this case is GSMPlane3Points which creates a plane passing through 3 points. The following attributes are available for this sub-type: • • • Element1 (First point) Element2 (Second point) Element3 (Third point)
These attributes can be combined as follows: Combination • • • Element1 which is defined by the syntax below: Element1 = object: .. Point.1; Element2 which is defined by the syntax below: Element2 = object: .. Point.2; Element3 which is defined by the syntax below: Element3 = object: .. Point.3;
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Through 2 Lines (GSMPlane2Lines)
The sub-type to be used in this case is GSMPlane2Lines which enables you to create a plane passing through 2 lines. The following attributes are available for this sub-type: • • Element1 (First line) Element2 (Second line)
Combination • • Element1 which is defined by the syntax below: Element1 = object: .. Line.1; Element2 which is defined by the syntax below: Element2 = object: .. Line.2;
Through a Point and a Line (GSMPlane1line1Pt)
The sub-type to be used in this case is GSMPlane1Line1Pt which enables you to create a plane passing through a line and a point. The following attributes are available for this sub-type:
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• •
Line: Line used to create the plane. RefPoint: Point used to create the plane.
The attributes should be used as follows: Combination • • Line which is defined by the syntax below: Line = object: .. Line.1; RefPoint which is defined by the syntax below: RefPoint = object: .. Point.2;
Normal to a Curve (GSMPlane1Curve)
The sub-type to be used in this case is GSMPlane1Curve which enables you to create a plane normal to a curve at a specified point. • Element1: Line
This attribute is to be used as follows: Combination • Line which is defined by the syntax below: Line = object: .. Spline.1;
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Tangent to a Surface (GSMPlaneTangent)
The sub-type to be used in this case is GSMPlaneTangent which enables you to create a plane tangent to a surface at a specified point. The following attributes are available for this sub-type: • • RefPoint (Point) Support (Surface)
These attributes are to be used as follows: Combination • Support which is defined by the syntax below: Support = object: .. • Spline.1;
RefPoint which is defined by the syntax below: RefPoint = object: .. Point.4;
Normal to a Plane (GSMPlaneNormal)
The sub-type to be used in this case is GSMPlaneNormal. The following attributes are available for this sub-type: • • Curve: Reference curve used to create the plane. RefPoint: Reference point used to create the plane.
These attributes are to be used as follows: Combination
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•
Curve which is defined by the syntax below: Curve = object: .. Spline.1;
•
RefPoint which is defined by the syntax below: RefPoint = object: .. Point.4;
GSMCircle
Definition:
A GSMCircle is a circle: • • generated by the Generative Shape Design product. available in the BasicWireFrame Package.
To find out more about circles, see the Generative Shape Design User's Guide.
Attributes:
PointType A point is defined by the following attributes: • CircleType: The syntax to be used is CircleType = i, i corresponding to the type of circle that you want to create.
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• • •
CircleRelimitation: The syntax to be used is CircleRelimitation =. EndAngle: The syntax to be used is EndAngle = xxxdeg. StartAngle: The syntax to be used is StartAngle =xxxdeg.
Please find below a table listing the existing types of circles that you can create and the digit to indicate. PlaneType in GSD Three Points Center and Radius Center and Point Plane Type in the Package GSMPCircle3Points GSMCircleCtrRad GSMCircleCtrPt 3 0 1 Corresponding digit
As mentionned above, you may create 3 different circle sub-types. Please find below a description of each sub-type, as well as its attributes and the syntax to use.
Three Points (GSMCircle3Points)
The sub-type to be used in this case is GSMCircle3Points which enables you to create a circle passing through 3 points. The following attributes are available for this sub-type: • • • • Element1: First point Element2: Second point Element3: Third point Support: Support surface onto which the circle will be projected (optional)
These attributes can be combined as follows: Combination • • • • Element1 which is defined by the syntax below: Element1 = object: .. Point.1; Element2 which is defined by the syntax below: Element2 = object: .. Point.2; Element3 which is defined by the syntax below: Element3 = object: .. Point.3; Support which is defined by the syntax below: Support = object: .. Extrude.1;
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Center and Radius (GSMCircleCtrRad)
The sub-type to be used in this case is GSMCircleCtrRad which enables you to create a circle by indicating its center and its radius. The following attributes are available for this sub-type: • • • • • Center: Point that will be the center of the circle. FirstDirection Geodesic Radius: Radius of the circle. Support: Support plane or surface onto which the circle is to be created.
These attributes can be combined as follows: Combination • • • Center which is defined by the syntax below: Center = object: .. Point.1; Radius which is defined by the syntax below: Radius = 120mm; Support which is defined by the syntax below: Support = object: .. Extrude.1;
Center and point (GSMCircleCtrPt)
The sub-type to be used in this case is GSMCircleCtrPt which enables you to create a circle by indicating its center and a point. The following attributes are available for this sub-type: • • • • Center: Point used as the center of the circle. Geodesic: Curve. RefPoint: Second point used to create the circle. Support: Support plane or surface where the circle is to be created. Combination • Center which is defined by the syntax below:
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• •
Center = object: .. Point.1; RefPoint which is defined by the syntax below: RefPoint = object: .. Point.1; Support which is defined by the syntax below: Support = object: .. Extrude.1;
Part Design Package
Please find below a table listing the types available in the Part Design package. Box Counterbored Hole Cylinder Pocket Shaft SoldCombine Thickness Chamfer Counterdrilled Hole Hole RemoveFace Shell Split ThickSurface Cone Countersunk Hole Pad ReplaceFace SimpleHole TaperedHole Torus
Box
Definition:
A box is a pad extruded from a rectangular sketch.
Attributes:
A box is defined by the following attributes: • • • Length which is the pad first limit. The syntax to be used is Length = 10mm. Width which is the pad width. The syntax to be used is Width = 20mm. Height which is the pad height. The syntax to be used is Height = 12mm.
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MyBox isa CATPart { BoxPart isa Part { PartBody isa BodyFeature { // Create a box Box1 isa Box { // Specify the box properties Width = 20.0 mm ; Height = 25.0 mm ; Length = 15.0 mm ; } } } }
Chamfer
Definition:
A cut through the thickness of the feature at an angle, giving a sloping edge.
Attributes:
A chamfer is defined by the following attributes: • • • Angle. The syntax to be used is Angle = 20 deg; Length1. The syntax to be used is Length1 = 5 mm; Length2. The syntax to be used is Length2 = 5 mm;
Important Notes: • A chamfer has a Length2 attribute which is the default chamfer length. You don't have to manipulate this attribute in a script.
To specify a chamfer within your script, you must have a part open, then: 1. Create a Chamfer by using the isa function Chamfer1 isa Chamfer ( ) { } 2. Right-click anywhere inside the parentheses and select the 'Get Edge' or the 'Get Surface' command from the contextual menu. Then, in the geometry
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area, select the edge or surface to be chamfered. MyBox isa CATPart { BoxPart isa Part { PartBody isa BodyFeature { // Create a box Box1 isa Box { Width = 20.0 mm ; Height = 25.0 mm ; Length = 15.0 mm ; } // Create a chamfer // The edge definition must be captured // from the geometry area // Use the Get Edge command from the // contextual menu Chamfer1 isa Chamfer (Edge Definition) { Angle = 20 deg; Length1 = 5 mm ; } Chamfer2 isa Chamfer (Edge Definition) { Angle = 30 deg; Length1 = 10 mm ; } } } }
Cone
Definition:
A cone is a shaft created by rotating a triangular sketch.
Attributes:
A cone is defined by the following attributes: • • Length. The syntax to be used is Length = 15.0 mm ;. Radius. The syntax to be used is Radius = 20.0 mm ;.
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MyCone isa CATPart { ConePart isa Part { PartBody isa BodyFeature { // Create a cone Cone1 isa Cone { Radius = 20.0 mm ; Length = 15.0 mm ; } } } }
Counterbored Hole
Definition:
A mechanical feature of Hole type you create when you click icon in the Part Design the workbench. For more information, refer to the Part Design User's Guide.
Attributes:
A counterbored hole is defined by the following attributes: • • CounterboreDepth. The syntax to be used is CounterboreDepth =12mm. CounterboreDiameter: The syntax to be used is CounterboreDiameter =15mm.
Counterdrilled Hole
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Definition:
A mechanical feature of Hole type you create when you click icon in the Part Design the workbench. For more information, refer to the Part Design User's Guide.
Attributes:
A counterdrilled hole is defined by the following attributes: • • • CounterdrillAngle. The syntax to be used is CounterdrillAngle = 22deg. CounterdrillDiameter. The syntax to be used is CounterdrillDiameter =12mm. CounterdrillDepth. The syntax to be used is CounterdrillDepth =12mm.
Countersunk Hole
Definition:
A mechanical feature of Hole type you create when you click icon in the Part Design the workbench. For more information, refer to the Part Design User's Guide.
Attributes:
A countersunk hole is defined by the following attributes:
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• • •
CountersinkAngle. The syntax to be used is CountersinkAngle = 12deg. CountersinkDepth. The syntax to be used is CountersinkDepth =15mm. CountersinkDiameter. The syntax to be used is CountersinkDiameter =15mm.
Cylinder
Definition:
A cylinder is a pad created by extruding a circular sketch.
Attributes:
A cynlinder is defined by the following attributes: • • EndLimit Length. The syntax to be used is Length =12mm. Radius: The syntax to be used is Radius =5mm.
Cylinder1 isa CATPart { Part isa Part { PartBody isa BodyFeature { // Create a cylinder Cyl1 isa Cylinder { Radius=15.0 mm; EndLimit=20.0 mm; } } } }
Hole
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Definition:
A is an opening through a feature.
Attributes:
A hole is defined by the following attributes: • • • • • • • • • • • • BottomAngle BottomType Depth Diameter DiameterThread HoleType LimitType Pitch TapSide Threaded ThreadingDepth Radius
To specify a hole within your script, you have to use one of the holes listed below. Hole is the father type and cannot be used. • • • • Counterbored Hole Countersunk Hole Counterdrilled Hole Tapered Hole
Pad
Definition:
A pad is a feature created by extruding a sketch.
Attributes:
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A pad is defined by the following attributes: • • • the sketch the pad is extruded from. the FirstLimit the SecondLimit Length (or StartLimit Length ( or EndLimit Length) Length).
A limit which is not specified is set by default to zero. // Use the Insert File Path command from the // contextual menu to specify the path of the file // to be imported import PktSketchToImport.CATPart;/*In the script above, the P0 pad is created from the Sketch.1 sketch which is imported from the document.*/
myDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { Sketch isa Sketch.1 {} P0 isa Pad("Sketch") { SecondLimit } } } } Length=40.0mm;
Shaft
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Attributes:
A shaft has two attributes: • • • • • • • The The The The The The The StartAngle. The syntax to be used is StartAngle=12deg. EndAngle. The syntax to be used is EndAngle=23deg. MergeEnd NeutralFiber Thickness1 Thickness2 Thinmode
The sketch to be rotated must be imported from an external CATPart document. This external document must also include a rotation axis. /* Use the Insert File Path command from the contextual menu to select the the sketch to be imported */ import //Use the Insert File Path command to insert the Pktsketch_shaft.CATPart file. MyShaft isa CATPart { myPart isa Part { PartBody isa BodyFeature { Sketch isa Sketch.1 {} S0 isa Shaft("Sketch") { StartAngle = 20 deg ; EndAngle = 300 deg ; } } } }
Shell
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Definition:
A shell is a hollowed out feature.
Attributes:
A shell is defined by the following attributes: • • DefaultInsideThickness. The syntax to be used is DefaultInsideThickness = 2mm. DefaultOutsideThickness: The syntax to be used is DefaultOutsideThickness = 1mm.
To specify a shell within your script, you must have a part open, then: 1. create a Shell by using the isa function Shell1 isa Shell ( ) { } 2. right-click anywhere inside the parentheses and select the 'Get Surface' function from the contextual menu. Then, in the geometry area, select the face to be hollowed out. A 1mm thick shell is created by default. MyBox isa CATPart { BoxPart isa Part { PartBody isa BodyFeature { Box1 isa Box { Width = 20.0 mm; Height = 25.0 mm; Length = 15.0 mm; } Shell1 isa Shell (face definition) { DefaultInsideThickness = 2mm; DefaultOutsideThickness = 1mm; } } } }
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SimpleHole
Definition:
A mechanical feature of Hole type you create when you click the icon in the Part Design workbench. For more information, refer to the Part Design User's Guide..
Attributes:
Hole1 isa CATPart { Part isa Part { PartBody isa BodyFeature { P isa Pad { } F isa SimpleHole("Use the Get Edge command to select the edge") { } } } }
Sphere
Definition:
A sphere is a shaft created by rotating half a circle around an axis passing through the arc extremities. The only property is the Radius.
Attributes:
A sphere is defined by the following attribute: • Radius. The syntax to be used is: Radius = 20.0 mm.
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MySphere isa CATPart { SpherePart isa Part { PartBody isa BodyFeature { Sphere1 isa Sphere { Radius = 20.0 mm ; } } } }
Tapered Hole
Definition:
A mechanical feature of Hole type you create when you click icon in the Part Design the workbench. For more information, refer to the Part Design User's Guide.
Attributes
A tapered hole is defined by the following attribute: • TaperAngle:
Thickness
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Definition:
A thick
Attributes
A thickness is defined by the following attribute: • DefaultThickness:
ThickSurface
Definition:
A thicksurface is a surface to which material was added in two opposite directions.
Attributes:
A thicksurface is defined by the following attributes: • • TopOffset, the thickness in one direction. The syntax to be used is TopOffset = 0.5mm. the BotOffset, the thickness in the one direction. The syntax to be used is BotOffset = 10 mm.
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myThickSurface isa CATPart { myPart isa Part { OpenBody1 isa OpenBodyFeature { P1 isa GSMPoint { PointType = 0; TypeObject isa GSMPointCoord { X = 0mm; Y = 0mm; Z = 0mm; } } C isa GSMCircle { CircleType = 0; TypeObject isa GSMCircleCtrRad { Center = object : .. object : .. .. .. .. P1; Support = `xy-plane`; Radius = } StartAngle = EndAngle = } Fi isa GSMFill { Boundary = object : .. } } PartBody isa BodyFeature { Thick1 isa ThickSurface { TopOffset = 0.5mm; C;
150mm; 0deg; 360deg;
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BotOffset = 10 mm; Surface = object : .. } } } .. } OpenBody1 Fi;
Torus
Definition:
A torus is a shaft created by rotating a circular sketch around an axis.
Attributes:
A torus is defined by the following attributes: • • InnerRadius SectionRadius
BodyDoc isa CATPart { BodyPart isa Part { Body isa BodyFeature { // Create a sphere Sphere1 isa Sphere { Radius = 15.0 mm; } // Create a torus Torus1 isa Torus { InnerRadius = 20.0 mm ; SectionRadius = 10.0 mm ; } } } }
Part Shared Package
Fillet Object
Definition
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Describes the feature you create when you click the icon in the Part Design workbench. For more information, please refer to the Part Design User's Guide. It is defined by one property: • Radius
There are 3 different types of fillets: • ConstantEdgeFillet • • FaceFillet TriTangentFillet
Constant Edge Fillet Object
Definition
A fillet is a curved surface of a constant or variable radius that is tangent to, and that joins two surfaces. Together, these three surfaces form either an inside corner or an outside corner. Important Note: To specify a fillet within your script, you must have a part open, then: 1. Create a Fillet by using the isa keyword. Fillet1 isa ConstantEdgeFillet ( ) { } 2. Right-click anywhere inside the parentheses and select the 'Get Edge' or the 'Get Surface' function from the contextual menu. Then, in the geometry area, select the edge or the face to be filleted.
Example
Box1 isa CATPart { BoxPart isa Part { PartBody isa BodyFeature { Box1 isa Box { Width = 20.0 mm ; Height = 25.0 mm ; Length = 15.0 mm ; } // Use the Get Edge or Get Surface command // from the contextual menu to retrieve // the edge or face to be filleted
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Pattern
Definition
A pattern is a set of similar features repeated in the same part. Two types of patterns can be created with CATIA: the rectangular patterns and the circular patterns. At present, only rectangular patterns can be generated from a script. A rectangular pattern is defined by the following properties: • Nb1, the number of elements to be replicated along the first direction • • • • Nb2, the number of elements to be replicated along the second direction Step1, the element spacing along the first direction Step2, the element spacing along the second direction Activity.
Syntax
pattern1 isa pattern [Nb1,Nb2] of feature_to_be_repeated
Example
MyBox isa CATPart { BoxPart isa Part {
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PartBody isa BodyFeature { Box1 isa Box { Width = 20 mm ; Height = 20 mm ; Length = 20 mm ; }
// Use the Get Surface command from the // contextual menu to specify the hole // anchor Hole1 isa SimpleHole ("Face:(Brp:(Pad.1;2);None:();Cf9:())") { Diameter = 15 mm; } Pattern1 isa Pattern[3,4] of Hole1 { Step1 = 50 mm; Step2 = 50 mm; } } } }
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Standard Package
Old Types Names Old Attributes New Types Names Feature New Attributes Id Name Owner Color Layer Pick Show
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List Visualizable
GSD Shared Package
Types Names GSMAffinity Attributes AxisFirstDirection AxisOrigin AxisPlane Ratio
GSMAxisToAxis GSMRotate GSMScaling GSMSymetry GSMTransformation GSMTranslate Angle Axis Ratio Reference Reference Activity ToTransfor Direction Distance
GSD Package
Please find below a table listing the types contained in the GSD package: GSM3DCurveOffset GSMBlend GSMConic GSMCurve GSMCylinder GSMExtractContour GSMExtremumPolar GSMAssemble GSMBoundary GSMConnect GSMCurvePar GSMDirection GSMExtrapol GSMExtrude GSMAxisToAxis GSMCombine GSMCorner GSMCurveSmooth GSMExtract GSMExtremum GSMFill
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GSMFillet GSMHelix GSMLawDistProj GSMNear GSMReflectLine GSMSpine GSMSweep GSMSweepSegment GSMUnfold GSOJunction GSOVariableOffset
GSMFilletBiTangent GSMIntersect GSMLineCorner GSMOffset GSMRevol GSMSpiral GSMSweepCircle GSMSweepSketch GSMWSupport GSOSeatDiabolo GSOWrapCurve
GSMHealing GSMInverse GSMLoft GSMProject GSMSphere GSMSplit GSMSweepConic GSMTrim GSOBump GSPShapeMorphing GSOWrapSurface
GSMAssemble
Definition:
A GSMAssemble is an object which joins at least two surfaces or two curves. The surfaces or curves to be joined must be adjacent. See the Generative Shape Design User's Guide for more information.
Attributes:
Click here to open the GSMAssembleScript script file.
GSMCurve
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Definition:
A GSMCurve is an object generated by the Generative Shape Design product. You can create a corner by ) clicking the Corner icon ( in the Generative Shape Design workbench. Click here to open the GSMCurveScript script file.
GSMCurvePar
Definition:
An GSMCurvePar object is a Generative Shape Design parallel curve.
Attributes: A GSMCurvePar is defined by the following attributes: • • • • • • • • • • InvertLaw. Length1. Length2. Mode. Offset. Orientation. PassingPoint. Support. TMDeviation. Type.
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Click here to open the GSMCurveParScript script file.
GSMExtrude
Definition:
A surface created by extruding a profile along a given direction. You can create an extruded surface by clicking the Extrude ) in the Generative icon ( Shape Design workbench. Attributes: A GSMExtrude is defined by the following attributes: • • • • • Direction. Element1. Length1. Length2. Orientation.
Click here to open the GSMSplit script file.
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GSMFillet
Definition:
An GSMFillet object is curved surface of a constant or variable radius that is tangent to and joins two surfaces. Together these three surfaces form either an inner or outer corner. Attributes: A GSMFillet is defined by the following attributes: • • • Element1. Element2. Radius.
Click here to open the GSMFilletScript.CATGScript file.
GSMProject
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Definition:
A Generative Shape Design projection. See the Generative Shape Design User's Guide for more information.
Attributes: A GSMProject is defined by the following attributes: • • • • • • Direction. Normal which corresponds to the Projection type field in the Projection Definition dialog box ( Normal = 1 for an orthogonal projection - otherwise specify a direction, a GSMLine for example). SolutionType. TMDeviation. ToProject which corresponds to the Projected field in the Projection Definition dialog box. Support which corresponds to the Support field in the Projection Definition dialog box.
Click here to open the GSMSplit script file.
GSMSplit
Definition:
A surface or wireframe element that was split by means of a cutting element. You can split: • a wireframe element by a point, another wireframe element or a surface a surface by a
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wireframe element or another surface. You can split geometry by ) in clicking the Split icon ( the Generative Shape Design workbench. Click here to open the GSMSplit script file.
GSMSweepSegment
Definition:
Attributes: A GSMSweepSegment is defined by the following attributes: • • • • • • • Angle. GuideCrv. GuideSurf. Length. Length1. Length2. Spine.
Click here to open the GMSweepSegmentScript file.
Knowledge Expert Package
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knowledgewareAdvisor Please find below a table listing the types contained in the Knowledge Expert package: KWECheck KWEGenericRuleBaseComponent KWERule KWERuleBaseComponent
KWERuleBase KWERuleSet
KWECheck
Definition:
Expert Checks are features generated by the Knowledge Expert product. Checks are regrouped into rule sets. Rule sets belong to a rule base. When writing a script with checks you must comply with the Rule Base/Rule Set hierarchy. Refer to the Knowledge Expert User's Guide for more information on the concepts behind the expert rules and checks. Click here to open the KnowledgeExpertScript file.
KWERule
Definition:
Expert Rules are features generated by the Knowledge Expert product. Rules are regrouped into rule sets. Rule sets belong to a rule base. When writing a script with rules you must comply with the Rule Base/Rule Set hierarchy. Refer to the Knowledge Expert User's Guide for more information on the concepts behind the expert rules and checks.
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Reference
Click here to open the KnowledgeExpertScript file.
KWERuleBase
Definition:
Rule bases are features generated by the Knowledge Expert product. Refer to the Knowledge Expert User's Guide for more information on the concepts behind this type of feature. Click here to open the KnowledgeExpertScript file.
KWERuleSet
Definition:
Rule sets are features generated by the Knowledge Expert product. Refer to the Knowledge Expert User's Guide for more information on the concepts behind this type of feature. Click here to open the KnowledgeExpertScript file.
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Mechanical Modeler Package
Some types and attributes were changed. Please find below a conversion table listing the old types, their attributes, their new names (if any) as well as their attributes: BodyFeature MechanicalFeature OpenBodyFeature GeometryFeature OpenBodyFeature
BodyFeature
Definition:
A body is the combination of several features within a part. For more information, see the Part Design User's Guide.
BodyDoc isa CATPart { BodyPart isa Part { Body isa BodyFeature { // Create a sphere Sphere1 isa Sphere { Radius = 15.0 mm; } // Create a torus Torus1 isa Torus { InnerRadius = 20.0 mm ; SectionRadius = 10.0 mm ; } } } }
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Workbench Description
Workbench Description
This section contains the description of the icons and menus specific to the Knowledge Advisor workbench. The Knowledge Advisor workbench is shown below. Click the sensitive areas (toolbars) to access the related documentation.
Knowledge Advisor Menu Bar Knowledge Toolbar Reactive Features Toolbar Control Features Toolbar Organize Knowledge Toolbar Actions Toolbar Tools Toolbar Set of Equations Toolbar
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Toolbars
Knowledge Toolbar
The Knowledge toolbar contains the following tools
See Creating a Parameter and Creating a Formula. See Associating URLs and Comments with Parameters or Relations. See Creating a Design Table from Current Values and Creating a Design Table from a Pre-Existing File. See Creating a Law. See Using the Knowledge Inspector. See Using the Equivalent Dimensions Feature. See Locking and Unlocking a Parameter.
Reactive Features Toolbar
The Reactive Features Toolbar contains the following tools:
See Creating a Rule. See Creating a Check. See Creating a Reaction: DragAndDrop Event.
Organize Knowledge Toolbar
The Organize Knowledge Toolbar contains the following tools:
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See Creating Sets of Parameters. See Creating Sets of Relations. See Adding a Parameter to a Feature. See Adding a Parameter to an Edge. See Associating URLs and Comments with Parameters or Relations.
Control Features Toolbar
The Control Features Toolbar contains the following tools:
Here is a brief description of each icon. See Creating a List. See Creating a Loop.
Actions Toolbar
The Control Features Toolbar contains the following tools:
See Launching a VB macro with Argument. See Using the Knowledge Advisor Action Feature.
Tools Toolbar
The Tools Toolbar contains the following tools: 293
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See Updating Relations Using Measures. Select the Update icon to update a document without exiting the Knowledge Advisor workbench.
Set of Equations Toolbar
The Tools Toolbar contains the following tools:
See Solving a Set of Equations.
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Customizing for Knowledge Advisor
Customizing
Before you start your first working session, you can customize the way you work to suit your habits. This type of customization is stored in permanent setting files: these settings will not be lost if you end your session 1. Select the Tools -> Options command. The Options dialog box is displayed. 2. Choose the General category in the left-hand box. 3. Click the Parameters and measure tab. The following tabs are displayed.
This tab lets you define: o o o the Knowledge settings the libraries you want to load the report settings
4. Two other tabs, located in the Infrastructure category, in the Part Infrastructure workbench, also interfere with Knowledgeware applications.
o o
General Display
5. Change these options according to your needs. 6. Click OK when done to validate your settings.
Knowledge
This page deals with these categories of options:
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knowledgewareAdvisor • • • • Parameter Tree View Parameter names Relations update in part context Design Tables
Parameter Tree View
There are 2 types of items that you can display in the specification tree.
With value
Displays the parameter values in the specification tree. By default, this option is unchecked.
With formula
Displays the formulas constraining the parameter in the specification tree. By default, this option is unchecked.
Parameter names
This option should be checked if you work with non-Latin characters. If this option is unchecked, parameter names should have to be renamed in Latin characters when used in formulas. By default, this option is unchecked.
Relations update in part context
Before V5R12, Knowledge relations (formulas, rules, checks, design tables, and sets of equations) used to execute as soon as one of their inputs was modified. The user can now choose, when creating the relation, if it will be synchronous (i.e. the evaluation will be launched as soon as one of its parameters is modified) or 296
Project Standards asynchronous (i.e. the evaluation will be launched when the Part is updated). Each relation can therefore be synchronous or asynchronous. The 2 following options enable the user to create synchronous or asynchronous relations.
Creation of synchronous relations
Enables the user to create synchronous relations, that is to say relations that will be immediately updated if one of their parameters/inputs is modified. Relations based on parameters are the only one that can be synchronous. By default, this option is unchecked
Creation of relations evaluated during the global update
Enables the user to associate the evaluation of asynchronous relations with the global update. The relations can be asynchronous for 2 reasons: • • • • • The user wants the relations to be asynchronous The relation contains measures. Relations based on parameters: These relations can be synchronous or asynchronous. Relations based on geometry: These relations can only be asynchronous. Relations based on parameters and on geometry: For the part of the relations containing parameters, the user decides if he wants the update to be synchronous or not. For the other part of the relations, the update occurs when the global update is launched. Note that the user can also decide if already existing relations are synchronous or asynchronous. To know more, see Controlling Relations Update in the Infrastructure User's Guide. •
By default, this option is checked.
Design Tables
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There are 2 types of items that you can set up.
Automatic Synchronization at Load
When loading a model containing user design tables, if the design table files have been modified and the external file data is contained in the model, the design table will be synchronized automatically if this radio button is checked. By default, this option is checked.
Interactive Synchronization at Load
When loading a model containing user design tables whose external source file was deleted, this option enables the user to select a new source file or to save the data contained in the design tables in a new file. By default, this option is unchecked.
Manual Synchronization
When loading a model containing user design tables, if the design table files have been modified and the external file data is contained in the model, the design table will be synchronized if this radio button is checked. To synchronize both files, rightclick the design table in the specification tree and select the DesignTable object>Synchronize command or the Edit->Links command. By default, this option is unchecked.
Default Mode: Copy Data Into Model
If checked, the data contained in the external source file will be copied into the model. By default, this option is unchecked.
Default Mode: Do Not Copy Data Into Model
If checked, the data contained in the external source file will not be copied into the
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model. By default, this option is checked.
Language
This page deals with the following categories of options: • • Language Reference Directory for Types
Language
This field is to be used when using measures in relations or user functions. Measures are specific functions to be used in formulas and rules. The Knowledge Advisor User's Guide provides you with tasks explaining how to use measures. For how to create and use user functions, see the CATIA Application Architecture documentation.
Load extended language libraries
If checked, enables the user to select the packages he wants to load under Packages (if he wants to load a limited number of packages.)
This option is particularly useful for the administrator to limit the number of packages used by the user. It is also very useful to improve performances since only the required libraries are loaded.
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•
When you open a document and some relations are broken, you might need to load all libraries to solve the error, which may take quite a long time. It is strongly recommended to identify the packages you will need and to select them.
•
By default, this option is unchecked.
All packages
Enables the user to select all packages.
Reference Directory For Types
Reference Directory For Types
Enables the user to save the CATGScript file in the Directory indicated in the Reference Directory for Types field for later re-user (To know more, see the PKT User's Guide). By default, this option is not available.
Report Generation
This page explains how to customize the reports generated by the Global Check Analysis tool in the Knowledge Advisor and Knowledge Expert workbenches. It deals with the following categories of options: • • • • • Configuration of the Check Report Input XSL Report content Output directory HTML Options
Configuration of the Check Report
Html
Enables the user to generate a HTML report.
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Xml
Enables the user to generate a XML report. By default, the HTML option is enabled.
Input XSL
Note that this option is available only if the XML configuration setting is set.
Input XSL
Enables the user to select the XSL style sheet that will be applied to the generated XML report. The StyleSheet.xsl file is the default XSL file, but you can use your own template.
Report content
Failed Checks
If checked, the generated report will contain information about the failed checks only. By default, this option is unchecked.
All Checks
If checked, the generated report will contain information about all the checks contained in the document. By default, this option is checked.
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Check Advisor
If checked, the generated report will contain information about all the Knowledge Advisor checks contained in the document. By default, this option is checked.
Parameters information
Not available
Check Expert
If checked, the generated report will contain information about all the Knowledge Expert checks contained in the document. By default, this option is checked.
Passed objects
If checked, the generated report will contain information about the objects that passed the Expert checks as well as information about the parameters of these objects (diameter, depth, pitch,...). By default, this option is checked.
Objects information
Not available
Output directory
Output directory
Enables the user to select the output directory that will contain the generated report. By default, this option is available.
HTML Options
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Open HTML browser into CATIA Session
This option is available for Windows only. It enables the user to define if the report will be opened in a CATIA session (in this case, the check box should be checked) or if it will be opened in an Internet Explorer session (in this case, the check box should remain unchecked.) Note that it is highly recommended not to use this report as a basis for macros or for other applications. It is only provided for information purposes. By default, this option is checked.
Part Infrastructure for Knowledgeware Applications
This page deals with the options concerning: • • the external references: Keep link with selected object the specification tree display
Part Infrastructure General option
Keep link with selected object
You need to select this option to take advantage of the associativity. Click here to know more about the Part Infrastructure General options.
Part Infrastructure Display option
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Parameters
Select this option to display the parameters when working in a CATProduct context. By default, this option is unchecked.
Relations
Select this option to display the relations when working in a CATProduct context. By default, this option is unchecked. Click here to know more about the Part Infrastructure Display options.
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Knowledge Advisor
Table Of Contents
Overview ...................................................................................................... 1 Knowledge Advisor in a Nutshell .................................................................... 1 Before Reading this Guide ............................................................................ 2 Getting the Most out of this Guide ................................................................. 2 Accessing sample documents ........................................................................ 2 Conventions Used in this Guide ..................................................................... 2 What's New? ................................................................................................. 3 New Functionalities...................................................................................... 3 Getting Started.............................................................................................. 5 Using Parameters ........................................................................................ 5 Using Formulas ........................................................................................... 6 Using Rules ................................................................................................ 8 Using Checks .............................................................................................10 User Tasks ...................................................................................................13 User Tasks ................................................................................................13 Working with Parameters ............................................................................13 Working with Parameters..........................................................................13 Introducing Parameters ............................................................................13 Creating a Parameter ...............................................................................14 Copy/Pasting Parameters..........................................................................15 Specifying the Material Parameter ..............................................................16 Valuating the Mechanical Property Parameters .............................................17 Specifying a Parameter Value as a Measure .................................................17
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knowledgewareAdvisor Importing Parameters ..............................................................................20 Creating Points, Lines... as Parameters .......................................................21 Applying Ranges to Parameters by Using a Rule ...........................................22 Creating an Associative Link Between Measures and Parameters ....................24 Publishing Parameters ..............................................................................29 Activating and Deactivating a Component ...................................................34 Creating an External Parameter .................................................................39 Deactivating and Re-activating External Parameters .....................................40 Getting Familiar with the Parameters Explorer .............................................41 Adding a Parameter to a Feature ...............................................................43 Adding a Parameter to an Edge .................................................................45 Locking and Unlocking a Parameter ............................................................47 Creating Sets of Parameters......................................................................49 Working with Formulas................................................................................50 Working with Formulas .............................................................................50 Introducing Formulas ...............................................................................50 Getting Familiar With the f(x) Dialog Box ....................................................51 Using the Dictionary.................................................................................54 Creating a Formula ..................................................................................62 Creating Formulas based on Publications.....................................................63 Specifying a Measure in a Formula .............................................................66 Using Geometry to Create a Formula ..........................................................68 Refering to External Parameters in a Formula ..............................................69 Using the Equivalent Dimensions Feature ....................................................72 Associating URLs and Comments with Parameters or Relations..........................74
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Table Of Contents Associating URLs & Comments with Features ...............................................74 Assigning a Comment to a Knowledge Feature .............................................74 Working with Design Tables .........................................................................76 Working with Design Tables ......................................................................76 Introducing Design Tables.........................................................................77 Getting Familiar with the Design Table Dialog Box ........................................81 Creating a Design Table from the Current Parameters Values .........................86 Creating a Design Table from a Pre-existing File...........................................88 Interactively Adding a Row To a Design Table External File ............................90 Controlling Design Tables Synchronization...................................................93 Storing a Design Table in a Power Copy ......................................................96 Creating and Using a Knowledge Advisor Law .................................................98 Using the Knowledge Inspector .................................................................. 102 The 'What If' Mode................................................................................. 103 The 'How To' Mode ................................................................................ 105 Working with the Rule Feature ................................................................... 107 Working with the Rule Feature................................................................. 107 Creating a Rule ..................................................................................... 108 Using Rules and Checks in a Power Copy................................................... 110 Using the Rule Editor ............................................................................. 111 Handling Errors ..................................................................................... 112 Working with the Check Feature ................................................................. 114 Working with the Check Feature .............................................................. 114 Creating a Check ................................................................................... 114 Performing a Global Analysis of Checks..................................................... 116
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knowledgewareAdvisor Using the Check Editor ........................................................................... 126 Using the Action Feature......................................................................... 127 Working with the Reaction Feature.............................................................. 130 Working with the Reaction Feature ........................................................... 130 Using the Reaction Feature Window.......................................................... 131 Creating a Reaction Event....................................................................... 134 Creating a Loop in a Reaction .................................................................. 156 Launching a VB Macro with Arguments ........................................................ 159 Working with Relations.............................................................................. 161 Working with Relations ........................................................................... 161 Creating Sets of Relations ....................................................................... 161 Using Relations based on Publications at the Product Level .......................... 162 Activating and Deactivating a Component ................................................. 166 Instantiating Relations from a Catalog ...................................................... 171 Updating Relations Using Measures .......................................................... 172 Controlling Relations Update ................................................................... 173 Working with the List Feature..................................................................... 177 Working with the List Feature ................................................................. 177 Using the List Edition Window.................................................................. 178 Creating a List....................................................................................... 180 Working with the Loop Feature ................................................................... 183 Working with the Loop Feature ................................................................ 184 Introducing the Loop Feature .................................................................. 184 Getting Familiar with the Loop Edition Window and Menus ........................... 184 Creating a Loop..................................................................................... 188
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Table Of Contents Creating a Power Copy Containing a Loop ................................................. 191 Using the Scripting Language .................................................................. 196 Declaring Input Data.............................................................................. 208 Defining the Context .............................................................................. 209 Solving a Set of Equations ......................................................................... 210 Solving a Set of Equations ...................................................................... 210 Using the Equations Editor ...................................................................... 211 Using the Knowledge Advisor Language ....................................................... 213 Using the Knowledge Advisor Language .................................................... 213 Attributes ............................................................................................. 220 Object Methods ..................................................................................... 220 Messages and macros ............................................................................ 227 Limitations .............................................................................................. 231 Parameters and Formulas ....................................................................... 231 Design Tables ....................................................................................... 231 Rules ................................................................................................... 231 Sets of Equations .................................................................................. 231 Macros with Arguments .......................................................................... 231 Loops .................................................................................................. 231 Useful Tips .............................................................................................. 232 Relations .............................................................................................. 232 Rules ................................................................................................... 233 Parameters ........................................................................................... 234 Formulas .............................................................................................. 235 Design Tables ....................................................................................... 235
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knowledgewareAdvisor Loops .................................................................................................. 236 Reactions ............................................................................................. 238 Use Cases ............................................................................................... 238 Use Cases ............................................................................................ 238 The Ball Bearing .................................................................................... 238 System of Three Equations in Three Variables............................................ 245 Reference .................................................................................................. 247 Reference ............................................................................................... 247 Basic Wireframe Package........................................................................... 247 GSMPoint ............................................................................................. 247 GSMLine............................................................................................... 252 GSMPlane............................................................................................. 256 GSMCircle............................................................................................. 262 Part Design Package ................................................................................. 265 Box ..................................................................................................... 265 Chamfer............................................................................................... 266 Cone.................................................................................................... 267 Counterbored Hole................................................................................. 268 Counterdrilled Hole ................................................................................ 268 Countersunk Hole .................................................................................. 269 Cylinder ............................................................................................... 270 Hole .................................................................................................... 270 Pad ..................................................................................................... 271 Shaft ................................................................................................... 272 Shell.................................................................................................... 273
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Table Of Contents SimpleHole ........................................................................................... 275 Sphere................................................................................................. 275 Tapered Hole ........................................................................................ 276 Thickness ............................................................................................. 276 ThickSurface ......................................................................................... 277 Torus ................................................................................................... 279 Part Shared Package................................................................................. 279 Fillet Object .......................................................................................... 279 Constant Edge Fillet Object ..................................................................... 280 Pattern ................................................................................................ 281 Standard Package .................................................................................... 283 GSD Shared Package ................................................................................ 283 GSD Package ........................................................................................... 283 GSMAssemble ....................................................................................... 284 GSMCurve ............................................................................................ 284 GSMCurvePar........................................................................................ 285 GSMExtrude.......................................................................................... 286 GSMFillet.............................................................................................. 287 GSMProject........................................................................................... 287 GSMSplit .............................................................................................. 288 GSMSweepSegment ............................................................................... 289 Knowledge Expert Package ........................................................................ 289 KWECheck ............................................................................................ 290 KWERule .............................................................................................. 290 KWERuleBase........................................................................................ 291
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knowledgewareAdvisor KWERuleSet.......................................................................................... 291 Mechanical Modeler Package ...................................................................... 292 BodyFeature ......................................................................................... 292 Workbench Description ................................................................................ 293 Workbench Description ............................................................................. 293 Toolbars ................................................................................................. 294 Knowledge Toolbar ................................................................................ 294 Reactive Features Toolbar....................................................................... 294 Organize Knowledge Toolbar ................................................................... 294 Control Features Toolbar ........................................................................ 295 Actions Toolbar ..................................................................................... 295 Tools Toolbar ........................................................................................ 295 Set of Equations Toolbar......................................................................... 296 Project Standards ....................................................................................... 297 Customizing for Knowledge Advisor............................................................. 297 Customizing.......................................................................................... 297 Knowledge............................................................................................ 297 Language ............................................................................................. 301 Report Generation ................................................................................. 302 Part Infrastructure for Knowledgeware Applications .................................... 305
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Overview
This book is intended for the user who needs to become quickly familiar with Knowledge Advisor. This overview provides the following information: • • • • • Knowledge Advisor in a Nutshell Before Reading this Guide Getting the Most out of this Guide Accessing sample documents Conventions Used in this Guide
Knowledge Advisor in a Nutshell
CATIA - KNOWLEDGE ADVISOR is a CATIA product which allows users to embed knowledge within design and leverage it to assist in engineering decisions, in order to reduce errors or automate design, for maximum productivity. Users can embed knowledge in design such as formulas, rules and checks and leverage it when required at any time. Knowledge is then taken into account and acts according to its definition. Its meaning is also accessible: For example a check intent can highlight the parameters involved in a verification, it is easy and immediate to understand in what way a standard has been violated. In short, Knowledge Advisor enables users to: • Capture corporate engineering knowledge as embedded specifications allowing complete consistency. • • • • • • • • Easily define and share know-how among all users. Automate product definition. Ensure compliance with corporate standard. Increase productivity. Increase Knowledge management for sharing and understanding intents. Build Knowledge components management for customization and reuse. Allow early attention to final design specifications preventing costly redesigns. Guide and assist users through their design tasks.
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Before Reading this Guide
Before reading this guide, you should be familiar with basic Version 5 concepts such as document windows, standard and view toolbars. Therefore, we recommend that you read the Infrastructure User's Guide that describes generic capabilities common to all Version 5 products. It also describes the general layout of V5 and the interoperability between workbenches.
Getting the Most out of this Guide
To get the most of this guide, we suggest that you start performing the step-by-step Getting Started tutorial. Once you have finished, you should move on to the User Tasks section. The Workbench Description section, which describes the Knowledge Advisor workbench, and the Customizing section, which explains how to set up the options, will also certainly prove useful.
Accessing sample documents
To perform the scenarios, you will be using sample documents contained in either the online/kwrug/samples folder. For more information about this, please refer to Accessing Sample Documents in the Infrastructure User's Guide.
Conventions Used in this Guide
To learn more about the conventions used in this guide, refer to the Conventions section.
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What's New?
New Functionalities
Deactivating and Re-activating External Parameters Users can now re-activate and synchronize external parameters previously deactivated.
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Getting Started
Using Parameters
This task explains how to use parameters. For a fuller outline of the parameters-related tasks, see Knowledgeware Infrastructure - Tips and Techniques - Summary dedicated to the knowledgeware infrastructure capabilities. Check the settings below: • From the Tools menu, select Options->General>Parameters and Measure.
•
In the Knowledge tab, check the With Value and Wi Formula check boxes, and click OK.
When working in a Japanese environment, check the Surrounded by the symbol' check box under Parameter names. • From the Tools menu, select Tools->Options...>Infrastructure->Part Infrastructure. Check at least the Relations and Parameters boxes the Display tab, and click OK. It is recommended to check all the options located below the Specification tree settings.
•
1. Open the KwrStartDocument.CATPart document. If you expand the Parameters node in the specification tree, the Material parameter is the only one displayed. At this stage of the scenario, don't pay any attention to this default parameter.
The Relations node can't be expanded as there is no default relation in a CATIA document.
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2. Click the
icon. The Formulas dialog box is displayed.
3. In the New Parameter of type scrolling list, select the Length type, then click the New Parameter type button.
4. In the Edit name or value of the current parameter field, replace the Length.1 string with PadLen and click Apply. A new parameter is added to the document parameter list both in the Formulas dialog box and in the specification tree. You have just created a user parameter. 5. Click OK in the Formulas dialog box to terminate the dialog. Keep your document open and proceed to next task.
Using Formulas
This task explains how a parameter can be constrained by a formula. See the Knowledgeware Infrastructure - Tips and Techniques - Summary dedicated to the infrastructure knowledgeware capabilities for more information on formulas.
1. Click the
icon. The Formulas dialog box is displayed.
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Getting Started
2. In the parameter list, select the PartBody Sketch.1 Radius.1 item, then click Add Formula. The Formula editor is displayed.
Radius
The icon located on the right is simply a rubber you can use to erase the formula. 3. Enter the 2 * PartBody Hole.1 Diameter relation.
4. Click OK in the Formula Editor once you have typed your relation. The Formula.1 relation is added to the specification tree. In the parameter list of the dialog box, a formula is now associated with the sketch radius. 5. In the parameter list, select the PadLength item, click Add Formula to create the formula below: PadLength = PartBody PartBody Pad.1 Pad.1 SecondLimit FirstLimit Length Length +
In the parameter list, the Formula.2 relation is now associated with the PadLength user parameter. In the specification tree, PadLength is also displayed with the value resulting from Formula.2. 6. Click OK twice in the Formulas dialog box to terminate this task. Keep your document open and proceed to the next task. This is now what you should see in the specification tree under "Relations":
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Using Rules
This task introduces the Knowledge Advisor rules. Unlike the parameter and formula capabilities which are available to all CATIA users, the rule and check capabilities require the Knowledge Advisor product. For more information about Rules, see Working with the Rule Feature. To know more about the Rule Editor, see Using the Rule Editor. 1. Select the KwrStartDocument item in the specification tree 2. Access the Knowledge Advisor workbench from the Start>Knowledgeware menu. 3. Click the rule icon. The following dialog box is displayed:
4. The dialog box fields display default values that can be modified: 5. a - The rule name: Rule.1. The first rule created in a document is Rule.1 by default. This name is the one displayed in the specification tree unless you modify the default name at creation. 6. b - The user and the date of creation. 7. c - The destination, i.e. the feature you are going to add the rule to. By default, in this scenario, the destination is the Relations feature (the Relations node in the specification tree). But a rule could be added to another feature, then only apply to this feature. 8. Replace the Rule.1 string with Cylinder_Rule, if need be modify the comments but don't modify the destination. Click OK. The Rule Editor is displayed (see below).
9. Type the code below into the edition box or copy/paste it from your browser to
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Getting Started
the edition box. PartBody Hole.1 Activity = true if PadLength <= 50mm and PadLength > 20mm { PartBody Hole.1 Diameter = 20mm Message("PadLength is: # | Internal Diameter is: #", PadLength,PartBody Hole.1 Diameter) } else if PadLength > 50mm and PadLength < 100mm { PartBody Hole.1 Diameter = 50mm Message("PadLength is: # | Internal Diameter is: #", PadLength,PartBody Hole.1 } else if PadLength >= 100mm { Diameter)
PartBody Hole.1 Diameter = 80mm Message("PadLength is: # | Internal Diameter is: #", PadLength,PartBody } else { Hole.1 Diameter)
PartBody Hole.1 Activity = false Message("PadLength is: # | Internal Diameter is: #", PadLength,PartBody } Hole.1 Diameter)
10. Users working in a Japanese environment should use the script below: `PartBody Hole.1 Activity` = true if `PadLength` <= 50mm and `PadLength` > 20mm { `PartBody Hole.1 Diameter` = 20mm Message("PadLength is: # | Internal Diameter is: #", `PadLength`,`PartBody Hole.1 Diameter`) } else if `PadLength` > 50mm and `PadLength` < 100mm { `PartBody Hole.1 Diameter` = 50mm Message("PadLength is: # | Internal Diameter is: #", `PadLength`,`PartBody } Hole.1 Diameter`)
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else if `PadLength` >= 100mm { `PartBody Hole.1 Diameter` = 80mm Message("PadLength is: # | Internal Diameter is: #", `PadLength`,`PartBody } else { Hole.1 Diameter`)
`PartBody Hole.1 Activity` = false Message("PadLength is: # | Internal Diameter is: #", `PadLength`,`PartBody } Hole.1 Diameter`)
11. Click Apply. An information window displays the PadLength and Pad internal diameter values. Click OK in the Information window. The Cylinder_Rule relation is added to the specification tree. 12. Click OK to terminate this part of the dialog. Keep your document open and proceed to the next task.
Using Checks
This task explains how to create a check and what happens when you add a check to a document. The Knowledge Advisor product is required for this task. See the Rule and Check Tasks for more information on check-related tasks.
1. Click the
icon. The first "Check Editor" dialog box is displayed.
2. Replace the Check.1 default name with Cylinder_Check, then click OK. The Check Editor box is displayed. It is similar to the Rule Editor. The Incremental box must be unckecked.
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Getting Started
3. Select the Information item in the Type of Check list. 4. Enter a string in the message field (for example: Pad too short). This message is to be displayed whenever the statement specified by the check is not fulfilled. 5. Enter the following statement into the edition box: PadLength > 20mm 6. Click OK to confirm the check creation. The Cylinder_Check relation is added to the specification tree. A green icon in the specification tree means that the check is fulfilled. No message is displayed. 7. Change the Pad limits so that PadLength <= 20mm. The Cylinder_Rule relation is re-applied. An information window displays the new PadLength and Pad internal diameter values. Then, you are warned by another window ("Pad too short") that the check is no longer valid. The check icon in the specification tree turns to red.
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User Tasks
Refer to the Quick Reference of Tasks for a comprehensive list of interactions to be carried out on rules and checks. See also the Useful Tips, the Limitations, and the CATIA Knowledgeware Infrastructure sections. This section shows you how to manage the Knowledge Advisor relations.
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Working with Parameters
Working with Parameters
Select the Formula icon to create parameters. Select the Add Set of Parameters icon to create sets of parameters. These sets of parameters are all grouped below the Parameters node. Select the Parameters Explorer icon to add new parameters to a feature. Select the Add parameters on geometry icon to add new parameters to a face, a vertex, or an edge.
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Introducing Parameters
When you create a part like the hollow cylinder of our "Getting Started" example, you often start by creating a sketch, then you create a pad by extruding the initial sketch, then you add other features to the created pad. The final document is made up of features which define the intrinsic properties of the document. Removing one of these features results in a modification of the document. These features are called parameters. Parameters play a prominent role in Knowledgeware applications. They are features that can be constrained by relations and they can also be used as the arguments of a relation. In addition to these parameters, CATIA allows you to create user parameters. These user parameters are extra pieces of information added to a document. User parameters are very handy in knowledgeware applications:
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knowledgewareAdvisor • • • They can be used to add specific information to a document They can be defined or constrained by relations They can be used as the arguments of a relation.
Parameters are created clicking one of the following icons: The parameters are created using the Formulas Editor. To find out more about this editor, see Getting Familiar With the f(x) Dialog Box. The parameters are created using the Parameters Explorer Editor. To find out more about this editor, see Getting Familiar with the Parameters Explorer. The created parameters only apply to edges, faces and vertex. The editor is similar to the Parameters Explorer editor. The Set of Parameters enables you to gather user parameters below a set.
A given relation may take as its arguments both types of parameters (intrinsic and user). For the parameters to display in the specification tree, check the settings below: • From the Tools menu, select Options>General->Parameters and Measure. In the Knowledge tab, check the With Value and With Formula check boxes, and click OK if you want the parameters to display their values and associated formulas (if any.) When working in a Japanese environment, check the Surrounded by the symbol' check box under Parameter names. • From the Tools menu, select Tools->Options...>Infrastructure->Part Infrastructure Check at least the Relations and Parameters boxes in the Display tab, and click OK.
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Creating a Parameter
This task explains how to create a Time type parameter and assign a value to it.
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1. Open the KwrStartDocument.CATPart document. 2. Click the icon. The f(x) dialog box is displayed.
3. Select the Time item with Single Value in the New Parameter of type list, then click New Parameter of type. The new parameter appears in the Edit name or value of the current parameter field. 4. Replace the Time.1 name with Machining_Time and assign the 1000s value to this parameter. Then click Apply. The Machining_Time parameter is added to the specification tree. The dialog box is modified as follows:
5. 6. Click OK when done to close the dialog box. • You can add properties to a .CATPart or a .CATProduct document by using the Properties command from the contextual menu. You just have to click the Define other properties... button in the Product tab then click New parameter of type. The dialog is similar to the f(x) dialog. See the Product Structure User's Guide for more information. The properties you define that way are also displayed in the parameter list of the f(x) dialog box. You can specify that a parameter is constant by using the Properties command from the contextual menu. This command also enables you to hide a parameter.
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Copy/Pasting Parameters
The Tools->Options->General->Parameters and Measure check boxes allow you to: • Paste a parameter without the formula which defines it. For example:
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knowledgewareAdvisor Holeplus= 15 = Diameter + 10 will be pasted as Real.i = 15 (if the With Value box is checked)
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Paste a parameter as well as the formula which defines it, but only if the parameters referred to in the formula are also selected in the copy. For example: Holeplus= 15 = Diameter + 10 will be pasted as Real.i = 15 if the Diameter parameter does not belong to the items selected for the copy but HolePlus will be pasted as Real.i = 15 = Real.j + 10 if Diameter is selected in the copy (use multi-selection).
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Paste a parameter as well as the formula. Holeplus= 15 = Diameter + 10 will be pasted as Real.i = Diameter + 10 When copying parameters sets containing hidden parameters, these parameters are automatically pasted when pasting the parameters sets and appear as hidden parameters.
Specifying the Material Parameter
Whatever your document, the Material parameter is always displayed in the specification tree. The Material parameter is created only after a material is applied to a Part or a Product. The Mechanical_Property features are calculated from the Material value. Specify a material to set the values of the Mechanical_Property features. 1. Open the KwrStartDocument.CATPart document. The Material parameter is displayed by default in the specification tree. Its value is set to None. 2. Double-click the Material feature in the specification tree to edit the parameter. The dialog box below is displayed.
3. Click OK and select the root feature in the specification tree. icon in the standard toolbar to display the available material 4. Click the library. Select the Metal->Iron material. 5. Click Apply Material and OK.
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This is what you should see now in the specification tree. The Iron feature is added to the specification tree and a new material is added under the Parameters node.
6. Remember: To display parameter values, check Tools->Options>General->Knowledge->Parameters and Measure->With value. 7. Keep your document open and proceed to the next task.
Valuating the Mechanical Property Parameters
Once the Material value has been specified, the Mechanical_Property parameters are automatically updated when the Properties option is selected in the contextual menu. 1. Select the root item in the specification tree and open the Properties dialog box from the contextual menu. 2. Select the Mass tab. The document mechanical properties have been updated from the value assigned to the Material parameter. 3. Click OK to go back to your document.
Specifying a Parameter Value as a Measure
This scenario shows how to assign a value to a parameter deducing it from a graphic selection. In this scenario, you deduce the value assigned to the Thickness parameter by selecting 2 circular edges. A common way to assign a value to a parameter is to use the Edit name or value of the current parameter field of the Formulas dialog box. But there is another way to proceed. The value you assign to a parameter can be deduced from a graphic selection. 1. In Tools->Options->General->Parameters and Measure, check the Load extended language libraries box of the Language tab. 2. Open the KwrStartDocument.CATPart document. 3. Click the icon. The f(x) dialog box is displayed.
4. Select the Length item with Single Value in the New Parameter of type list, then click New Parameter of type. The new parameter appears in Edit name or value of the current parameter. 5. Replace the Length.1 name with Thickness, then right-click in the value field of Edit
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name or value of the current parameter.
6. 7. Select the Measure Between... command from the contextual menu. The Measure Between dialog box is displayed. Select Edge only as Selection 1 mode and Edge only as Selection 2 mode. 8. In the document geometry area, select successively one of the inner circular edge of the part, then the outer circular edge located on the same face. The 17.5 mm value is displayed in the Measure Between dialog box.
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8. Click OK when done in the Measure Between dialog box. The 17.5 mm value is displayed in the Formulas dialog box. 9. Click OK to close the Formulas dialog box. The parameter is displayed below the Measure node in the specification tree and below the Parameters node. To edit this parameter: • • • Double-click it in the specification tree. The Edit Parameters dialog box is displayed. icon located next to the value field. The Click the Measure between dialog box is displayed. Edit the parameter and click OK when done.
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Importing Parameters
This scenario shows how to import parameters from an excel or a .txt file into a CATPart document. • Parameters and parameter values can be imported from a text file or from an Excel file (Windows) into documents (CATPart, CATProduct, Drawings...). If imported parameters already exist in the document, the import process automatically updates the document. Note that if 2 parameters have the same name in the import file, no clone is created and the parameters are not renamed. Make sure that the parameters have different names before importing them. Identical parameters names are not supported.
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Please find below the formatting rules the external file should comply with: • Column 1 Parameter names Column 2 Parameter values. Multiple values are allowed. Values should then be separated by a ";". The imported value is the one delimited by the "<" and ">" tags. Use the Tab key to skip from one column to the other in a tabulated text file. Column 3 Formula. If no formula is specified, the third column should be left empty. In a tabulated text file, just press the Tab key twice from column 2 to leave column 3 empty. Column 4 Optional comment.
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1. Open the KwrStartDocument.CATPart document. 2. Click the icon. The f(x) dialog box is displayed.
3. Click Import.... A file selection dialog box is displayed. 4. Select the ExCompanyFile0.xls file (Windows only) or the TxCompanyFile0.txt file, then click Open. The list of parameters to be imported into the KwrStartDocument.CATPart document is displayed.
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5. Click OK to import the parameters from the input file into the KwrStartDocument.CATPart document. The imported parameters are now displayed in the parameter list of the f(x) dialog box and in the specification tree.
6. Click OK to terminate the dialog.
Creating Points, Lines... as Parameters
The scenario below explains how to determine the position of the inertia axis of a pad. To do so, start from a pad, then: ) 1. Create a line by using either method ('datum' or 2. Use the inertiaAxis line constructor to specify that this line is to be the inertia axis of the pad. 3. Retrieve the coordinate of the point located at the intersection of the inertia axis and the pad extrusion plane.
To create elements such as Points, Lines, Curves, Surfaces, Planes or Circles and use them in knowledgeware relations, you can: • Create these elements as 'Isolate' elements in the Generative Shape Design workbench. 'Isolate' elements also called Datum are elements that have no link to the other entities that were used to create them. For information on 'Datum' type elements, see the Generative Shape Design User's Guide. Create these elements by using the f(x) capabilities and select the right type of element in the New parameter of type list.
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1. Access the Part Design workbench, create any sketch in the yz plane, then extrude this sketch to create a pad. If need be, refer to the Part Design User's Guide. 2. Create a line intended to be used as an inertia axis afterwards. 3. To do so, click the Formulas icon , select the Line item in New Parameter of type, then click New Parameter of type. 4. Click the Formulas icon. In the parameter list, select the line you have just created (Geometrical Set.1 Line.1).
5. Click Add Formula and add the formula below in the editor: Geometrical Set.1 Line.1 = inertiaAxis(3,PartBody) The inertiaAxis function is accessible through the Line constructors. The axis number 3 is the one which is in the extrusion direction (normal to yz). Click OK in the Formulas dialog box. The inertia axis is displayed in the geometry area. 6. Back to . Create three length type parameters: X, Y and Z.
7. Retrieve the coordinates of the point located at the intersection of the inertia axis and the 'yz plane'. To do so, create the formulas below: X=intersect(Geometrical Set.1 plane').coord(1) Y=intersect(Geometrical Set.1 plane').coord(2) Z=intersect(Geometrical Set.1 plane').coord(3) Line.1, 'yz Line.1, 'yz Line.1, 'yz
8. You get the intersect function from the Wireframe constructors and the point.coord method from the Measures item of the dictionary. 9. Check the value displayed in the specification tree as well as in the Formulas dialog box. The KwoGettingStarted.CATPart document used as a sample for the Product Engineering Optimizer User's Guide illustrates this scenario.
Applying Ranges to Parameters by Using a Rule
This task explains how to apply ranges to parameters by using a rule.
1. Open the KwrRangesParameters.CATPart. 2. Click the icon and select Real in the scrolling list to create two parameters of Real type: Real.1 and Real.2. 3. Select Real.1 and right-click the field next to the Edit name or value of the
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current parameter box. 4. Select Add Range The Range of Real.1 dialog box opens.
5. Specify the Minimum and the Maximum bounds (-5 and 5 for example), and click OK twice. 6. Access the Knowledge Advisor workbench and click the Rule icon ( Rule editor opens. 7. Enter the following rule: Real.2 =Real.1 .InferiorRange and click OK: Real.2 value changes to -5. ). The
8. Double-click the rule under the Relations node and replace the existing script with Real.2 =Real.1 .SuperiorRange and click OK: Real.2 value changes to 5.
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Creating an Associative Link Between Measures and Parameters
This scenario explains how to create a persistent and associative link between a measure created using the Measure Item or Measure Between command and a parameter. • Measure Item allows you to get the length of a curve (edge, line, curve), radius or angle depending on the parameter magnitude. Measure Between allows you to get the minimal distance or angle between two elements, depending on the parameter magnitude.
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This link can be created only if the Keep measure option is checked in the Measure Item and Measure Between dialog boxes (if not the result is copied as a simple value.) • No formula is created when using the Measure Item or the Measure Between commands. The icon located on the right of the editor field is a measure between or item icon. Note that you will be able to edit the measure.
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The parameters located below the Parameters node are directly linked to the measures. You can invert the sign of the parameter using the Invert value command in the Measure Item or Measure Between window. The sign concerns only the valuated parameters and not the parameter of the measure.
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To have an associative link, you must make an associative measure. If you select the Picking point mode and the Measure between function, the measure will not be associative. As a result, there will be no associative geometry. When a measure is not associative, the value is displayed in the value field. Even in the case of an associative measure, if you only want to get the result of the measure, uncheck the Keep measure check box.
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To create a "smart" customization, click the Customize... button in the Measure Item dialog box to see the properties the system can detect for the various types of item you can select.
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1. Open the KwrPlaneWing.CATPart file. The following image is displayed.
Using the Measure Item... command
2. Add a parameter of Length type. o Click the Formula icon ( o ). The Formulas dialog box is displayed.
In the New parameter of type scrolling list, select Length and click the New parameter of type button. Length.1 is displayed in the Edit name or value of the current parameter field. Right-click the value field of Length.1 and select the Measure Item... command. The Measure Item dialog box is displayed.
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Make sure the Keep measure option is checked in the Measure Item dialog box. In the specification tree, expand the Sketch.1 node, and select Spline.2. The selected item is highlighted in the geometry and its measure is displayed in green.
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Click OK in the Measure Item dialog box and OK in the Formulas dialog box. A new parameter is added below the Parameters node and below the Measure node. The Length.1 parameter is now linked to the result of the measure.
Using the Measure Between... command
1. Add a parameter of Angle type. o Click the Formula icon ( ). The Formulas dialog box is displayed.
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o
In the New parameter of type scrolling list, select Angle and click the New parameter of type button. Angle.1 is displayed in the Edit name or value of the current parameter field. Right-click the value field of Angle.1 and select the Measure Between... command. The Measure Between dialog box is displayed.
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In the Selection 2 mode scrolling list, select the Edge only option. In the specification tree, select Plane xy then select the geometry as shown below.
The selected items are highlighted in the geometry and the measure is displayed in green.
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Click OK in the Measure Between dialog box and OK in the Formulas dialog box. An angle parameter is added below the Parameters node and the measure is displayed below the Measure node.
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o
Click here to display the result sample.
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Note that: • • if several characteristics of the measure are computed and have the same magnitude, the system will choose the most convenient according to predefined rules. To remove the link to the measure, right-click the measure item in the specification tree and select the measure object->Remove the link with measure command.
Publishing Parameters
This scenario explains how to publish parameters. The scenario described below is divided into the following steps: • Add parameters to the Screw.2 document and publish its Diameter, Depth, and Volume parameters. Repeat the same operations with the second CATPart file. Create a CATProduct file and import Screw.2.
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In the context of the Bolt product, insert the Nut part that imports the Depth and the Diameter parameters by selecting the publication MyDepth and MyDiameter of Screw.2. In the context of the bolt, replace Screw.2 (KwrScrew.CATPart) by Screw.2 (KwrScrew2.CATPart) that doesn't have the same structure as the first one but owns the same publications. Both the parameters and the check are recomputed.
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A publication has a name and references a geometry or parameters inside the product (or one of its subproducts). The publication of parameters should be used when: • Defining an import of parameters between two parts (similar to the import of geometry). Defining relations at the assembly level between parameters (similar to constraints).
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Before you start, make sure that the Keep link with selected object check box is checked (Tools->Options->Infrastructure->Part Infrastructure->General). 1. Open the KwrScrew.CATPart document. The following image is displayed.
2. Add parameters to the part. icon. The Formula Editor opens. In the New parameter of type scrolling Click the list, select Volume and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the
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parameter: MyVolume. Click Apply and click the Add Formula button. The Formula Editor opens. o Enter the following formula by using the Dictionary: smartVolume(PartBody Click OK, and Yes. o Pad.1 ) + smartVolume(PartBody Pad.2 ) .
In the New parameter of type scrolling list, select Length and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: MyDepth. Click Apply and click the Add Formula button. Enter the following formula: MyDepth=PartBody Pad.2 FirstLimit Length and click OK.
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In the New parameter of type scrolling list, select Length and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: MyDiameter. Click Apply and click the Add Formula button. Enter the following formula: MyDiameter=PartBody twice. Sketch.2 Radius.2 Radius * 2. Click OK
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3. Publish the MyVolume, MyDepth, and MyDiameter parameters.
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To do so, select the Tools>Publication command and select the MyVolume, MyDepth, and MyDiameter parameters in the specifications tree. Click OK. The published parameters appear in the specifications tree below the Publication node. Close the file.
4. Open the KwrScrew2.CATPart and repeat the steps listed above (steps 1 to 3 included). The part should be identical to the one below. Close the file.
5. Create a CATProduct file. Select the Insert->Existing Component... command and click the root of the specifications tree. The File selection box is displayed. Select the KwrScrew.CATPart file and click Open. The screw is imported. 6. Select the Insert->Existing Component... command, select the Kwrnut.CATPart file and
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click Open. The nut part is inserted.
7. Double-click the inner circle of the nut, the Hole Definition window is displayed. o Right-click the Diameter field and select the Edit formula... command. The Formula Editor opens. Select MyDiameter in the screw publications. The formula should be as follows: PartBody o Hole.1 Diameter=`External Parameters
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MyDiameter`. Click O
Right-click the Depth field and select the Edit formula... command. The Formula Editor opens. Select MyDepth in the screw publications. The formula should be as follows: PartBody Parameters Hole.1 HoleLimit.1 Depth=`External
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MyDepth`. Click OK twice.
8. Double-click, then right-click the Screw.2 component in the specifications tree and select the Components->Replace Component... command. The File Selection window opens. Select the KwrScrew2.CATPart file and click Open. 9. Click Yes when prompted to replace all instances with the same reference as the selected product. Update the nut part: the parameters are recomputed.
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Activating and Deactivating a Component
This task explains how to activate and deactivate a component. In the scenario described below, the CATProduct file contains two CATPart files that you will activate and deactivate alternatively after creating user parameters and a rule based on these parameters. Note that: • Relations located at the product level are not integrated to the
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product update. If your relation drives the parameters of a Part, create the relation at the Part level. Parameters driven by rules are designed to enable you to control components activities at assembly level.
When working in a Japanese environment, remember to check the Surrounded by the Symbol' option (Tools->Options->General->Parameters and Measure->Knowledge tab).
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1. Open the KwrSyringe.CATProduct file and save the following files in the same directory (SyringePiston.CATPart, HollowSyringePiston.CATPart, and SyringeContainer.CATPart): This file contains a syringe made up of three different parts: A barrel, and two different plungers. 2. Create a multiple value parameter of string type. • • Click the icon. The Formulas Editor opens.
Select String in the scrolling list with Multiple Values. Click the New Parameter of type button. The Value List dialog box opens. Enter two different values, Hollow and Full, and click OK. Edit the name of the new parameter (SyringeType in this scenario) in the Edit Name or value of the current parameter and click OK. The new parameter is displayed under the Parameters node of the Specification tree.
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3. Access the Knowledge Advisor workbench and click the Rule icon to create a rule. The script of this rule will allow you to enable or disable one of the plungers. 4. Enter the code below in the Rule Editor, and click OK. if (SyringeType == "Hollow") { `S3\Component Activation State` `S2\Component Activation State` } else { `S2\Component Activation State` `S3\Component Activation State` }
= false = true
= false = true
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Note that Japanese users should enter the following rule.
6. Double-click the SyringeType parameter under the Parameters node and select Hollow in the Edit Parameter window. The SyringeBarrel CATPart and the HollowSyringePlunger CATPart are displayed.
7. Double-click the SyringeType parameter and select "Full" in the Edit Parameter window. The SyringeBarrel CATPart and the SyringePlunger
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CATPart are displayed.
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Creating an External Parameter
This tasks shows how to create an external parameter. • Make sure you have checked: o the Parameters and the External References check boxes below the Display in Specification tree settings in the Tools->Options->Infrastructure-> Part Infrastructure->Display dialog box, as well as the With Formula and With Value check boxes below the Parameter Tree View settings in the Tools->Options->General->Parameters and Measure dialog box.
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Open the DeactivatingExternalParameter.CATProduct file.
Note that the external parameters created at a product level are not integrated to the update process.
1. Expand the Part1_External_Parameter(Part1.1)\Part1_External_P arameter document, right-click the Line_Length parameter located below the Parameters node in the specification tree, and select the Copy command. 2. Double-click, then right-click Part2_External_Parameter (Part2.1)\Part2_External_Parameter and select the Paste Special command. In the Paste Special dialog box, select As Result With Link and click OK to validate. The External Parameters node is added to the specification tree and the Line_Length parameter is displayed.
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Deactivating and Re-activating External Parameters
This tasks shows how to deactivate, re-activate and synchronize external parameters. In the scenario described below, you: • • • • Create an external parameter Deactivate the external parameter Modify the parameter pointed by the external parameter Re-activate the external parameter
Until now, external parameters (external references) could be: • • synchronized (if their values were different from the values of the pointed parameter). isolated (external parameters become simple parameters) .
Now you can deactivate and re-activate external parameters. It means that when the external reference is deactivated, it cannot be synchronized with the pointed value, but it keeps its last value (the value cannot be changed any longer). The external parameter can also be reactivated: Its native behavior is then restored. Note that: • • •
A deactivated external parameter will only lose the ability to be synchronized and will keep its last value. A deactivated external parameter can be re-activated using its contextual sub-menu. The Activate, Deactivate, Synchronize, and Isolate commands can also be accessed from the Links dialog box (Edit->Links.) Make sure you have checked: o the Parameters and the External References check boxes below the Display in Specification tree settings in the Tools->Options->Infrastructure-> Part Infrastructure->Display dialog box. as well as the With Formula and With Value check boxes below the Parameter Tree View settings in the Tools->Options->General->Parameters and Measure dialog box,
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Open the DeactivatingExternalParameter.CATProduct file.
Creating the external parameter
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1. Expand the Part1_External_Parameter(Part1.1)\Part1_External_P arameter document, right-click the Line_Length parameter located below the Parameters node in the specification tree, and select the Copy command. 2. Double-click, then right-click Part2_External_Parameter (Part2.1)\Part2_External_Parameter, and select the Paste Special command. In the Paste Special dialog box, select As Result With Link and click OK to validate. The External Parameters node is added to the specification tree and the Line_Length parameter is displayed.
Deactivating the external parameter
3. Right-click this external parameter and select the Part2_External_Parameter\External Parameters\Line_Length object-> Deactivate command. A mask ( ) indicating that the paramete is deactivated is displayed next to the parameter name.
4. Double-click Part1_External_Parameter, right-click Line_Length twice in Part1_External_Parameter and select the Line_Length object->Formula->Edit... command. Modifying the parameter pointed by the external parameter
5. In the Formula Editor, modify the formula so that it matches the following formula: Line_Length=Length(PartBody\Line.1)*2. Click OK when done. The Line_Length parameter value updated in Part1_External_Parameter. Note that it is not updated in Part2_External_Parameter since th external parameter is deactivated. Re-activating the external parameter
6. Go back to the external parameter you've created, right-click it and select the Part2_External_Parameter\External Parameters\Line_Length object->Activate command. A mask ( ) indicating that the parameter is deactivated is displayed next to the parameter name. 7. Right-click it and select the Part2_External_Parameter\External Parameters\Line_Length object->Synchronize command. The parameter is updated and a mask ( ) indicating that the parameter is deactivated is displayed next to the parameter name.
Getting Familiar with the Parameters Explorer
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Contrary to the parameters created using the Formulas editor, the parameters created using the Parameters Explorer display below the feature selected in the specification tree.
icon in the standard tool The Parameters Explorer dialog box is displayed when you click the bar. This dialog box allows you to add parameters to features. It is made up of the following fields: • • • • • Feature Parameters Parameter Properties Ranges
Feature
This field indicates the item selected in the specification tree to which the parameter will be added.
Parameters
This field enables you to create the parameters that will be added to the feature that you selected in the specification tree. To know more about this field, see Getting Familiar With the f(x) Dialog Box.
Parameter
The Value field enables you to assign a value to the created parameter.
Properties
The Local Name field enables you to modify the name of the parameter that you created. The Name field indicates the way the parameter will be displayed in the editors. The Comment field enables you
Ranges
The Inf. Range check box, if checked, enables you to add
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an inferior range to the parameter.
to add comments to the parameter.
The Sup. Range check box, if checked, enables you to add an inferior range to the parameter. The Constant check box, if checked, enables you to lock the parameter. In this case, the parameter cannot be modified. The Hidden check box, if checked, enables you to decide if you want the parameter to be displayed or not.
Adding a Parameter to a Feature
This task explains how to add two parameters to a circular pattern feature. One parameter is a multiple value string, the other is a mass with upper and lower bounds. 1. Open the KwrBallBearing1.CATPart document. 2. In the specification tree, select the root feature, then select the Start->Knowledgeware->Knowledge Advisor command to access the Knowledge Advisor workbench. 3. In the specification tree, select the CircPattern.1 feature. 4. Click the Parameters Explorer displayed: icon, the dialog box below is
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5. In the New Parameter of Type list, select the String type, then in the opposite field ('With'), select the Multiple Values item. Click New Parameter of Type. 6. In the <Value list dialog box: a) enter the Type1 string, then press Enter b) enter the Type2 string, then press Enter c) click OK to go back to the Parameter Explorer dialog box. 7. If need be, rename the created parameter in the Local Name field and add a comment. 8. In the New Parameter of Type list, select the Mass type, then in the opposite field ('With'), select the Single Value item. Click New Parameter of Type. The MASS.1 name is displayed by default in the Properties and a default value of 0kg is assigned to the created parameter. 9. Modify these values as indicated on the figure below:
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10. Click OK. Both parameters are displayed in the specification tree right below the CircPatter.1 feature. Parameters added by using the Parameters Explorer are displayed right below the feature they are assigned. 11.
Adding a Parameter to an Edge
This task explains how to add parameters to an edge by using the Parameters Explorer. Note that this new function is designed to work on edges, faces and vertex.
1. Open the KwrSupport.CATPart file. The following image is displayed.
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2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 3. Click the Add Parameters on Geometry icon ( of Pad.2. ) and select the upper edge
The Parameter Explorer dialog box opens. 4. In the New Parameter of type scrolling list, select the Length parameter type, and click the New parameter of type button. 5. In the Local Name field, enter the name of the parameter. For the purpose of this scenario, enter Extract_Length, and click OK to validate. A new Extract feature is created and the parameter you just created is added to this feature.
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Parameters added by using the Parameters Explorer are displayed right below the feature they are assigned.
Locking and Unlocking a Parameter
This task explains how to lock and unlock parameters: 2 new commands are now available in the Knowledge toolbar: the Lock selected parameters... and the Unlock selected parameters... commands. 1. Open the KwrLockingUnlockingParameters.CATPart file. 2. Expand the Parameters node and click the f1 parameter. 3. In the Knowledge toolbar, click the Lock selected parameters... icon ( ) to lock this parameter. The parameter is locked (a lock is displayed next to the parameter in the specification tree.) 4. To unlock the parameter, select the f1 parameter in the specification tree and click the Unlock selected parameters... icon ( toolbar. Note that: ) in the Knowledge
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The Lock selected parameters... and Unlock selected parameters... commands enable the multiselection of parameters or features.
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The parameter contextual menu can be used to lock or unlock the parameter.
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The Lock selected parameters... and Unlock selected parameters... commands are recursive: If you select a feature, the parameters located below this feature are locked or unlocked. Parameters that do not have a 3D representation can be locked and unlocked. o o o Open the Formulas Editor to access the parameter. Select the parameter in the Parameters list In the Edit name or value of the current parameter value field, access the contextual menu and select the Lock/Unlock command. (click the graphic opposite to enlarge it.)
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Constraints can be locked and unlocked. o Select the constraint in the specification tree and click the Lock selected parameters... )/Unlock selected parameters A lock is displayed next to the constraint in the ( ) icon, or Sketcher. Locked constraints Right-click the constraint in the display in orange. specification tree and select the Lock the parameter/Unlock the parameter command. (
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Creating Sets of Parameters
This task explains how to create sets of parameters. You can create sets of parameters below the Parameters node of the specification tree. Using this capability enables you to regroup parameters by categories. 1. Check at least the Parameters and Relations options of the Display tab in the Tools->Options...->Infrastructure->Part Infrastructure settings. 2. Open any document containing at least one parameter or create a document and add a parameter to it (otherwise, you won't have the Parameters node displayed in the specification tree). 3. Click the icon, then select the Parameters node in the specification tree. The Parameters.1 (or Parameters.n) parameter set is added to the specification tree right below the Parameters node. 4. Click the icon to add a new parameter in the created parameter set. The Parameter Explorer dialog box is displayed. In the specification tree, select the Parameter Set you want to add a parameter to. The name of the parameter set is displayed in the Feature field of the Parameter Explorer dialog box. 5. Fill in the other fields of the Parameter Explorer dialog box. If need be, see Adding a Parameter to a Feature. 6. After you have finished specifying the new parameter, click OK in the Parameter Explorer dialog box. In the specification tree, you can expand the feature which represents the parameter set. A new parameter has been added below the parameter set.
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Parameters belonging to a parameter set can be reordered by using the Reorder... command from the contextual menu.
Working with Formulas
Working with Formulas
Select the Formula icon to specify relations between parameters.
Introducing Formulas Getting Familiar With the f(x) Dialog Box Using the Dictionary Creating a Formula Creating Formulas based on Publications Specifying a Measure in a Formula Using Geometry to Create a Formula Referring to External Parameters in a Formula Using the Equivalent Dimensions Feature
Introducing Formulas
Formulas are features used to define or constrain a parameter. A formula is a relation: the left part of the relation is the parameter to be constrained, the right part is a statement. Once it has been created, a formula can be manipulated like any other feature from its contextual menu. The formula language uses operators and functions of all types whereby you can perform operations on parameters.
Displaying Formulas in the Specification Tree
Formulas are relations and as such they can be displayed below the Relations node provided you check the 'Relations' box below the 'Specification tree' settings in the Tools->Options>Infrastructure-> Part Infrastructure->Display dialog box. In addition, formulas can also be displayed below the Parameters node provided you check: • the 'Parameters' box below the 'Specification tree' settings in the Tools>Options->Infrastructure-> Part Infrastructure->Display dialog box • as well as the 'With Formula' box below the Parameter Tree View settings in the Tools->Options->General->Parameters and Measure dialog box
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The Activity Parameter
A formula is a feature which is assigned a parameter called the activity. The activity value is a boolean. If the activity is set to true, the parameter value cannot be calculated from the formula. If a formula is created for a parameter which is not already constrained by another formula, the activity of the new formula is set to true by default. A parameter can be constrained by several formulas, but only one formula can be active at a time. Before activating a formula on a given parameter, you must deactivate the other formulas defined on the same parameter. Activity value Relation icon in the specification tree false true
Importing Formulas
Parameters as well as the associated formulas can be imported from an external file. Refer to Introducing Parameters and Importing Parameters for more information on how to import formulas.
Getting Familiar With the f(x) Dialog Box
The f(x) dialog box is displayed when you click the box allows you to: • Display the list of parameters • • Create parameters and formulas Import external files. icon in the standard tool bar. This dialog
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The parameter list
Basically, the parameter list displays the parameters related to the feature selected either in the specification tree or in the geometry area. If no feature has been selected, all the document parameters are displayed. The dialog box being open, you can select a given feature either in the tree or in the geometry area and display its related parameters. You can restrict the list of displayed parameters by using the Filter Name and Filter Type capabilities as well as the Incremental check box.
The Filter Name filter
This filter allows you to narrow the list of displayed parameters by specifying a substring. If you specify *Limit* as filter, only the parameter with Limit as sub-string will be displayed, for example: PartBody PartBody PartBody PartBody Pad.1 Pad.1 Hole.1 Hole.1 FirstLimit SecondLimit HoleLimit.1 HoleLimit.1 Length Length Depth Angle
The Filter Type filter
This filter allows you to restrict the list of parameters by specifying a type. Selecting User parameters will display only the parameters created by the New Parameter of type button.
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Selecting Hidden parameters will display only the list of parameters which have been declared as hidden by using the Hide command from the value field contextual menu. The Hide command is only available for user parameters.
The Incremental check box
Selecting a feature in the specification tree or in the geometry area is displayed in the editor only the first level of features right below the selected feature. The parameter list on figure above displays all the parameters related to the Pad.1 and Hole.1 features. Selecting Pad.1 in the tree (Incremental unchecked) will display the parameters below: PartBody PartBody PartBody Pad.1 Pad.1 Sketch.1 FirstLimit SecondLimit Radius.3 Length Length Radius
Checking Incremental restricts the list of parameters to the one below: PartBody PartBody Pad.1 Pad.1 FirstLimit SecondLimit Length Length
The 'Edit name of value of the current parameter' field
This field displays the parameter which has been selected in the parameter list. The value field on the right-hand side is grayed out when the parameter is constrained by a formula, a design table or any type of relations. Right-clicking this value field provides you with a number of commands whereby you can refine the parameter definition.
The New Parameter of type button
This button allows you to create a user parameter. This user parameter can be assigned a single value or multiple values (akin to the enum idea).
The Delete Parameter button
This capability operates only for user parameters.
The Add Formula button
When you create a formula, you specify that a parameter, whatever its type, is to be constrained by a relation. Clicking the Add Formula button displays the Formula editor. The formula which is created is displayed in the parameters list as well as its activity. To know more about the Dictionary available in the Formula editor, see Using the Dictionary.
The Delete Formula button
When a parameter which is constrained by a formula is selected in the parameter list, clicking Delete Formula removes the formula.
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The Import button
This capability allows you to import parameters and parameter values from a text file or from an Excel file (Windows).
Using the Dictionary
Using the Dictionary
The Dictionary allows you to access the functions, operators and feature attributes that can be used in relations. It can be accessed from the Formula Editor, the Rule Editor, the Check Editor, and from the Action Editor.
Packages displayed in the left part of the browser are those you selected from the Tools->Options ->General->Parameters and Measure->Language tab. Keywords Point Constructors Line Constructors Direction Constructors Messages and macros Measures Part Measures Object Design tables Law Circle Constructors Electrical Functions Attribute Surface Constructors Plane Constructors Math Operators Search Function String Space Analysis List Wireframe Constructors Analysis Operators
Constants
The following constants are specified or recognized by CATIA when programming rules and checks. As a result, they can be used anywhere in a relation in place of the actual values. • • • • false - one of the two values that a parameter of type Boolean can have true - one of the two values that a parameter of type Boolean can have PI - 3.14159265358979323846 - The ratio of the circumference of a circle to its diameter. E - The base of natural logarithm - The constant e is approximately 2.718282.
Electrical User Functions
About the Electrical User Functions...
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User Tasks • • • • • • Elec_DistanceCommon DistanceWireProduct ListAllOuterLayerObjects ListDirectlyCoveredObjects ListDirectlyOuterLayerObjects VisualMode
To be able to use these functions, you need to activate the ElectricalMeasure package. To do so: 1. Select Tools -> Options... -> General -> Parameters and Measures and go to the Language tab. 2. Choose the ElectricalMeasure package and click the right arrow: 3. Click OK to validate.
Elec_DistanceCommon
Syntax Elec_DistanceCommon(Wire1: Wire, Wire2: Wire):Length Returns the common length of the two wires given as input arguments. The type of Wire1 and Wire2 is ElecWire. Example 1 The Elec_DistanceCommon user function can be used in Knowledge Expert to find all the couples of wires in the session that have a common length greater than a given value. Example 2 In Knowledge Advisor, it can be used to define a rule giving the common length of two specific wires sharing properties. Applying the rule displays the following message if the condition is met: Example 3 Still in Knowledge Advisor, to verify that two wires selected in the specification tree have a common length, the following action can be defined: then ran: select two wires in the specification tree and click OK to validate. The following message displays:
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DistanceWireProduct
Syntax DistanceWireProduct(Wire1: Wire, Object: Product):Length Returns the minimum length between a wire and a product in session. The product must contain at least one part. Example 1 The DistanceWireProduct user function can be used with the f(x) command to display the distance between a wire and a component in the session. This formula returns the following value: Example 2 The DistanceWireProduct user function can be used in Knowledge Expert to find all the wires in the session that have a minimum distance to defined components smaller than a critical value chosen by the user. The components can be defined as heat-resistant. Properties have been added to the product: and to the wires: A check is defined as follows: Updating the session displays green/red light on the check: A report is generated showing the check result: some wires verify the condition, other not. Example 3 The DistanceWireProduct user function can be used in Knowledge Advisor to define a rule that displays a warning message if a minimum distance between a wire and an object is smaller than a critical value chosen by the user. Running this rule displays the following message: Example 4 Still in Knowledge Advisor, an action can be defined using the DistanceWireProduct user function, to know the distance between a wire and an object selected in the specification tree: Run the action using the Action.1 contextual menu:
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User Tasks select a wire and a product in the specification tree then validate. This message displays:
ListAllOuterLayerObjects
Syntax
ListAllOuterLayerObjects (ElecBundleSegmentExtremity:Feature,Offset:Real,ListOfAllCoveringProducts(Protections/Supports):out List):Boolean Returns an ordered list of protective coverings and supports that cover the bundle segment at the point of interest. The point of interest is defined by specifying from which end of the bundle segment and entering an offset in mm. Example A check (in KWE advanced language) to determine the protective coverings and supports at 150 mm from end 1 (Extremity 1) of the bundle segment is written as follows:
ListDirectlyCoveredObjects
Syntax ListDirectlyCoveredObjects((Protection/Support):Feature, ListOfCoveredProducts(BundleSegments/Protections/Supports): out List):Boolean Returns the list of bundle segments, protective coverings and/or supports directly under the component (protective covering or support) you want to analyze. If the component you want to analyze is not a protective covering or a support, the list returned will be empty. Example
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Tape A is placed directly over the bundle segment Corrugated tubes B and C are linked to the bundle segment, and corrugated tube B covers tube C Standard support D is linked to the bundle segment.
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knowledgewareAdvisor A check (in KWE advanced language) to determine the list of bundle segments, protective coverings and supports under corrugated tube C is written as follows:
Running this check returns: • • The name of the component analyzed, in our case, corrugated tube C The number of objects covered by corrugated tube C:
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Followed by the name of this component: the bundle segment.
ListDirectlyOuterLayerObjects
Syntax ListDirectlyOuterLayerObjects ((BundleSegment/Protection/Support):Feature, ListOfCoveringProducts(Protections/Supports): out List):Boolean Returns the list of outer layers of protective coverings and/or supports directly over the component (bundle segment, protective covering or support) you want to analyze. If the component you want to analyze is not a bundle segment, protective covering or a support, the list returned will be empty. Example
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Tape A is placed directly over the bundle segment Corrugated tubes B and C are linked to the bundle segment, and corrugated tube B covers tube C
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A check (in KWE advanced language) to determine the list of outer layers that directly cover the bundle segment in the example is written as follows:
Running this check returns: • • The name of the component analyzed, in our case, the bundle segment. The number of outer layers over the bundle segment:
Only 3 are found because corrugated tube B does not directly cover the bundle segment since it covers corrugated tube C. • Followed by the names of these components:
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VisualMode
Syntax VisualMode (BundleSegment: Feature, Visualization Mode (LIGHT/FULL): String): Boolean Description This function is useful to minimize the size of the harness in LIGHT mode. It simplifies the visualization, the curve and the diameter only are represented, the rib being deleted. This function is only available for bundle segments belonging to multi-branchable documents. Example Create a rule in Knowledge Expert:
Running this rule displays the harness in LIGHT mode:
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The rule is reversible: you can load a harness in LIGHT mode and reload the geometry by applying the rule with the FULL parameter:
The harness is displayed in FULL mode: the rib is recreated:
Working in LIGHT mode allows you to modify the route and route wires but the split, transfer and add branch point commands are not supported. To know more about these commands, refer to Electrical Harness Installation - Working with
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knowledgewareAdvisor Branches, Splitting Branches and Transferring Branches.
Creating a Formula
This task explains how to create a formula specifying that the external radius of a hollow cylinder is twice its internal diameter. Note that the radius of a sketch can be defined by a formula provided it is declared as a constraint. Make sure the Relations option is active in the Tools->Options...>Infrastructure->Part Infrastructure->Display tab. 1. Open the KwrStartDocument.CATPart document. icon to display the f(x) dialog box. Make sure that the 2. Click the Incremental box is unchecked. Method 1 o Double-click the PartBody Sketch.1 Radius.3 Radius parameter in the parameter list. The Formula Editor is displayed. Enter the PartBody Hole.1 HoleLimit.1 Depth*2 relation in the formula field. Go to Tips and Techniques for information on how to manipulate parameters and formulas. Click OK in the Formula Editor.
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Method 2 o Select the PartBody parameter list. Sketch.1 Radius.1 Radius in the
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Click Add Formula. The Formula Editor is displayed. Enter the PartBody Hole.1 HoleLimit.1 Depth*2 relation in the formula field. Go to Tips and Techniques for information on how to manipulate parameters and formulas. Click OK in the Formulas Editor.
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3. Click Apply to update the document. 4. Click OK to close the dialog box.
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Creating Formulas based on Publications
This task explains how to create a formula based on publications in a CATProduct file.
1. Open the Screw1.CATPart document. 2. Add a Volume parameter to the part. o icon. The Formula Editor opens. In the New parameter Click the of type scrolling list, select Volume and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: ScrewVolume1. Click Apply and click the Add Formula button. The Formula Editor opens. Enter the following formula by using the Dictionary to access the smartVolume operator: ScrewVolume1=smartVolume(PartBody times. Pad.1). Click OK three
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3. Create another Volume parameter called ScrewVolume2 based on Pad.2. 4. Create another Volume parameter called Volume_Total. Click OK when done to exit the Formula editor. 5. Access the Tools->Publication menu, and select the 3 parameters that display below the Parameters node. Assign them new names (see graphic below):
6. Click OK when done. The parameters, the formulas, and the publications are created (see graphic below).
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7. Save your file and close it. 8. Open the Screw2.CATPart document. Repeat the above steps (2 to 7).
9. Create a new product (File->New menu). Click OK when done. 10. Select the Insert->Existing Component... command to insert Screw1.CATPart into the product. 11. In the File Selection window, select the Screw1.CATPart file that you have just saved. Click Open. 12. Create a formula that will compute the volume of the screw. o Click the Root product and click the icon. The Formula Editor
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opens. o Enter the following formula into the editor by selecting the publications in the specification tree:
o o Click OK when done. The screw volume is displayed below the parameters node.
13. Double-click screw.1 in the specification tree, right-click it, and select the Components>Replace Component command. 14. In the File Selection window, select the screw2.CATPart file that you have just saved and click Open. 15. Click OK in the Impacts On Replace window. The new screw is inserted into the product and its volume is computed.
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Specifying a Measure in a Formula
The purpose of this task is to explain how to specify that the value of a Length type parameter is equal to the curvilign abcissa of a point located on a curve. Measures, i.e. values captured from the geometry area can be used in formulas. Here are some examples of measures that can be used in formulas: • • • Distance between two points. Total length of a curve. Length of a curve segment - between a point and the origin or between a point and the curve extremity. Length of a curve segment - between two points. Area of an extruded surface.
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1. Check the Load extended language libraries box in the Tools>Options->General->Parameters and Measure->language tab. 2. Open the KwrMeasure.CATPart document. The whole document has been created using the Generative Shape Design product. The Extrude.1 and Extrude.2 surfaces are extruded from the Spline.1 and Spline.2 curves. The point whose abscissa is to be measured is Point.5. The origin of the curve where Point.5 is located on is Point.8
3. Click the Formula icon. The f(x) dialog box is displayed. 4. Create the CurveLengthFromOrigin parameter.
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Select the Length item with Single Value in the New Parameter of type list, then click New Parameter of type. The new parameter appears in Edit name or value of the current parameter. Replace the Length.1 name with CurveLengthFromOrigin, and click Apply.
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5. Specify that the value of CurveLengthFromOrigin is the abscissa of Point.5: 4. a. Select the CurveLengthFromOrigin parameter in the parameters list, then click Add Formula. The Formula editor is displayed. b. Select the Measures item from the Dictionary list. c. In the list of measures, double-click the length(Curve,Point,Boolean) item. The length function is added to the Formula Editor.
d. Fill in the Formula editor field as indicated below. 1. The three arguments are: a curve to be selected from the geometry area, a point to be selected from the geometry area and a boolean. 2. Position the cursor where the first argument is intended to be typed. Then double-click the Spline.2 feature in the specification tree. The curve argument is added to the length definition. 3. Position the cursor where the second argument is intended to be typed. Then double-click the Point.5 feature in the specification tree. The point argument is added to the length definition. 4. Type a boolean for the third argument: True if the length is to be calculated from the origin, False if the length is to be calculated from the curve end.
5. Click OK to confirm the formula definition. You are
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back to the Formulas dialog box. The CurveLengthFromOrigin formula and value(47.5mm) are added to the parameter list. e. Click OK to add the parameter as well as its formula to the document.
Using Geometry to Create a Formula
This task explains how to use geometry to create a formula. Before performing this scenario, make sure you have checked the Keep link with selected object option (Tools->Options-> Infrastructure->Part Infrastructure->General tab.) 1. Create a Product and add 2 parts to this product. 2. From the Start->Shape menu, access the Generative Shape Design workbench. Select the first part. 3. Add a line to the part. 4. Select the second part and add a Length parameter to the part as well as a formula that will be based on the line. o Click the icon. The Formula Editor opens. In the New parameter of type scrolling list, select Legnth and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: LineLength. Click Apply and click the Add Formula button. The Formula Editor opens. Enter the following formula by using the Dictionary to access the length(Curve,...) operator: LineLength=length(). Position the cursor between the parenthesis and double-click the Line in the geometry or in the specification tree. The External parameter selection window is displayed. Select Line.1 and click OK. The formula is displayed as follows: LineLength=length(`External References\Line.1` ) Click OK when done. Click Yes in the Automatic update window.
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Refering to External Parameters in a Formula
This scenario shows how to use external parameters in a formula. In a formula, you can use parameters defined in external documents. This works between any types of document. For example, in a CATPart document, you can specify a formula referring to parameters defined in a CATDrafting document. External parameters can also be used when working within an assembly. Prior to performing this scenario, make sure that the Keep link with selected object option is checked (Tools->Options...->Infrastructure->Part Infrastructure->General).
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1. Open the KwrStartDocument.CATPart document as well as the KwrImportParameter.CATPart document. Select the Window->Tile Vertically command from the standard menu bar. Both documents are displayed. 2. Make active the KwrImportParameter document. Click the icon to display the f(x) dialog box. 3. Create a parameter of Length type and click the Add Formula button. The formula editor is displayed. 4. In the KwrStartDocument specification tree, select the Hole.1 feature. The External parameter selection dialog box is displayed.
5. In the External parameter selection dialog box, select the Diameter object in the external parameter list. Then click OK. The Length.1 definition is carried forward to the formula editor. (Click the picture below to enlarge it.)
6. Complete the formula definition as indicated below: Length.1 = Diameter*0.45 7. Click OK in the formula editor. You are back to the Formulas dialog box. In the parameter list, the Length.1 parameter value is modified according to the formula specified. In the KwrImportParameter specification tree, the External Parameters node is added. Expand this node to display the Diameter parameter.
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8. Click OK to add the formula to the KwrImportParameter.CATPart document and exit the dialog. 9. Select the Edit->Links command from the standard menu bar. The displayed dialog box confirms that there is a link between the KwrImportParameter KwrStartDocument Length.1 object and the PartBody Hole.1 Diameter object.
10. Click Isolate in the Links dialog box, then click OK. In the KwrImportParameter.CATPart specification tree, the External Parameters node can no longer be expanded and the Diameter parameter is added below the Parameters node.
11. Select the Edit->Links command from the standard menu bar. A message box informs you that the active document has no external links.
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Using the Equivalent Dimensions Feature
This scenario explains how to use the Equivalent Dimensions Feature. The scenario described below is divided into the following steps: • • you apply constraints to an existing sketch. you use the Equivalent Dimensions feature to create a list of Length type parameters that will have the same value.
To know more about the Equivalent Dimensions feature, see Getting Familiar with the Equivalent Dimensions Interface. 1. Open the KwrEquivalentDimensions.CATPart. The following image is displayed:
2. In the specification tree, expand the PartBody node and double-click Sketch.1 to access the sketcher. 3. Double-click the Constraint icon ( graphic below). ) to constraint some lines of the sketch (see
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4. In the Knowledge toolbar, click the Equivalent Dimensions icon ( Equivalent Dimensions Edition window is displayed.
). The
5. Click the Edit List... button. In the opening window, use the arrow key to select the following parameters and click OK when done. o o o Length.34 Length.36 Length.37
6. In the Equivalent Dimensions Edition window, set the value to 150mm and click OK. 7. Exit the Sketcher. The sketch is modified accordingly and the EquivalentDimensions.1 feature is displayed below the Relations node.
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8. Double-click Value=150mm twice in the specification tree. The Edit Parameter window is displayed. 9. Enter 140mm and click OK.
Associating URLs and Comments with Parameters or Relations
Associating URLs & Comments with Features
Link Bar 2
Assigning a Comment to a Knowledge Feature
This tasks shows how to add comments to parameters and formulas using the URLs & Comment toolbox as well as the Properties dialog box.
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You can now edit the text that is displayed in the contextual bubbles when dragging your mouse over a relation or a parameter so that you can assign a text to a particular feature. There are 2 ways to edit the text that is displayed in the contextual bubbles: 1. Select the feature to which you want to add a comment. 2. Click the Comment & URLs icon ( ). 3. Enter the text you want to display in the Comment field. 4. Click OK when done. - Or 1. Right-click the relation in the specificatio n tree. 2. Select the Properties command. 3. Enter the comment in the Comment field of the Properties dialog box. Note that:
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• •
if you want the value of the parameter/formula to display, the "\V" combination should be used (see example below). if no comment is added to the feature, the default name of the feature will be displayed.
1. Open the KwrComment.CATPart file. This file contains 3 Length type parameters and a formula that computes the length of a line. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 3. Click the Length.1 parameter in the specification tree and click the Comment & URLs icon ( ).
4. In the Comment field, enter Length.1 is equal to Length.2: \V. Click OK when done. 5. Right-click Formula.1 in the specification tree, and select the Properties command. 6. In the Comment field of the Properties dialog box, enter the following text: Formula that computes the length of the line. 7. Drag your cursor over Length.1 and Formula.1: The bubbles text is modified (see picture below.)
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Working with Design Tables
Working with Design Tables
Select the Design Table icon to create a design table. Introducing Design Tables Getting Familiar with the Design Table Dialog
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User Tasks Box Creating a Design Table from Current Parameters Values Creating a Design Table from a Pre-Existing File Interactively Adding a Row To the Design Table External File Controlling Design Tables Synchronization Storing a Design Table in a Power Copy If you are already familiar with CATIA and only need a quick access to information, see the CATIA Knowledgeware Infrastructure - Tips and Techniques - Summary.
Introducing Design Tables
A design table: • provides you with a means to create and manage component families. These components can be for example mechanical parts just differing in their parameter values. is a tool mainly intended to ease the definition of mechanical parts. It is provided to all CATIA users. But you will make the best use of it in a Knowledge Advisor application. A design table can be created from a CATIA document, the document data is then exported to the design table. It can also be applied to a document, the document data is then imported from the design table. is designed to drive the parameters of a CATIA document from external values. These values are stored in the form of a table either in a Microsoft Excel file on Windows or in a tabulated text file. When using a design table the trick is to associate the right document parameters with the right table parameters. The design table columns may not all correspond to your document parameters and you may decide to apply only part of the design table values to your document. By creating associations, you declare what document parameters you want to link with what table columns. • becomes a more powerful tool when it is used with the Knowledge Advisor. You are provided with functions to read the design table parameters. These design table functions can be used when programming your checks and rules. Using these functions spares you all the association operations. To know more, click here.
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Example
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knowledgewareAdvisor Screws are a good example of mechanical parts that can be described by a design table. To simplify, imagine they are all described by four parameters: the head width, the head height, the body width and the body height. The sets of four parameter values that can be assigned to a screw can be easily regrouped in a design table. This design table has as many columns as screw parameters and as many rows as sets of parameter values. In a design table, a set of parameter values is called a configuration and it is registered in a row. Design Table Formats • • • The Excel Sheet Format (under Windows) The Tabulated Text File Format The CATIA Design Table
Design Table Status
Design Tables Formats
The Excel Sheet Format (under Windows)
The values mentioned in the sheet cells have to be expressed in appropriate units. Otherwise, the right values won't be associated with the document parameters. Only Excel sheets created with Excel 97 and subsequent versions are supported.
If no unit is mentioned within a cell: • the unit taken into account is the one mentioned in the first row • and if no unit is specified in the first row, the unit taken into account is the relevant SI unit.
Here is an example of an Excel sheet: When a configuration which contains empty cells is selected, the parameters associated with the empty cells are not modified. This property enables you to modify parameters but only under certain conditions.
column name
column unit
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Within a given column, you can change the units.
Units can be specified in cells. No unit = SI
Note that it is highly recommended to choose the General format and not the Cells format in Excel.
The Tabulated Text File Format
Here is an example of a tabulated file format. You can use your favorite text editor to create this design table. Use the Tab key to skip from one column to the other. Unit rules are the same as for the Excel sheets.
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Under UNIX, it is possible to change the default design table editor. To do so, type: export CATTextEditorDT=... (indicate the path of the editor.)
The CATIA Design Table
Once it has been read and processed by CATIA, the design table looks something like this: No units in column Check box to modify the activity
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Displays the design table raw Values with units data.
Duplicates the design table external data into the CATIA document. Check this box whenever you intend to re-access your design table on another platform.
Design Tables Status:
Design tables can have different statuses: Synchronized: The Design Table is copied into the model ("Duplicate data in CATIA model" option checked) and the data stored in the model are synchronized with the content of the file. Not synchronized: The Design Table is copied into the model ("Duplicate data in CATIA model" option checked) and the data stored in the model are synchronized with the content of the file. (The .xls or .txt file was modified outside CATIA.) Inactive: The Design Table is deactivated. The associated parameters are not driven by the design table any longer. Broken: The Design Table is functionally KO because it cannot be used to valuate the associated parameters (data cannot be accessed because the file is lost or there are 2 columns with the same name ...). Light Broken: The filter is not compatible with the current configuration, or if the current configuration value does not correspond to one of the rows of the file.
Getting Familiar with the Design Table Dialog Box
Here is the dialog box sequence you get onscreen when you click the standard toolbar. icon in the
Creation of a design table
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"Create a design table from a pre-existing file" check box Check this option whenever you want to create a design table from the values of an external file. In this case, the created design table is made up of: • either only the columns whose name is a document parameter name. If the external file contains a "Length" column but no such "Length" parameter is defined in the document, the "Length" column will not appear in the created design table. This is the "automatic" association process. • or only the columns that have been associated one-by-one with a document parameter. If the external file contains a "Length" column but no so-called parameter in the document, you can choose to associate the "Length" column of the external with a parameter of the same type (a sketch radius for example).
"Create a design table with current parameter values" check box Check this option whenever you want to create a design table from a subset of the document parameters. You just have to select among all the document parameters the ones you want to be included as columns in the design table. In this case, the created design table only contains a single row. The Orientation check boxes These options allow you to choose the design table orientation. A vertical orientation is recommended when the design table contains many parameters.
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User Tasks The sheet index You can specify an Excel or Lotus sheet number. The Destination field All knowledgeware relations such as design tables, rules, checks or formulas, are created by default below the Relations node. Creating a relation below a given feature may help you organize your document. To specify a destination, select the default destination in the Destination field, then click the feature intended to be the new destination either in the specification tree or in the geometry area.
Selection of the parameters to insert
This dialog box pops up when you check the "Create a design table with current parameter values" check box.
There are two ways to restrict the list of parameters to be displayed in the 'Parameters to insert' list. You can use the: 1. Filter Name field Use the * character to specify any string to be included in a parameter name. Specifying *Len* will display in the "Parameters to insert" part of the dialog box all the parameters having the Len substring in their name. 2. and the Filter Type field. When you click OK in the dialog box above, the "Select the pathname of the file to be created" window is displayed.
Selection of the file to be created
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Use this dialog box to specify the .xls (Windows) or .txt file to be created. Specify the .xls extension when filling out the 'File name' field. Then click Open to display the design table dialog box. When working in a french environment, make sure that the decimal numbers contained in the text file linked to the design table are not written with a comma "," but with a decimal point. (This way you will be able to move to an english environment easily.)
Design table dialog box
The 'Configurations' tab
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User Tasks The current configuration as well as its number (< configuration number >) are highlighted. To change the current configuration, you just have to click the new configuration in the design table. A single row design table is created when you generate a design table with the current parameter values. • The Filter The filter is a means to help you query for a configuration meeting specific criteria. Click the "Edit... " button to display the "Design Table Request Editor". See Using the Dictionary for information on how to use the syntax provided by the dictionary. In a query, you can specify a condition referring to the design table parameters as well as the parameters external to the design table. • The "Activity" check box A design table is created active by default. The activity check box provides you with a way to deactivate the design table to be created. The "Edit table..." push button Click this button to display the edit table to be created. Depending on whether you have selected a .xls extension or not, you will launch a Microsoft Excel application or your default text editor for a .txt file. The "Duplicate data in CATIA model" check box Check this box whenever you intend to reuse your document on an operating system different from the one used to create the design table. That way, your design table data will be duplicated into your document.
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The "Associations" tab
This tab provides you with a way to associate the document parameters with the columns of the external design table. The left part of the dialog box allows you to associate parameters with the design table columns while the right part displays the list of associated parameters.
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The "Create parameters..." push button When a parameter is referred to in the design table but has not been created in the document, clicking this button allows you to create a parameter in the document and associate it with the right column of the design table. The "Rename associated parameters" push button If a parameter does not have the same name as the column it is associated with, you can rename this parameter so that it has the same name as the column. Clicking the "Rename associated parameters" push button displays a dialog box which asks you whether you want to rename all the parameters or only a few of them.
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Creating a Design Table from the Current Parameters Values
A design table is a feature that you create from your document parameters or from external data. No matter the existence of external data, you must create the design table in CATIA. There are two ways to create a design table: • • From the current parameter values From a pre-existing file.
The scenario described below explains how to proceed in the first case. The design table creation process includes the following steps:
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a. Create a table from the document parameters. b. Select the parameters to add to the design table. c. Specify a file to contain the generated design table. d. Edit the generated CATIA design table. e. Apply the design table to your document. For information on how to use the different dialog boxes related to the design table, see The Design Table Dialog. 1. Open the KwrStartDocument.CATPart document. 2. Click the Design Table icon in the standard toolbar. The Creation of a Design Table dialog box is displayed. See The Design Table Dialog for further information. 3. If need be replace the default name and comment for the design table. 4. Check the Create a design table with current parameter values option. 5. Click OK. The Select parameters to insert dialog box is displayed. 6. In the Parameters to insert list, select the PartBody Pad.1 FirstLimit Length and the
PartBody Pad.1 SecondLimit Length items. Then click the right arrow to add both items to the Inserted parameters list. 7. Click OK. A file selection box is displayed. 8. Specify the pathname of the design table to be created. Click OK in the file selection dialog box. The design table feature is added to the specification tree and a dialog box displays the newly created design table. This design table contains only one configuration. By default it is active. If the file specified already exists, the Creation of a Design Table dialog box is re-displayed as well as a message box asking you whether you want to overwrite the existing file. 9. Click Edit table... to start an Excel application (under Windows) or open the text editor under Unix. Replace the PartBody value with 80mm. Pad.1 FirstLimit Length parameter
10. Save your Excel or .txt file and close your application. Some information messages are displayed in a dialog box warning you about events related to the design table. Click Close. 11. Click Apply into the CATIA design table dialog, the document is updated as well as the CATIA design table. Click OK to exit the dialog and add the design table to the document.
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Creating a Design Table from a Pre-existing File
A design table is a feature that you create using your document parameters or external data. No matter the existence of external data, the design table must created in CATIA. There are two ways to create a design table: • • Using the current parameter values Using a pre-existing file
The scenario below describes how to proceed in the second case. Here are the main steps to follow: a. Select the pre-existing file containing the raw data. b. Create the associations between the document parameters and the external table columns. You can choose to create these associations automatically. c. Edit the generated CATIA design table. d. Select a configuration in the generated design table. You can modify the default configuration proposed by CATIA. e. Apply the design table feature to your document. For information on how to use the different dialog boxes related to the design table, see The Design Table Dialog. It is now possible to select a Design Table external file from a VPDM (ENOVIA LCA, ...). To do so, make sure you have enabled the desired environment in the Document Environments field (Tools->Options>General->Document.) Your documents will be accessible via the Document Chooser. 1. Open the KwrStartDocument.CATPart document. 2. Click the Design Table icon ( ) in the standard toolbar. The Creation of a Design Table dialog box is displayed. Enter a name (DesignTable1 for example) and a comment. 3. Check the Create a design table from a pre-existing file option. Click OK. 4. Select the KwrBallBearing.xls file, and click Open. A dialog box asks you whether you want to perform automatic associations between the design table columns and the document parameters which have the same name. 5. Click Yes. The Material parameter is the only one which is common to the document parameters and to the external design table. A multi-row design table is created. The '<' and '>' symbols denote the current configuration. 6. Select the configuration you want to apply to the document (line 4 for
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example). Click Apply. The Iron parameter value is displayed in the specification tree. 7. Click OK to end the design table creation.
The scenario below illustrates how to create a design table by associating one by one the document parameters with the input file columns. 1. Open the KwrStartDocument.CATPart document. Design Table icon in the standard toolbar. 2. Click the The "Creation of a Design Table" dialog box is displayed. Enter a name (DesignTable2 for example) and a comment. 3. Check the Create a design table from a pre-existing file option. Click OK. A file selection window is displayed. 4. Select the KwrBallBearing.xls file. Click Open. The Automatic associations dialog box is displayed. 5. Click No. The design table dialog box informs you that there is no associations between parameters and columns. Now, you have to associate one by one the document parameters with the design table columns. 6. Click the Associations option. The table design dialog box now displays side by side the document parameter list and the input file columns. 7. In the Parameters list, select the PartBody Hole.1 Diameter item. In the Columns list, select the d1 parameter. Then click Associate. A parameter couple is now displayed in the Associations between parameters and columns list. 8. Repeat the same operation for the Material parameter. Selecting a parameter or an association in the list highlights the corresponding values in the geometry area. The parameter list can be filtered: o By clicking on a feature (either in the specification tree or in the geometry area). All the parameter values of the selected feature (and children) are highlighted in the geometry area. The parameter list displays only the parameters of the selected features (and children). By specifying a string in the Filter Name field. For example, typing *ength* enables you to display all Length parameters By specifying a type in the Filter Type field.
o o
The Create parameters... button allows you to create automatically parameters and associations for items of the Columns list. The Rename associated parameters button replaces the parameter name with the
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column name. 9. Click OK to end the DesignTable2 creation dialog. The DesignTable2 feature is added as a relation to the specification tree. Double-click DesignTable2 in the specification to edit the table. By default, the configuration 1 is applied to the document. A new material (Aluminum) is applied to the document and the hole diameter is modified.You can select another configuration and apply it to your document.
Interactively Adding a Row To a Design Table External File
The task described below explains how to add a row to a design table external file. The scenario is divided into the following steps: • • • • You open the CATPart file and inserts the design table You deactivate the design table and creates a new configuration You add the configuration to the design table external file You activate the design table and implements the new configuration
This new function enables you to add a contextual menu on design table feature (in the tree) which appears only: • • • If the design table is deactivated If the design table external file exists and is read/write If at least one parameter is associated.
The behavior of this command is to add a row at the end of the design table file with associated parameters values. For not associated columns, an empty cell is added. To perform this scenario, you will need the following files: KwrAddARow.CATPart KwrAddARow.xls Note that this task can only be performed in an english environment.
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Prior to performing this scenario, make sure the With value and With formula options are checked in the Tools->Options->General->Parameters and Measure->Knowledge tab. 1. Open the KwrAddARow.CATPart file. The following image is displayed.
2. Click the Design Table icon (
).
3. Click the Create a design table from a pre-existing file radio button and click OK. 4. In the opening File Selection window, select the KwrAddARow.xls file and click Open. 5. Click Yes in the Automatic associations window: The design table opens. Click OK to close it. 6. Click the Measure update icon to update Formula.1. 7. Under the Design Tables node, double-click Configuration=1. The Edit Parameter dialog box is displayed. 8. Click the Design table icon in the Edit Parameter dialog box: The Design Table window is displayed. 9. In the dialog box, select the second configuration (line 2), click Apply, and OK twice. 10. Right-click Formula.1 in the specification tree and select the Local Update command. 11. In the Specification tree, right-click DesignTable.1 and select the DesignTable.1 object->Deactivate command. The design table is deactivated. 12. Modify the spline: • Double-click Point.1 twice in the specification tree or in the Geometry. Enter the coordinates indicated below into the Point Definition dialog box.
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•
Modify the coordinates of X Point.2 and Point.3 (see Y table Z opposite) Click OK when done.
Point 1 0 0 0
Point 2 100 100 -100
Point 3 50 50 -226
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13. Add the new configuration to the design table. To do so, right-click DesignTable.1 in the specification tree and select the DesignTable.1 object>Add row with current values command.
14. Right-click DesignTable.1 and select the DesignTable.1 object->Activate command. 15. Double-click Configuration=1 under DesignTable.1 and click the Design Table icon ( ).
16. In the DesignTable.1 window select the configuration that you have just added and click Apply and OK twice. The spline is updated accordingly.
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Controlling Design Tables Synchronization
This topic aims at providing you with short examples when working with design tables in the following modes: • • • Automatic Synchronization At Load Interactive Synchronization At Load Manual Synchronization
Automatic Synchronization At Load
When loading a model containing user design tables, if the design table files have been modified and the external file data is contained in the model, the design table will be synchronized automatically if this radio button is checked. 1. Open the KwrBallBearing1.CATPart file. The following image is displayed.
2. Click the Design Table icon ( is displayed.
). The Creation of a Design Table dialog box
3. Click the Create a design table from a pre-existing file option and click OK. The File Selection dialog box opens. 4. Select the KwrBearingDesignTable.xls file and click Open. Click Yes when prompted to associate the columns of the tables with the parameters. 5. Click OK to apply the default configuration. 6. Save your file and close it. 7. Open the KwrBearingDesignTable.xls file. Change the material of row 2 to Gold. Save your file and close it. 8. Go back to Catia. Open the part: The Part is updated accordingly to your changes.
Interactive Synchronization At Load
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When loading a model containing user design tables whose external source file was deleted, this option enables you to select a new source file or to save the data contained in the design tables in a new file. 1. From the Tools->Options... menu, select General->Parameters and Measure and check the Interactive Synchronization At Load option in the Knowledge tab. 2. Open the KwrBallBearing1.CATPart file. The following image is displayed.
3. Click the Design Table icon ( is displayed.
). The Creation of a Design Table dialog box
4. Click the Create a design table from a pre-existing file option and click OK. The File Selection dialog box opens. 5. Select the KwrBearingDesignTable.xls file and click Open. Click Yes when asked if you want to associate the columns of the tables with the parameters. 6. Click OK to apply the default configuration. 7. Save your file and close it. 8. Go to the directory containing the KwrBearingDesignTable.xls file and delete it. 9. Go back to Catia. Open the KwrBallBearing1.CATPart file: A dialog box is displayed asking you if you want to select a new file. Click the Select button and select a new Excel file.
Manual Synchronization
When loading a model containing user design tables, if the design table files have been modified and the external file data is contained in the model, the design table will be synchronized if this option is checked. To synchronize both files, right-click the design table in the specification tree and select the DesignTable object->Synchronize command or the Edit->Links command. 1. From the Tools->Options... menu, select General->Parameters and Measure and check the Manual Synchronization At Load in the Knowledge tab. 2. Open the KwrBallBearing2.CATPart file. This file already contains a design table whose values are identical to those contained in the
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KwrBearingDesignTable.xls file (Note that the KwrBearingDesignTable.xls file and the KwrBallBearing2.CATPart file should be located in the same directory.)
3. Select the Edit->Links command to edit the Excel file path and select the appropriate KwrBearingDesignTable.xls file. Save the file and close it. 4. Open the KwrBearingDesignTable.xls file and modify the material values for example. Close the file. 5. Go back to CATIA. Open the KwrBallBearing2.CATPart file. 6. Select the Edit->Links command and click the Synchronize button to synchronize both files. If the Duplicate data in CATIA model option is checked, and if you choose another design table file without using the Edit Table command in the CATIA session, the following message is displayed whatever the settings:
If the Duplicate data in CATIA model option is unchecked, the synchronization occurs automatically.
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Storing a Design Table in a Power Copy
This task shows how to store a design table in a power copy for later use. In this scenario, you want to instantiate the inner and the outer cages of a ball bearing in a different context. To do so, you create a power copy only containing the outer and the inner cages of an already existing ball bearing. This scenario is divided into the following steps: • Inserting the Design Table into the CATPart file • • Creating the Power Copy Instantiating the Power Copy containing the Design Table
To perform this scenario, the Product Knowledge Template license is required. To perform this scenario, you will need the following files: • • KwrBallBearing1.CATPart KwrBearingDesignTable.xls
To store a design table in a Power Copy, do not forget to select the parameters pointed by the design table. 1. Open the KwrBallBearing1.CATPart file. The following image is displayed.
Inserting the Design Table into the CATPart file
2. Click the Design Table icon ( ) in the Standard toolbar. The Creation of a Design Table dialog box is displayed. 3. Check the Create a design table from a pre-existing file radio button and
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click OK. The File Selection dialog box is displayed. 4. Select the KwrBearingDesignTable.xls and click Open. 5. Click Yes when asked for automatic associations and click OK. The Design table is displayed below the Relations node.
Creating the Power Copy
6. From the Start->Knowledgeware menu, access the Product Knowledge Template workbench (if need be) and click the Create a PowerCopy icon. The Power Copy Definition dialog box is displayed. 7. In the Specification tree, select the following items: o o o o o o o o o DesignTable.1 Shaft.1 Shaft.2 Shaft.3 Sketch.1 Sketch.2 Sketch.3 the Material Parameter. Click OK when done. The Power Copy is displayed below the PowerCopy node in the specification tree.
8. Save your file and close it.
Instantiating the Power Copy
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9. From the File->New menu, select Part in the List of Types and click OK. 10. If need be, from the Start->Knowledgeware menu, access the Product Knowledge Template workbench and click the Instantiate From Document icon. The File Selection dialog box is displayed. 11. Select the KwrBallBearing1.CATPart file and click Open. The Insert Object dialog box is displayed. 12. Select the yz plane in the specification tree and click OK. The Design Table is instantiated
Creating and Using a Knowledge Advisor Law
The scenario which is developed below illustrates how to create a Knowledge Advisor law, then use a combination of a Generative Shape Design law and a Knowledge Advisor law in the same relation. • The Evaluate method is to be used to calculate a parameter value when this parameter is defined by a Generative Shape Design law. Note that the result you obtain on completion of this task depends on the initial lines. You can replay the scenario with different lines and see how it affects the result.
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A Knowledge Advisor law is a relation whereby a parameter is defined with respect to another. Both parameters involved in a law are called formal parameters. Formal parameters and laws are specifically designed to be used in the creation of shape design parallel curves. A Generative Shape Design law can be used in a Knowledge Advisor law. Laws only specify a relation between one parameter and another single parameter.
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1. From the Start->Shape menu, access the Generative Shape Design workbench. 2. Define a working support using the Work on Support icon ( ).
3. Select the zx plane, for example, and click OK in the updated Work on Support dialog box without modifying any other parameter. 4. Click the Line icon ( 5. ). The Line dialog box is displayed.
Right-click in the Point 1 field, and choose the Create point command.
6. The Point Definition dialog box is displayed, the Point type and Plane fields being automatically filled. 7. Create a point at H:0mm and V:0mm, and click OK.
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8. Repeat the operation, right-click the Point 2 field from the Line dialog box to create another point at H:100mm and V:0mm, then click OK in the Point Definition dialog box. 9. Click OK in the Line dialog box to create the line. icon. If need be, use the 10. Access the Knowledge Advisor workbench and click the Tools->Customize command to access the icon. A dialog box similar to the one below is displayed. This editor is similar to the other relation editors. If need be, replace the default values specified in the dialog box fields.
11. Click OK. The law editor is displayed. The right-hand part allows you to create the parameters to be used in the law. The left-hand part is the law edition box. 12. Click the New Parameter of type button to create two real type parameters FormalReal.1 and FormalReal.2, then enter the law below into the edition window: FormalReal.1 = 5*sin(5*PI*1rad*FormalReal.2)+ 10
13. Click OK to add the law to the document. The Law.1 feature is added to the specification tree right below the Relations node.
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14. Select your document root feature and re-access the Generative Shape Design workbench. icon to create a curve parallel to the line created at the very beginning of the 15. Click the scenario. The Parallel Curve Definition dialog box is displayed. 16. Select the line that you previously created as the reference Curve.
Note that only positive laws, i.e. with positive values only, can be used when creating parallel curves (positive is to be understood as "strictly positive"). 18. Click the Law ... button. The Law Definition dialog box is displayed. 19. Click the Advanced Law type, click Law.1 in the specification tree and click Close.
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20. Click OK. A curve parallel to the selected one is created, taking the law into account.
The KwrCreatingaLaw.CATPart sample illustrates this scenario.
Using the Knowledge Inspector
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The Knowledge Inspector allows you to query a design to determine and preview the results of changing any parameters without committing themselves to actually changing the design. This "what if" analysis provides immediate feedback that helps you experiment and refine designs. While it is important to determine what happens when one or more parameters are changed, it is equally significant for you to see how a design can be changed to achieve a desired result. The Knowledge Inspector supports this by allowing you to query "how to" make a particular change. In short, the Knowledge Inspector is a tool designed to study impacts and dependencies. What if (impacts) Helps you understand to what extent changing any parameter of your design (such as material, pressure, or a dimensional parameter) changes the operation or design of the product on which you are working. Can be used to examine interactions of parameters with each other and with the rules that make up the product's specifications. A "Geometric Update" option enables you to visualize the result of your modification in the geometry area. How To Helps you determine how your design can be changed to achieve a (dependencies) desired result.
You shouldn't use the
capabilities with the Knowledge Inspector.
The 'What If' Mode
This task explains how to use the 'What If' mode. 1. Open the KwrFormula1.CATPart document and access the Knowledge Advisor workbench. 2. Click the Knowledge Inspector icon or select the Knowledge Inspector from the standard tool bar. The "Knowledge Inspector" dialog box is displayed. Check the 'What If' option. 3. Select the KwrStartDocument PartBody Pad.1 this stage, don't modify its value in the Equals field). FirstLimit Length parameter (at
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4. Click Apply. The following list of parameters and parameter values is displayed in the Then area.
5. The first line describes the parameter which has just been selected. The other lines describe the impacted parameters. 6. Use the Equals field to replace the KwrStartDocument PartBody Pad.1 FirstLimit Length parameter value with 60mm. Click Apply. In the Then area, the parameter values are updated as follows:
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7. The InitialValue column shows the initial parameter values (when you open the Knowledge Inspector). The OldValue column shows the parameter values resulting from the previous 'What if' operation. The Var (variations) columns show comparison operators between values located in adjacent columns. 8. Check the Geometric Update option to display in the geometry area the modifications resulting from the 'What If' operation. Click Apply to update the document in the geometry area. 9. Click OK to apply the values resulting from the current 'What If' operation to your document. Otherwise, click Cancel>. Note that: • Using the buttons reloads in the 'Then' area the previous or next values in the history of the 'What if" operations. Checking the Show All Parameters option displays all the document parameters. An f letter in the Dvn column indicates that the parameter is constrained by a formula. Selecting a parameter in the Then area while the Show All Parameters is checked, highlights the selected parameter in the parameter list above.
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Modifying a parameter value does not imply that the values of the impacted parameters are automatically updated by a 'What If' operation. For example, if a parameter is constrained by a formula such as: if Parameter1 > A then Parameter2 = B replacing the Parameter1 value with a value greater than A won't modify Parameter2 if Parameter2 was previously set to B.
The 'How To' Mode
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This task explains how to use the 'How To' mode. 1. Open the KwrFormula1.CATPart document. 2. Click the Knowledge Inspector icon in the standard toolbar. The Knowledge Inspector dialog box is displayed. Check the 'How To' option. By default, only the parameters which are constrained by a formula are displayed. 3. If need be, check the Show All Parameters to display all the document parameters. 4. Select the KwrStartDocument PartBody Hole.1 Diameter parameter (assuming that you would like to have this parameter modified). 5. Click Apply or Enter. The list of parameters to be modified in order to change the Hole.1 Diameter parameter is displayed in the 'Use' area. FirstLimit Length parameter.
6. Select the Pad.1
7. Check the What If option. 8. Modify the FirstLimit Length parameter in 'What If' mode.
9. Click OK to apply the parameter modification to your document.
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Note that: • Checking the Show All Parameters option displays all the document parameters. An f letter in the Dvn column indicates that the parameter is constrained by a formula. • Selecting a parameter in the 'Use' area while the Show All Parameters is checked, highlights the selected parameter in the parameter list above.
Working with the Rule Feature
Working with the Rule Feature
Select the Rule icon to create a rule, write its code, test its syntax and apply it to your document. A rule is a set of instructions, generally based on conditional statements, whereby the relationship between parameters is controlled. In addition, depending on the context described by the rule instructions, actions can be executed: • To set a value or a formula to parameters, including feature activity • • • To display information windows To launch Visual Basic macros stored in external files or in the V5 document. To affect points, curves and surfaces and thus allow contextual and automatic topological changes
In the specification tree, the rule is displayed as a relation that can be activated or deactivated. Like any feature, a rule can be manipulated from its contextual menu.
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knowledgewareAdvisor A rule is executed when one of its input parameters has changed or when one of its input features has changed and if you require the update of the rule. The consequence is that it is impossible for you to completely control when the rule is to be fired. As a result, rules should only manipulate parameters and features and should be used to control the status of a design (change of parameters and geometry).
If you want to control when the action takes place, you should use the Reaction feature. Creating a Rule Using the Rule Editor Using Rules and Checks in a Power Copy Using the Dictionary
Creating a Rule
The task described below explains how to create a rule which retrieves the abscissa of a point and, depending on the coordinate value, displays a message or another. This scenario uses two special functions allowing you to retrieve the coordinates of a point. These functions can be accessed from the Measures item of the Dictionary. To find out more about the Dictionary, see the Using the Dictionary. 1. Open the KwrMeasure.CATPart document. The whole document has been created using the Generative Shape Design product. The extruded surfaces are extruded from the Spline.1 and Spline.2 curves. The point whose coordinates are to be retrieved and tested is Point.5.
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2. 3. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. editor to create three Length type parameters: Point5X, Point5Y 4. Use the and Point5Z. icon. In the first dialog box which is displayed, enter a rule name 5. Click the (MeasureRule for example). If need be, replace the default comments. If you want to add the rule to be created to a specific relation set, specify a destination. To do so, see Creating Sets of Relations. 6. Click OK. The Rule Editor is displayed. 7. Enter the rule below in the edition window.
if Geometrical Set.1
Point.5.coord(1) > 0mm
Message("Point.5 abscissa is positive") else { Geometrical Set.1 Point.5.coord(Point5X, Point5Y, Point5Z)
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Message("Point.5 abscissa is: # ", Point5X) } 8. In the rule above, you can retrieve the Point.5 definition (Geometrical Set.1 Point.5) by double-clicking the feature in the specification tree. 9. Click OK. The message "Point.5 abscissa is: 0mm" is displayed. 10. Edit the Point.5 feature (double-click the object in the specification tree for example) and replace the Point.5 X value with 10 mm. The rule is in a to-beupdated status. See Updating Measures for information on relations to be updated. 11. Re-access the Knowledge Advisor workbench, then click the message box informs you that "Point.5 abscissa is positive"). icon. A
To find out more about the Rule Editor, see Using the Rule Editor.
Using Rules and Checks in a Power Copy
This task explains how to use rules and checks in a Power Copy. Rules and checks as well as other relations can be applied to a document by retrieving them from another document provided they have been stored in a power copy. For further information on the power copy mechanism, see the Generative Shape Design User's Guide.
1. Open the KwrMeasurePCopy.CATPart document. If need be, access the Generative Shape Design workbench. 2. In the standard menu bar, select the Insert->Knowledge Templates>PowerCopy... command. The Power Copy definition window is displayed. 3. In the specification tree, select the Rule.1 and Check.1 relations. Both relations are carried forward onto the Power Copy definition window. Click OK in the Power Copy creation window. Save and close your document. 4. Open the KwrSplineInPcopy1.CATPart document and access the Generative Shape Design workbench. 5. Select the Insert->Instantiate From Document... command from the standard menu bar. The Select PowerCopy dialog box is displayed. Select the document which contains the power copy storing the Rule.1 and Check.1 relations and click Open. The Insert Object dialog box is displayed. 6. Select the Spline.1 feature either in the specification tree or in the geometry area. Click OK. A message box launched by the check is displayed informing you that the Spline Length is < 100mm. Both relations are carried forward to the specification tree and the check icon is red. The rule has not been fired. 7. Open the KwrSplineInPcopy2.CATPart document and repeat the same operation (from step 5). An information box displays the Spline Length
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indicating that Rule.1 is fired. This time, the check icon is green is the specification tree.
Rules and checks can be stored in catalogs and instantiated later in a document. See Instantiating Knowledgeware Relations from a Catalog
Using the Rule Editor
The Rule Editor is intended to help you key in the check body using the Dictionary. It is made up of:
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In the Rule Editor, you can: • Restrict the list of parameters displayed in the dictionary: in the specification tree, simple click the feature you want to display the parameters. If the 'Incremental' option is selected, only the first level of parameters right below the selected feature are displayed, otherwise, all the parameters at all levels are displayed. Suppose your document contains a Geometrical Set feature which itself is made up of several Shape Design points. When the 'Incremental' box is unchecked, selecting the Geometrical Set feature in the specification will display all the parameters related to the points (the parameters which defines the coordinates are included in the list). When the 'Incremental' box is checked, selecting the Geometrical Set feature displays only the first level of parameters below the Geometrical Set (the point coordinates are not displayed). Insert the feature definition in a rule: in the specification tree, double click the feature you want to insert the definition. Check whether the rule syntax is correct: click Apply. Erase the contents of the edition window: click the Add the rule to the document: click OK. To find out more about the items displayed in the Dictionary, see Using the Dictionary or select one of the items and press the F1 key in Catia. To find out more about rules, see Creating a Rule. icon.
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Handling Errors
This task explains how to handle features that are in error. In the scenario described below, you are going to open a .CATPart file that is made up of 2 lines and a datum point. This point will be the intersection of the lines if they intersect, or the origin if they do not. To do so, you are going to create a rule. The use of geometrical operators to value geometry in relations may lead to update errors in the created features. If you value a datum point with the result of the intersection of 2 lines, these 2 lines may not intersect and the point is therefore in error. The Do not catch evaluation errors option which is available by selecting the relation in the specification tree and selecting the Properties command enables you: • • • To create features in error To know (through an error message) if a feature is in error and To make changes (or not) in case of errors.
Note that this error handling is only available for GSD features.
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1. Open the KwrErrorHandling.CATPart file. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. ) to create a rule that will react to the fact that the 3. Click the Rule icon ( datum point is the intersection of the 2 lines if they intersect or the origin if they do not. 4. In the Rule Editor, enter the following body: let x(Point) x =intersect(`Geometrical Set.1 Set.1 Line.2` ) if (x.Error==true) `Geometrical Set.1 else `Geometrical Set.1 Note that Japanese users should enter the following rule body: Point.5` = point(0mm,0mm,0mm) Point.5` = x Line.1` ,`Geometrical
5. Click OK when done. The intersect operator launches an error message if the intersection is empty.
6. Right-click the rule in the specification tree and select the Properties command. 7. Check the Do not catch evaluation errors check box and click OK when done. This way, the evaluation of the rule will be forced even if an update error occurs.
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Working with the Check Feature
Working with the Check Feature
Select the Check icon to create a check, write its code, tests its syntax and apply it to your document. A check is a set of statements intended to inform you if certain conditions are fulfilled or not. A check does not modify the document it is applied to. A check is a feature. In the document specification tree, it is displayed as a relation that can be activated and deactivated. Like any feature, a check can be manipulated from its contextual menu. Creating a Check Using the Check Editor Performing a Global Analysis of Checks Using the Check Analysis Tool Using Rules and Checks in a Power Copy Customizing Check Reports Using the Dictionary
Creating a Check
This task explains how to create a check.
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1. Open the KwrFormula0.CATPart document, select the root item in the specification tree and access the Knowledge Advisor workbench. 2. Click the Check icon . The first Check Editor dialog box is displayed.
3. Replace the default name with Cylinder_Check. If needed, add some comments to the Description field. If you want to add the check to be created to a specific relation set, specify a destination. To do so, see Creating Sets of Relations. By default, the check is created right below the Relations node. 4. Click OK. The Check Editor is displayed.
5. Select a type of check. Enter the message you want to be displayed in the information or warning box in case the check is not verified. 6. Enter the check statements in the edition window. You can simply Copy/Paste the following statements into the edition window:
Relations
Formula.1
Activity == false
7. Click Apply to test your check syntax. If the information message is displayed, the check syntax is correct. 8. Click OK to add Cylinder_Check to the relations node in the specification tree. A red icon is displayed in the specification tree meaning that the check is not valid. 9. Deactivate Formula.1, the check icon turns to green in the specification tree. Three parameters related to a check are displayed in the "Formulas" dialog box: • • • The activity The severity The result
When you select the result parameter, the icon indicating whether the check is valid or not is displayed opposite the value field. Double-clicking this icon opens the check editor. To find out more about the Check Editor, see Using the Check Editor.
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To find out more about the Check Editor, see Using the Check Editor.
Performing a Global Analysis of Checks
Performing a Global Analysis of Checks
This task explains how to perform an analysis of Knowledge Expert and Knowledge Advisor Checks. The scenario is divided into 2 major steps: • • parameters, formulas and checks are created, the checks analysis is run and the checks that failed are corrected.
To find out more about the Global Analysis tool and the Check Report, see Using the Check Analysis Tool and Customizing Check Reports. • For the check report to be correctly generated, go to Tools->Options->General>Parameters and Measure ->Report Generation, and select: - The Input XSL file under Input XSL. (An XSL file is provided by default. Click here to get a description of the generated XML file.) - The parameters you want to appear in the report under Report Content. - The Output directory under Output Directory. 1. Open the KwrCheckAnalysis.CATPart file. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 2. Create a parameter of Length type and assign it a formula. Click the icon. The formula editor opens.
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Select Length in the scrolling list to define the type of the parameter, click the New parameter of type button, change the name of the parameter (Length in this scenario), and click the Add Formula button. The Formula Editor opens.
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Under Dictionary, select Measures, and doubleclick distance(Body,Body). Position the cursor before the coma and double-click Point.1 in the specification tree or in the geometrical area. Position the cursor after the coma and doubleclick Point.2 in the specification tree. Click OK.
3. Create a parameter of Volume type and assign it a formula. o Click the o icon. The formula editor opens.
Select Volume in the scrolling list to define the type of the parameter, click the New parameter of type button, change the name of the parameter (Volume in this scenario), and click the Add formula button. Under Dictionary, select Part Measures, and double-click smartVolume. Position the cursor between the parentheses and select PartBody in the specification tree. Click OK.
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The parameters and the associated formulas are created
), change the 4. Access the Knowledge Advisor workbench, click the Check icon ( name of the check (Length in this scenario), and click OK. The Check Editor opens. 5. Enter the following script in the editor, then click Apply and OK. Length > 150mm
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The Knowledge Advisor Check is created.
6. Access the Knowledge Expert workbench, click the Expert Check icon, and change the name of the check (HoleCheck in this scenario). The Expert Rule Editor opens. 7. In the Condition tab, enter the following script: H:Hole Editor H.Diameter > 15mm
8. Click the Correction tab, select VB Script in the scrolling list and enter the following script in the editor: Dim aHole as Hole Set aHole = H.parent.Item(H.Name) Dim diam As Length Set diam = aHole.Diameter diam.Value = 16 MsgBox("Correction performed on "&H.Name) 9. In the Correction Comment field of the Correction tab, enter the following string, and click OK: Holes diameter should be greater than 15mm. 10. Select the Rule Base under the Relations node and click the Expert Check icon, change the name of the check (DraftandHole in this scenario), and click OK. The Expert Check Editor opens. 11. In the Condition tab, enter the following script, then click Apply and OK. H:Hole ; D:Draft Editor D.Activity AND H.Diameter > 12mm
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The checks are created (click the graphic opposite to enlarge it).
12. Click the
icon in the toolbar. The Global Analysis Tool opens.
13. Click the icon to update the status of the checks. The Checks lights turn to red in the specification tree. icon. An xml page opens indicating the items that failed. To find out 14. Click the more about this report, see Customizing Check Reports. icon to launch the correction method specified when creating the Expert 15. Click the check (See step 9). The checks have been corrected. Only the Advisor check (Length) could not be corrected: The value of the Length parameter is 100.175 mm (as indicated in the report) whereas it should be superior to 150mm (as indicated in the body of the check). 16. To correct the check, modify the value of the Length parameter. • • Double-click Point.1 in the geometrical area. The Point definition window opens. In the H: field, change the value of the point to 150mm. Click OK. The light of the check turns to green indicating that the check is passed.
Using the Check Analysis Tool
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knowledgewareAdvisor The Global Analysis Tool is designed to manage Expert and Advisor checks wherever they may be located in the specification tree. It helps you understand the validation status of your design and allows navigation by checks or violations and highlights failed components. You can: • Access information concerning failing items • • Gather information concerning objects and checks Perform automatic corrections if need be.
The Global Analysis tool can be accessed at the session level by clicking the icon in the toolbar. This icon provides you with a simple Checks status: All the checks are updated and could be fired successfully. The checks need to be updated. All the checks are updated and at least one of them is incorrect.
Check Analysis Tool Window
Click the
icon in the toolbar to access the Check analysis window.
Filter section This option enables you to apply a filter to the checks or to the items that failed.
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Check
Only the Expert and Advisor checks that failed when updating the check report are displayed.
Failure
All the items that failed when updating the check report are displayed.
Help section To display the help section associated with each item of the list, double-click the desired item. The following view is displayed: The check and the items that it controls are displayed in the view as well as its current status. The items entered when creating the check are displayed: • Associated comments • • • • • Type Attributes Variables Name Owner of the check...
In the graphic above, the selected check is TestHole, it checks the holes of the CATPart file (3 of them do not pass the check because their diameters is not superior to 15mm), and the attributes are displayed corresponding to the data entered when creating the check.
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Note that it is also possible to select the items associated with the check. To do so, double-click the desired item in the view: The Help section shows the information concerning this item (see graphic opposite.)
Toolbar Click this icon to generate the customizable check report. To find out more about the check report, see Customizing Check Reports. Click this icon to solve the checks created in your document. Click this icon to launch the correction method specified in the Check Editor when creating the check. For an example, see Performing a Global Analysis of Checks. Click here to display the URL associated with the object, or to assign an URL to an object. To know more, see Associating URLs and Comments with Parameters or Relations.
Introducing the Default Check Report
The default check report presents the Expert and Advisor checks that failed. This window lists the checks that failed and presents a percentage of the failed items per Expert Check.
Advisor Checks report
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The Advisor checks window lists the Advisor checks that failed and shows the following elements: - the body of the check (Length>150mm here) - the item(s) on which the check operates (here, the Length formula).
Expert Checks report
The Advisor checks window lists the Expert checks that failed and shows the following elements: - the Input items checked by the check operation. - the item(s) that failed (here Hole.1, Hole.2, and Hole.3).
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Remember that this report should not be used to generate macros or other files. It is provided as information only.
Customizing Check Reports
The reports generated by the Global Check Analysis Editor can be customized. You can choose to display a xml or a html report.
Displaying a HTML report
To generate a html report when performing the check analysis, go to Tools>Options->General->Parameters and Measure and select the Report generation tab. Select Html in the Select Configuration of the check report area. In this case, only the Check Advisor, the Check expert and the Passed objects options are available in the Report content area. You can specify the output directory containing the generated HTML report in the Select output directory field. Select Html if you use a Netscape browser.
Displaying a XML report
To display a XML report when performing the check analysis, go to Tools->Options>General->Parameters and Measure and select the Report generation tab. Select Xml in the Select Configuration of the Check Report area. The following window opens:
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The Report generation tab is made up of 4 different fields: The Input XSL, the Report Content, the Select output directory, and the HTML options fields. Input XSL field This field enables you to select the XSL style sheet that will be applied to the generated XML report. The StyleSheet.xsl file is the default XSL file, but you can use your own template. Report content field Failed Checks All Checks Check advisor If checked, the generated report will contain information about the failed checks only. If checked, the generated report will contain information about all the checks contained in the document. If checked, the generated report will contain information about all the Knowledge Advisor checks contained in the document. Parameters information Check expert If checked, the generated report will contain information about the parameters of the Advisor checks. If checked, the generated report will contain information about all the Knowledge Expert checks contained in the document. Passed objects If checked, the generated report will contain information about the objects that passed the Expert checks as well
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as information about the parameters of these objects (diameter, depth, pitch,...). Objects information If checked, the generated report will contain information about all the objects contained in the Expert checks as well as information about the parameters of these objects (diameter, depth, pitch,...).
Output directory field This field enables you to select the output directory containing the generated XML report. HTML options field This option is available for Windows only. It enables you to define if the report will be opened in a CATIA session (in this case, the check box should be checked) or if it will be opened in an Internet Explorer session (in this case, the check box should remain unchecked.) Note that it is highly recommended not to use this report as a basis for macros or for other applications. It is only provided for information purposes.
Using the Check Editor
The Check Editor is intended to help you enter the check body using the Dictionary. It is made up of 3 different areas:
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Three different types of checks can be used: • • • The silent checks The information checks The warning checks
Depending on the type of check and the result of the check, you will be warned as follows: Check verified Relation icon in the specification tree Silent check Information check Warning check Check not verified
no message displayed no message displayed
no message displayed
no message displayed the message specified at check creation is displayed in an information box the message specified at check creation is displayed in a warning box.
In the Check Editor, you can: • Restrict the list of parameters displayed in the dictionary: To do so, go to the specification tree, simple click the feature you want to display the parameters for. If the 'Incremental' option is selected, only the first level of parameters located right below the selected feature are displayed. If not, all the parameters at all levels are displayed. Insert the feature definition in a check: To do so, go to the specification tree, and double-click the feature you want to insert the definition for. Check whether the check syntax is correct by clicking Apply. Erase the contents of the edition window by clicking the Add the check to the document by clicking OK. To find out more about the Dictionary, see Using the Dictionary. To find out more about checks, see Creating a Check. icon.
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Using the Action Feature
This task explains how to use an action.
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The scenario described below is made up of 3 major steps: • You first create a pad containing an action. • • You store this action in a catalog You then import the action stored in the catalog into another CATPart product.
It is highly recommended to be familiar with the Part Design workbench to perform this scenario. 1. Access the Part Design workbench and create a Pad or open the KwrAction.CATPart file. 2. Create a parameter of volume type and assign it a formula. Click the icon, select Volume in the scrolling list, click the New Parameter of type button and rename the Parameter (V in this scenario).
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Click the Add formula button. The formula editor opens. Under Dictionary, select Part Measures, and double-click smartVolume. Position the cursor between the parentheses and select PartBody. Click OK, Yes (when prompted for an automatic update) and OK.
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) to 3. Access the Knowledge Advisor workbench and click the Action icon ( create an action. The Action editor opens. Enter the following script and click OK: Inputs B: Body field Editor B.Query("Pad","").Compute("+","Solid","smartVolume(x)",V) Message("Total volume of the pads under this body : #",V) • The action created above searches for the pads contained in the selected body and computes the volume of these pads.
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• • •
To find out more about Query and Compute, click here. To see the created .CATPart file, click here. Note that the arguments types must be written in English.
4. Save your file and store the created action in a catalog. • From the Start menu, select Infrastructure->Catalog Editor. The catalog editor opens.
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), or select the Insert -> Add Family... Click the Add Family icon ( commands from the main menu to display the Component Family Definition dialog box. Indicate the name of the family (ComponentFamily.2 in this scenario), and click OK. Double-click the ComponentFamily.2 family in the catalog structure ), or select the Insert -> Add and click the Add component icon ( Component... command to display the Description Definition dialog box.
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Click the Select external feature button. Go back to the geometry, select the Action.1 feature in the specification tree and click OK. Save your catalog. The action contained in your .CATPart file is now stored in the catalog you have just created.
5. Open the KwrReceiveAction.CATPart file.
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6. Click the Catalog icon ( ) to import the action stored in the catalog. Click the Browse ), select another catalog icon your catalog, and click Open. Double-click ComponentFamily.2, and double-click Action.1. The Insert object dialog box opens. (Click the graphic opposite to enlarge it.)
7. Select PartBody: the imported action displays the volume of the pads contained in this body. (Click the graphic opposite to enlarge it.) 8. Select Body.2: the imported action displays the volume of the pads contained in this body.
Working with the Reaction Feature
Working with the Reaction Feature
Click the Reactions icon to create a script specifying how to change some feature attributes when an event occurs. The reaction is a feature that reacts to events on its source(s) by triggering an action. It is designed to cope with the rules and the behaviors limitations and to create more associative and reactive design. A reaction is a feature that reacts to events
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User Tasks The source can be: • A selected feature (or a list of features) • A parameter (result of a test) Events can be: • General events on objects (creation, deletion, update, drag and drop, attribute changes) and parameter value changes. • Insert/Replace component • Object Drag and Drop
A reaction is similar to a rule in the fact that: • It is stored in the model. • It reacts to changes and can trigger modifications. • It also references other objects and parameters in the document and supports the replace mechanism. But • • Reaction features provide a better control over when the action has to be fired. Reactions enable you to perform more complex actions. Since you have better control when the action is triggered, and as you're not constrained by the update mechanism limitations, you can use all the power of any Visual Basic API (in CATIA but also in other automation applications...), and a Visual Basic macro can be called with arguments from an action. Reactions can be written to customize the update mechanism (to optimize user features, for example). Reactions can react to user actions (instantiation of a user defined feature), insertion of a component in an assembly, modification of a parameter... Reactions can be stored in the model and can be integrated in the definition of a power copy or user feature.
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The reaction feature is not integrated to the update contrary to the rule. If a reaction is launched when updating the document, it may impact the document.
Link Bar 3
Using the Reaction Feature Window
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You can access the Reaction window by clicking the Advisor workbench.
icon in the Knowledge
The Reaction window is made up of 3 major fields: The Source Type field, the Source field and the Action field.
Source Type
• Selection enables you to manually select one or more items in the specification tree or in the geometrical area. These items will be displayed in the Sources field. Owner enables you to link the action with a feature of the geometry or of the specification tree (see Using the Knowledge Advisor Reaction Feature: DragAndDrop Event where the reaction feature is linked with a Hole, for example). To link the reaction with an object of the geometry, click the Destination field and select an object in the specification tree or in the geometry.
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Sources Field
A reaction is a feature that reacts to events (see Available events below) on an object called the source and that triggers an action. The Sources field displays the selected items with which the reaction will be linked (only available if the Selection Source type is selected.)
Available events
The events available in this scrolling list depend on the source type selected in the Source type field. The reaction will be fired when one of the events detailed below happens. Available Events AttributeModification Explanation The reaction is fired because of a change in an attribute state. Only available if the Selection option is selected.
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BeforeUpdate DragAndDrop Insert Inserted Instantiation Remove Update ValueChange
The reaction is fired before a feature is updated. The reaction is fired after a feature is dragged and dropped. The reaction is fired when a feature is inserted. The reaction is fired after a feature is inserted. The reaction is fired when a User feature is instantiated. The reaction is fired when a feature is removed. The reaction is fired right after a feature is updated. The reaction is fired because of a parameter value change. Only available if the Selection option is selected.
FileContentModification The reaction is fired each time the file associated with the design table is modified.
Action Field
The action is triggered by a reaction that reacts to events on an object. This field enables you to select the language in which you want to write the action (VB or the Knowledge Advisor language) and to edit the action.
Edit action button
Click this button to access the Action Editor.
Action Editor
The action editor displayed depends on the language selected in the Action field. If Knowledgeware action is selected, the window below is displayed.
The Edition pane enables you to enter the body of the action.
The Dictionary is divided into 2 or 3 panes depending on the selected category: - The left-hand one displays the categories that can be used in an action. - The middle one lists the
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objects belonging to the selected category. - The right-hand one displays the members of the selected category.
If VB action is selected, the window below is displayed. - The Name field enables you to enter a name for the VB script. - The Comment field enables you to enter a comment associated with the VB script. - The Editor enables you to enter the VB script. - The Insert object resolution button enables you to select an object in the specification tree or in the geometry and to automatically add its resolution to the script. (Click the graphic opposite to enlarge it.)
Creating a Reaction: DragAndDrop Event Creating a Reaction: Insert Event Creating a Reaction: Inserted Event Creating a Reaction: Remove Event Creating a Reaction: AttributeModification Event Creating a Reaction: BeforeUpdate Event Creating a Reaction: ValueChange Event Using a Reaction with a User Feature: Instantiation Event Using a Reaction with a Document Template: Instantiation Event Creating a Reaction: Update Event Creating a Reaction: File Content Modification Event
Creating a Reaction Event
Creating a Reaction: DragAndDrop Event
This task explains how to use the DragAndDrop event in a reaction feature. In the scenario below, you are going to drag and drop a hole, which fires a
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reaction. a) The following information are displayed in a VB box when the rule is fired: • The type of feature. • Its name as well as its initial diameter.
b) You are prompted to click OK to convert the hole into a counterbored one or to click Cancel to skip the conversion. Note that this task could be carried out in the past by using the Behavior feature which has been replaced with the Reaction feature. For more information about Reaction features, see Working with the Reaction Feature. 1. Create .CATPart file and a pad with a hole or open the KwrReactionPad.CATPart file. 2. Access the Knowledge Advisor workbench and click the Reaction icon ( ) to create a reaction. The reaction dialog box opens. o In the Source type field, select Owner for the Reaction to be applied to the hole selected in the Destination area (see below). In the Available events list, select DragAndDrop for the reaction to occur when the hole is dragged and dropped. In the Action field, select VB action, to write the action in VB. Click the Destination area in the Reaction dialog box and select Hole.1 in the specification tree.
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3. Click the Edit Action... button, paste the following script in the editor, and click OK twice:
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Set H = DroppedFeature.Parent.Item(DroppedFeature.Name) Dim FeatureType, FeatureName, HoleType FeatureType = TypeName(H) FeatureName = H.Name HoleType = H.Type Str1 = "The feature to be dropped" Str2 = Str1 & vbCrLf & "is a " & FeatureType & " type feature" Str3 = Str2 & vbCrLf & "Its name is '" & FeatureName & "'" Str4 = Str3 & vbCrLf & "Its initial diameter is "_ & H.Diameter.Value & vbCrLf Str5=Str4 & vbCrLf &_ "Unless you click Cancel, it will be converted into a counterbored hole" Dim MyBox MyBox = MsgBox (Str5,1) if MyBox = 1 then H.Type = 2 H.HeadDiameter.Value = 20.0 H.Diameter.Value = 10.0 End If 4. Access the Part Design workbench. In the geometry, select the hole and drag and drop it. The following dialog box appears:
5. Click OK. The hole is converted into a counterbored hole (see graphic below).
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To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: AttributeModification Event
This task explains how to use the AttributeModification event in a reaction feature. In the scenario below, you are going to create a reaction based on the activity (activated or deactivated) of a point. If the point is activated, a message box is displayed. This reaction is designed to react to attributes modification (color, state, name, thickness...). Note that attribute modification events are not available for all features. If it is the case with the feature you have selected, select the attribute in the Select a source... window and use the ValueChange event. The reaction will be launched when the attribute is modified.
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1. Open the KwrAttributeModificationEvent.CATPart file. This file contains a point that is deactivated. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( dialog box opens. ) to create a reaction. The reaction o In the Source type field, select Selection and select Point.1 in the specification tree. In the Available events scrolling list, select AttributeModification. In the AttributesLabel scrolling list, select Activity for the reaction to be launched when the point is activated or deactivated. In the Action field, select VB action and enter the following text into the editor: MsgBox "Point.1 activated" Click OK when done. The reaction is created and is displayed below the Relations node in the specification tree.
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3. Double-click Point.1 in the geometry to access the Generative Shape Design workbench. 4. Right-click Point.1 and select the Point.1 object->Activate command. A dialog box is displayed indicating that Point.1 is activated. 5. Click OK. Point.1 is activated. To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: Insert Event
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This task explains how to use the Insert event in a reaction feature. In the scenario below, you are going to insert an element into the CATProduct document, which displays a message. 1. Open the KwrSyringeAssembly.CATProduct file. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( reaction dialog box opens. ) to create a reaction. The
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In the Source type field, select Selection for the Reaction to be applied to the element you select and select the syringe in the specification tree). In the Available events list, select Insert for the reaction to occur when an item is inserted into the CATProduct. In the Action field, select Knowledgeware action and enter the following message: Message("An element was added to your document"). This message will be displayed each time you insert a new component into the CATProduct. Click OK. A reaction is added to the Relations node in the specification
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3. Double-click the root of the specification tree, select the Insert->Existing Component... command and click the root of the specification tree. The File selection dialog box opens. 4. Select the KwrSyringePiston.CATPart file and click Open. 5. The new element is inserted and the reaction is fired. The following message is displayed:
To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: Inserted Event
This task explains how to use the Inserted event in a reaction feature. In the scenario below, you are going to insert an element into the CATProduct document, which displays a message.
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1. Create a CATProduct file called Container.CATProduct and insert the KwrSyringeContainer.CATPart file by using the Insert->Existing Component... command. Save your file and close it. 2. Create a CATProduct file called Plunger.CATProduct, rename the root of the specification tree to Plunger, and insert the KwrSyringePiston.CATPart file by using the Insert->Existing Component... command. Close the file. 3. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( dialog box opens. ) to create a reaction. The reaction
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In the Source type field, select Selection for the Reaction to be applied to the element you select (plunger in this example). In the Available events list, select Inserted if you want the action to be launched when the Plunger is inserted into the CATProduct. In the Action field, select Knowledgeware action and enter the following message: Message("Plunger inserted"). This message will be displayed after the plunger is inserted. Click OK. A reaction is added to the Relations node in the specification tree. Save the file and close it.
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4. Save the file and close it. 5. Open the Container.CATProduct file, select the Insert->Existing Component... command. The File Selection dialog box opens. Select the Plunger.CATProduct file and click Open. The message specified step 3 is
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displayed.
To find out more about the Reaction feature window, see Using the Reaction Feature Window.
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Creating a Reaction: Remove Event
This task explains how to use the Remove event in a reaction feature. In the scenario below, you are going to remove an element from the CATProduct document, which displays a message. 1. Open the KwrSyringeAssembly2.CATProduct file. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( dialog box opens. ) to create a reaction. The reaction
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In the Source type field, select Selection for the Reaction to be applied to the element you select (Syringe in this example). In the Available events list, select Remove for the reaction to occur after an item is removed from the CATProduct. In the Action field, select Knowledgewar e action and enter the following message: Message("An element was removed from your document"): This message will be displayed when you remove a component from the CATProduct. Click OK. A reaction is added to the Relations node in the
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3. Double-click the root of the specification tree, right-click the Syringe piston in the specification tree, and select Delete. The following message is displayed.
To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: ValueChange Event
This task explains how to use the ValueChange event associated with the reaction feature. The CATPart file contains a cable going through 3 points. You want the cable length to be optimized each time you modify the cable length. The scenario is divided into 3 parts: • • • you create an optimization you create a reaction you modify the cable length value
1. Open the KwrEventValueChange.CATPart file: It contains 3 points and a
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spline (called cable in this scenario).
2. From the Start->Knowledgeware menu, access the Product Engineering Optimizer workbench and click the Optimize icon ( window opens. 3. Enter the following data in the Optimization window: Problem tab Optimization type Optimized parameter Free parameters Minimization distance Geometrical Set.1 Algorithm Termination criteria Point.3 Z ). The Optimization
Simulated AnnealingConvergence speed Maximum number of updates: 100 Consecutive updates without improvements: 20 Maximum time (minutes): 5
Constraints tab New constraint `Geometrical Set.1 Point.3 Z` - max (Geometrical Set.1 Point.2 ,Geometrical Set.1 Point.1 <= 0mm 4. Click OK in the opening dialog box, click Run optimization. Z Z)
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5. Select an output file and click Save. 6. Click OK once the optimization process is over. 7. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( ). The Reaction dialog box opens. • In the Source type field, select Selection and select the CableLength parameter in the specification tree for the Reaction to be applied to the CableLength parameter. In the Available events list, select ValueChange. In the Action field, select VB action.
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8. Click the Edit action... button, paste the following script in the editor, and click OK twice: Dim partDocument1 As Document Set partDocument1 = CATIA.ActiveDocument Dim part1 As Part Set part1 = partDocument1.Part Dim relations1 As Relations Set relations1 = part1.Relations Dim optimizations1 As Optimizations Set optimizations1 = relations1.Optimizations Dim anyObject1 As Optimization Set anyObject1 = optimizations1.Item("Optimization.1") anyObject1.Run False
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The reaction is added to the specification tree.
9. Double-click twice the CableLength=400mm parameter and change its value to 600mm: The optimization is launched (the RealLength and the distance parameters have changed) and the geometry is changed accordingly. To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: BeforeUpdate Event
This task explains how to use the BeforeUpdate event in a reaction feature. In the scenario below, you are going to optimize the position of a point each time you modify the length of the cable (spline). You create your geometry and insert all the components in a User Feature (UDF). This UDF contains the geometry of a cable going through 3 points: • The two points located at both extremities are to be specified in input. The coordinate of the third point is optimized in order to reach a target length for the cable.
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This target parameter is a published parameter of the UDF. The optimization is launched by using a VBMacro with argument, called in a Reaction to the "Before Update" event of the UDF. This scenario requires the Product Engineering Optimizer product.
1. Open the KwrEvent_BeforeUpdate.CATPart file: It contains 3 points and a spline (called cable in this scenario).
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2. From the Start->Knowledgeware menu, access the Product Engineering Optimizer workbench and click the Optimize icon ( Optimization window opens. 3. Enter the following data in the Optimization window: Problem tab Optimization type Optimized parameter Free parameters Minimization distance Geometrical Set.1 Algorithm Termination criteria Point.3 Z ). The
Simulated AnnealingConvergence speed Maximum number of updates: 100 Consecutive updates without improvements: 20 Maximum time (minutes): 5
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New constraint
Geometrical Set.1 Point.3 Z` - max (Geometrical Set.1 Point.2 ,Geometrical Set.1 Point.1 <= 0mm Z) Z)
4. Click OK in the opening dialog box, click Run optimization. 5. Select an output file and click Save. 6. Click OK once the optimization process is over. 7. From the Start->Knowledgeware menu, access the Knowledge Advisor ). The Script Editor workbench and click the Macros with argument icon ( opens. Enter the following data in the editor and click OK: Argument Script body optim optim.Run false
8. Click the Reaction icon (
). The Reaction dialog box opens. • • In the Source type field, select Owner. In the Available events list, select BeforeUpdate. In the Action field, select Knowledgeware action.
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9. Click the Edit action... button, paste the following script in the editor, and click OK twice: if (CableLength <= distance (Geometrical Set.1 Point.1
,Geometrical Set.1 Point.2 )) Message ("Incompatible inputs: cable length is less than distance between points!") else { `VB Script.1` .Run(Relations Optimizations.1 Optimization.1 )
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10. Double-click the root of the specification tree and select the Insert>UserFeature->UserFeature Creation... command. The User Feature Definition window opens. 11. In the Name field, enter the name of the UDF: Cable1 in this scenario. 12. Select the Spline, Point3, Reaction.1, VB Script.1, Optimization.1, the 4 formulas, and the parameters: they are displayed in the User Feature definition window (see below.)
Note that the UDF becomes the owner of the reaction. This reaction will be fired before the update of the UDF instance. 13. Click the Parameters tab, select CableLength, click the Published name check box and click OK. 14. Save the file and close it. 15. Create a new .CATPart file, access the Generative Shape Design workbench, and create 3 points. 16. Select the Insert->Instantiate From Document... command. The File Selection window opens. Select the KwrEvent_BeforeUpdate.CATPart file you just saved and click the Open button. 17. The Insert object dialog box opens. Select Point.1 and Point.2 in the geometry or in the specification tree and click OK. The cable (UDF) is instantiated and the optimization is launched before the update. 18. Repeat steps 14 and 15: select Point.2 and Point.3 when instantiating the UDF: the cable lengths are optimized.
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19. Double-click the CableLength=400mm parameter and change its value to 200mm. This cable length is optimized once again just before the update. To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: File Content Modification Event
This task explains how to use the FileContentModification event associated with the reaction feature. This event launches a reaction each time the file associated with the design table is modified. 1. Open the KwrBallBearing1.CATPart file. The following picture is displayed.
2. Click the Design Table icon ( is displayed.
). The Creation of a Design Table dialog box
3. Click the Create a design table from a pre-existing file option and click OK. The File Selection dialog box opens. 4. Select the KwrBearingDesignTable.xls file and click Open. Click Yes when asked if you want to associate the columns of the tables with the parameters. 5. Click OK to apply the default configuration. 6. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( opens. ). The Reaction dialog box • In the Source type field, select Selection and select the DesignTable.1 in the specification tree for the Reaction to be applied to the design
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table. • In the Available events list, select FileContentModification. In the Action field, select Knowledgeware action and enter the following message: Message("The design table was modified"). Click OK when done. The Reaction feature is added to the Relations node.
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7. Double-click DesignTable.1 in the specification tree. The Design Table window is displayed. 8. Click the Edit table... button and change the material of row 2 to Gold. Save your file and close it. The reaction is launched and the message is displayed.
To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Creating a Reaction: Update Event
This task explains how to use the Update event associated with the reaction feature. The CATPart file contains a rulebase that is updated each time a modification is made. 1. Open the KwrEvent_Update.CATPart: It contains a part with holes and a rulebase made up of 2 checks.
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2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench and click the Reaction icon ( ). The Reaction dialog box opens. • In the Source type field, select Selection and select the RuleBase in the specification tree for the Reaction to be applied to the rulebase. In the Available events list, select Update. In the Action field, select Knowledgeware action and enter the following message: Message("Rulebase updated").
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3. Double-click the CATKWECheck.1. The Check Editor opens. Modify the check: (H Diameter == 20mm) and click OK 4. Right-click the rulebase and select the Rulebase object->Manual Complete Solve command. The reaction is fired and the following message is displayed:
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To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Using a Reaction with a User Feature: Instantiation Event
This task explains how to use a reaction in a User Defined Feature. The scenario described below is divided into two major steps: • In the first step, you first create a formula that returns the length of the line, you create a reaction that will add items of length type to a list when the document is instantiated and then you create a UDF containing the line, the reaction and the formula. In the second step, you open a second document, you create a rule based on a list that will display the total length, and then you instantiate the UDF that you previously created in this document.
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A basic understanding of the Part Design workbench and of Product Knowledge Template is required to perform this scenario. Note that the Instantiation event is available for User Features only. It cannot be used with Power Copies. 1. Open the KwrUDFandReaction.CATPart file. 2. Create a parameter of Length type and assign it a formula. • icon, select Length in the New Parameter of Click the Type scrolling list, click the New Parameter of type button, and click the Add Formula button. In the Dictionary, click Measures, and double-click length
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(Curve,): Length. • Position the cursor between the parentheses and double-click Line.1 in the specification tree. Click OK, Yes, and OK. (Length.1=length(Geometrical Set.1 3. Access the Knowledge Advisor workbench, click the List icon ) to ( create a list, and click OK. An empty list appears under the Parameters node. Line.1)).
4. Click the Reaction ( o o o
) icon. The Reaction editor opens:
In the Source type list, select Owner. In the Available events, select Instantiation. In the Action area, select Knowledgeware action and click the Edit action button. The Action editor opens. Click the list in the specification tree and, in the Dictionary pane select List, and in the Member pane, double-click List.AddItem. Position the cursor between the parentheses and enter Length.1 before the comma, and 0 after the coma. Click OK twice. The Reaction feature is created.
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5. Access the Part Design workbench and select the Insert->UserFeature>UserFeature creation command. The Userfeature Definition window opens: in the Definition tab, enter the name of the User Feature (UserFeature1 in this scenario) and select the Line, the Reaction, and the Length parameter in the specification tree. Click OK. The UserFeature1 is created and displayed under the Knowledge Templates node.
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6. Save your file, close it, and open the KwrUDFandReaction2.CATPart file This is the file into which you will instantiate the UDF you previously created. 7. Access the Knowledge Advisor workbench, and click the list icon ( create an empty list and click OK. ) to
8. Create a parameter of Length type (called Length.1 in this scenario) and apply a formula to it. icon, select Length in the scrolling list, click the New Click the Parameter of type button, and click the Add Formula button. Select the list in the specification tree, in the Dictionary pane select List, and in the Member pane, double-click List.sum. Click OK three times. ), click OK, enter the following script in the Rule
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9. Click the Rule icon ( Editor, and click OK:
Message("Total Length : #",Length.1 ) 10. The total length is displayed: 0mm. 11. Access the Part Design workbench and select the Insert->Instantiate from Document command. 12. Select the file you created (from step 1 to step 5, KwrUDFandReaction.CATPart in this scenario) and click Open. The Insert Object window opens: • • • Select Point.1 in the specification tree or in the geometry. Select Point.2 in the specification tree or in the geometry. Select List.1 in the specification tree and click OK. The rule is fired and the Total Length is displayed.
Creating a Loop in a Reaction
This task explains how to create a loop in a reaction. In the scenario described below, you are going to: • • • Create 3 points that are inserted into a list Create a formula that will automatically fill in the list Create a reaction that will set the Z coordinate of the points to
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• •
20mm if this value is inferior to 20mm. Create a reaction that will set the Y coordinate of the points to 40mm if this value is inferior to 40mm. Update the Part
It is now possible to create the While and the For constructs. To know more, see Using the Knowledge Advisor Language. 1. Create a Part containing 3 points. 2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 3. Click the List icon ( 4. ) to create the list that will contain the created points.
Add a formula to fill in the list. o Click the Formula Editor icon. The Formula Editor is displayed. In the specification tree, select List.1 and click the Add formula button. List.1=PartBody.Query("Point",""). Click OK twice when done. Note that Japanese users should enter the following formula.
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6. Click the Reaction icon (
). The Reaction dialog box opens. • In the Source type field, select Selection and select the list in the specification tree for the Reaction to be applied when the list is modified. In the Select a source... dialog box, select List.1 and click OK. In the Available events list, select ValueChange.
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In the Action field, select Knowledgeware action and enter the following message action body.
let x(Point) for x inside parameter { if (x.GetAttributeReal("Z") < 0.02) x.SetAttributeReal("Z",0.02) } • Click OK when done. The Reaction feature is added to the Relations node.
7. Click the Reaction icon (
). The Reaction dialog box opens. • In the Source type field, select Selection and select the list in the specification tree for the Reaction to be applied when the list is modified. In the Select a source... dialog box, select List.1 and click OK. In the Available events list, select ValueChange.
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In the Action field, select Knowledgeware action and enter the following message action body. let i = 1 let x(Point) for i while i<=parameter.Size() { x = parameter.GetItem(i) if (x.GetAttributeReal("Y") < 0.04)
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x.SetAttributeReal("Y",0.04) } • Click OK when done. The Reaction feature is added to the Relations node.
8. Create a new point with the following coordinates: X: 36mm Y: 12mm Z: 0mm 9. Update the Part twice: The Y and Z coordinates are set to 40 and 20 mm. Click here to display the result sample. To find out more about the Reaction feature window, see Using the Reaction Feature Window.
Launching a VB Macro with Arguments
The task below illustrates how to add arguments to a macro. Macros with arguments are features that can be: • • • stored in CATPart or CATProduct documents, stored in catalogs. Double-click them in the catalog to run them, called from a rule (VBScriptRun) or a reaction. In this case, arguments are passed from the rule.
icon enables you to access the macro editor. In addition to the usual The 'edit and run' capabilities, this editor allows you to: • specify arguments • carry forward a feature definition to the editor just by selecting the feature either in the tree or in the geometry area.
Note that the VB macro with arguments functionality is intended to help you write macros. It is not intended to find the code of other objects: Only the
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objects that were correctly integrated to the macros are supported. 1. Click the icon. The script editor is displayed.
2. Copy/paste the script below into the editor:
Dim oActiveDoc As Document Set oActiveDoc = CATIA.ActiveDocument
If (InStr(oActiveDoc.Name,".CATPart")) <> 0 Then
Dim oParams As Parameters Set oParams = oActiveDoc.Part.Parameters
Dim strParam1 As StrParam Set strParam1 = oParams.CreateString("FirstName", "")
Dim strParam2 As StrParam Set strParam2 = oParams.CreateString("LastName", "")
strParam1.Value = fname strParam2.value = lname
Else MsgBox "The active document must be a CATPart" End If
End Sub
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3. Enter the fname and lname arguments in the field located between the parentheses. The arguments must always be separated by a comma. 4. Click OK to add the macro to the document. A 'VB Scripts' sub-node is added to the specification tree below the Relations node. A VB Script object is added below this sub node. 5. Double-click the VB Script object. The Script Editor is displayed. The Insert Object Resolution button allows you to retrieve a feature definition. The VB Script.2 macro of the KwrObject.CATPart sample illustrates how to use this capability. 6. Click Run script.... The Select Inputs for Script Arguments is displayed. 7. If need be, select fname in the argument list, then enter a string into the value field (no quotation marks). Then select lname and enter the lname value. 8. Click OK to run the script. The two string type parameters are added to the document. Their values are those you have just specified. Note that the VB script features with arguments are provided with a contextual menu enabling the user to launch the script.
Working with Relations
Working with Relations
Relations located at a product level are not integrated to the product update process. If your relation drives parameters located at a Part level, create the relation at the Part level.
Select the Add Set of Relations icon to regroup relations into categories. Select the Measure Update icon to perform the update of relations using measures. Creating Sets of Relations Using Relations based on Publications at the Product Level Activating and Deactivating a Component Instantiating Relations from a Catalog Updating Relations Using Measures Controlling Relations Update
Creating Sets of Relations
This task explains how to create sets of relations below the Relations node of the specification tree.
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Using this capability enables you to regroup relations into categories. When you create a relation, you are prompted to enter a destination. i.e. a feature you add the new relation to. Formulas, design tables, rules and checks can all be created into relation sets. When no relation set has been created, the destination field of the relation editor is by default initialized to the Relations node. 1. Create a Part and from the Start->Knowledgeware menu, access the Knowledge Advisor workbench. icon and click the Relations node, the Relations.1 (or 2. Click the Relations.n) relation set is added to the specification tree right below the Relations node. 3. Click the Rule or the Check creation icon. The first dialog box displayed is similar to the one displayed when you create a relation right below the Relations node except that you must specify a destination. To do so, select the value specified in the Destination field of the relation editor, then select the Relation Set you want to add a relation to. This results in a modification of the destination path in the relation editor (partname partname Relations.n is replaced with Relations Relations.n).
4. Click OK to display the next dialog box and enter the relation body. 5. After you have finished specifying the new relation, click OK in the editor dialog box. In the specification tree, you can expand the feature which represents the relation set. A new relation has been added below this relation set.
Using Relations based on Publications at the Product Level
This scenario explains how to use relations based on publications at the product level. The scenario described below is divided into the following steps: • Add a parameter to the KwrScrew.CATPart called Screw_Volume, add a formula to calculate the volume of the screw and publish the Screw_Volume parameter. Add a parameter to the KwrScrew1.CATPart called Screw_Volume, add a formula to calculate the volume of the screw and publish the Screw_Volume parameter. Create a CATProduct file called Bolt and import the KwrScrew.CATPart Import KwrNut.CATPart. In the context of the Bolt product, create a formula calculating the bolt volume based
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• • •
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on the screw and the nut publications. • In the context of the bolt, replace KwrScrew.CATPart by KwrScrew1.CATPart. The volume is recomputed.
Before you start, make sure that the Keep link with selected object check box is checked (Tools->Options->Infrastructure->Part Infrastructure->General). Note that this function can be used with: • • • • • Design Tables Formulas Rules and Checks Set of Equations The optimization
1. Open the KwrNewScrew.CATPart document. The following image is displayed.
2. Add a Volume parameter to the part. Click the icon. The Formula Editor opens. In the New parameter of type scrolling list, select Real and click the New parameter of type button. In the Edit name or value of the current parameter field, enter the name of the parameter: Screw_Volume. Click Apply and click the Add Formula button. The Formula Editor opens. Enter the following formula by using the Dictionary:
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Screw_Volume=smartVolume(PartBody Pad.2 ). Click OK three times. 3. Publish the Screw_Volume parameter. To do so, select the Tools>Publication command and click the Screw_Volume parameter under the Parameters node in the specification tree. Click OK. The published parameter appears in the specifications tree below the Publication node. Save your file and close it.
Pad.1)+smartVolume(PartBody
4. Open the KwrNewScrew1.CATPart and repeat the steps listed above (steps 1 to 3 included). The part should be identical to the one below. Save your file and close it.
5. Create a CATProduct file named KwrBolt.CATProduct. 6. Click the Root product and select the Insert->Existing Component... command. The File selection box is displayed. Select the KwrNewScrew.CATPart file and click Open. The screw is
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imported. 7. Select the Insert->Existing Component... command, select the KwrNewnut.CATPart file and click Open. The nut part is inserted.
8. Add a Bolt_Volume parameter to the product to compute the volume of the bolt.
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icon. The Formula Editor opens. In the New param Click the Root product and click the of type scrolling list, select Real and click the New parameter of type button.
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In the Edit name or value of the current parameter field, enter the name of the paramet Bolt_Volume. Click Apply and click the Add Formula button. The Formula Editor opens.
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Enter the following formula by using the Dictionary and by clicking the published parameters i specification tree: Bolt_Volume=`..!screw.2!Screw_Volume` +`..!Nut!Nut_Volume` Click OK, and OK. The Bolt volume is displayed
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9. Replace the screw to compute a new volume: Double-click, then right-click the Screw.2 component in the specification tree and select the Components->Replace Component... command. The File Selection window opens. Select the KwrNewScrew1.CATPart file and click Open. 10. Click Yes and OK in the Impacts on Replace window. The new screw is inserted and the bolt volume is updated.
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Activating and Deactivating a Component
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This task explains how to activate and deactivate a component. In the scenario described below, the CATProduct file contains two CATPart files that you will activate and deactivate alternatively after creating user parameters and a rule based on these parameters. Note that: • • Relations located at the product level are not integrated to the product update. If your relation drives the parameters of a Part, create the relation at the Part level. Parameters driven by rules are designed to enable you to control components activities at assembly level.
When working in a Japanese environment, remember to check the Surrounded by the Symbol' option (Tools->Options->General->Parameters and Measure->Knowledge tab).
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1. Open the KwrSyringe.CATProduct file and save the following files in the same directory (SyringePiston.CATPart, HollowSyringePiston.CATPart, and SyringeContainer.CATPart): This file contains a syringe made up of three different parts: A barrel, and two different plungers. 2. Create a multiple value parameter of string type. • • Click the icon. The Formulas Editor opens.
Select String in the scrolling list with Multiple Values. Click the New Parameter of type button. The Value List dialog box opens. Enter two different values, Hollow and Full, and click OK. Edit the name of the new parameter (SyringeType in this scenario) in the Edit Name or value of the current parameter and click OK. The new parameter is displayed under the Parameters node of the Specification tree.
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3. Access the Knowledge Advisor workbench and click the Rule icon to create a rule. The script of this rule will allow you to enable or disable one of the plungers. 4. Enter the code below in the Rule Editor, and click OK. if (SyringeType == "Hollow") { `S3\Component Activation State` `S2\Component Activation State` } else { `S2\Component Activation State` `S3\Component Activation State` }
= false = true
= false = true
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Note that Japanese users should enter the following rule.
6. Double-click the SyringeType parameter under the Parameters node and select Hollow in the Edit Parameter window. The SyringeBarrel CATPart and the HollowSyringePlunger CATPart are displayed.
7. Double-click the SyringeType parameter and select "Full" in the Edit Parameter window. The SyringeBarrel CATPart and the SyringePlunger
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CATPart are displayed.
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Instantiating Relations from a Catalog
The scenario developed below explains how to instantiate a check stored in a catalog into a CATPart document. Formulas, rules and checks can be stored in a catalog. They can then be reused in a document by using an instantiation mechanism. For more information about catalogs, see the Infrastructure User's Guide. 1. Open the Formula_005_Start.CATPart file. 2. In the Tools toolbar, click the icon. The catalog browser is displayed.
3. Click the icon to open the CatalogFormula.catalog catalog. The catalog browser looks something like the one below (you may need to expand the Knowledge node to display the three relations Formula.1, Check.1, Check.2 what you see in the left-hand part of the Catalog Browser depends on the last interactions you have carried out with this dialog box).
4. Double-click the Check.1 object. The dialog box below is displayed.
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5. Rename the Check.1 check by using the Name field. Enter HeightCheck for example. 6. The 'Hauteur' input is highlighted. In the part specification tree, select the "Hauteur" parameter. The Rayon input is now highlighted. In the specification tree, select the "Rayon" parameter. Click OK and Close. The HeightCheck is added to the specification tree and, depending on the values assigned to the Height (Hauteur) and Radius (Rayon) parameters, a message can be displayed. 7. Double-click the HeightCheck relation twice in the specification tree. The relation below is displayed in the check editor: Hauteur >= Rayon. The relations of a catalog must be instantiated one-by-one in a document.
Updating Relations Using Measures
This task explains how to update relations using measures. A relation using measures is to be updated when the opposite the relation in the specification tree. Example MeasureRule requires an update symbol is displayed
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MeasureRule does not need to be updated
To update the rules: • Click the icon. To do this you must be in the Knowledge Advisor workbench. -or• Select the Measure Update command from the Relations node contextual menu. You can do this in any workbench.
All the document relations are then updated.
Controlling Relations Update
This topic provides you with 2 short examples showing you how to work with relations in Synchronous and in Update relation at global update command modes. • • In the first example, you update a formula. In the second example, you update an equation.
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For a given relation, it is possible to determine that it only executes in Synchronous mode using the Edit->Properties command. Its evaluation can then be launched manually. The Synchronous mode enables you to create synchronous relations, that is to say relations that will be immediately updated if one of their parameters is modified. Relations based on parameters are the only ones that can be synchronous.
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For a given relation, it is also possible to decide that its evaluation will be launched when the part is updated (Update relation at global update command). The relations can be asynchronous for 2 reasons: o You want the relation to be asynchronous o The relation contains geometry.
It is possible to change the update mode of a relation after it is created. • Right-click the relation in the specification tree and select the
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•
Properties command. Check the Synchronous or the Update relation at global update command check box.
To know more about the Synchronous or the Update relation at global update command options, see the description of the Knowledge tab in the Infrastructure User's Guide.
Updating a Formula
In this example, the document contains 2 parameters of Length type: • Length.1 is valuated by you. Length.2 is valuated by a formula computing the distance between 2 points + Length.1.
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1. Open the KwrUpdatingaFormula.CATPart file. The following image is displayed.
2. Expand the Relations node (if need be), right-click Formula.1 and select the Properties command. 3. In the Properties window, uncheck the Update relation at global update command check box. Click OK to validate.
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4. Double-click Length.1. The Edit parameter window is displayed. Enter 50 in the value field. Click OK to validate. The value of Length.2 is updated automatically and an update icon is displayed indicating that it will also be updated at the global update. 5. Right-click Formula.1 and select the Properties command. 6. In the Properties window, uncheck the Synchronous check box and check the Update relation at global update command check box. Click OK to validate. 7. Double-click Point.2 in the specification tree or in the geometry. 8. Enter the following values in the Point Definition window and click OK when done:
The Formula is not updated and an update icon is displayed next to the formula. 9. Right-click Formula.1 and select the Local Update command. The formula and Length.2 are updated.
Updating an Equation
In this example, you change 3 parameters, a, b and c before solving the equation. If you use the Synchronous mode, an error is displayed when modifying the parameters values since the update is launched at each modification. To ensure the stability of the equation, the update must be launched after the 3 parameters are changed. Thus you need to select the Update relation at global update command mode. 1. Open the KwrUpdatinganEquation.CATPart file. The following image is displayed: This document contains 4 parameters. x is a parameter valuated by an equation based on the other 3 parameters (a, b, and c).
2. Expand the Relations node (if need be), right-click Equations.2 and select the Properties command. 3. In the Properties window, check the Synchronous check box and uncheck the Update relation at global update command check box. Click OK to validate. 175 4. Double-click a in the specification tree. The Edit Parameter window is displayed. Enter 2 in the value field. A message is displayed indicating that the equation cannot be solved and click OK.
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Working with the List Feature
Working with the List Feature
Select the List icon to create a list of features that will be located under the Parameters node in the specification tree. Clicking this icon opens the List edition window.
List features can be used to manage lists of objects or parameters. These lists can be edited interactively. The List edition window enables you to sort items automatically and to specify the type of objects authorized. The list feature is integrated in the update mechanism, the size of the list is computed automatically (it is provided with functions designed to compute sums, areas, costs...). The list feature can be manipulated through the language to: • Create list • • • • • Copy the content of a list into another one Add and remove elements Get an element Retrieve values from the list Move elements of the list to another position
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Using the List Edition Window
The List Edition window enables you to manage the objects you want to add to the list you are creating. It can be accessed by clicking the List icon ( ).
The window contains four different buttons and is made up of 2 columns. Name Column indicating the name of the list. Enables you to add the items you selected in the specification tree or in the geometry to the list. Enables you to remove items from the list. Enables you to move up items in the list. Enables the user to move down items in the list. The Number of Elements field displays the number of items contained in the list. Value/<Type> Column indicating the value of the list or the associated type.
There are 4 different types of lists: • Not seen lists: These lists are created by CAA users and cannot therefore be modified interactively by the user (they are not displayed). In this case, the buttons of the List dialog box do not display. Read only lists: These lists are created by CAA users and cannot therefore be modified interactively by the user (they are in read only mode). Read/Write lists: These lists are created by CAA users, can be edited by the end user but they cannot be deleted.
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User lists: These lists can be edited and deleted by the end user.
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Like for any other parameter, it is now possible to hide and reorder lists. To do so, rightclick the list and select the Hide or Reorder... commands. When clicking the List icon to create a list, the MultiSelection window now is displayed. To find out more about this window, see the Infrastructure User's Guide. If you select an item in the List, and click another item in the specification tree or in the geometry, and click Add, the List item will be replaced with the one you have just added.
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Creating a List
This task explains how to use the List Feature. In the scenario described below, you are going to manipulate a plane wing to which you will add planes and intersections. You will then create parameters and formulas to calculate the surface of the intersections and will create a list that will compute the total area of the intersect sections. To find out more about the List Edition window, see Using the List Edition Window. To find out more about the List Feature, see Working with the List Feature. 1. Open the KwrPlaneWing.CATPart file. 2. Access the Generative Shape Design workbench. 3. Create three planes. • Click the Plane icon in the tool bar.
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a) The Plane Definition dialog box opens. b) In the Plane type area, enter the yz plane (select it in the geometry or in the specification tree): The yz plane is displayed in the Reference area. c) Indicate the required offset in the Offset field (-50mm for example). Click OK. d) Repeat this operation twice with offsets of -100 and -150mm. (Click the graphic to enlarge it)
4. Add formulas to calculate the intersection surface of the planes with the blend. • • Click the icon. The Formulas Editor opens.
Select Area in the scrolling list and click the New parameter of type button. Change the name of the parameter to Area_Intersect1 and click the Add Formula button. The Formula editor opens. In the Dictionary, select Measures, double-click area(Surface, ...):Area. Position the cursor between the parentheses, select Wireframe constructors in the Dictionary, and double-click intersect(Surface,Surface):Curve. Position the cursor before the coma and select Plane.2 in the specification tree (or in the geometry) then select Blend.1 in the specification tree. Click OK.
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Repeat the above steps for Area_Intersect2 and Area_Intersect3 by selecting Plane.3 and Plane.4.
(Click the graphic to enlarge it)
5. Access the Knowledge Advisor workbench, and click the List icon ( window opens. 6. Select the 3 parameters located under the Parameters node in the specification tree, and click the Add button. Click OK. Rename List.1 to Intersections for example. (Click the graphic to enlarge it)
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7. Click OK. The list is added to the parameters. 8. Add a formula that will compute the area of the 3 planes intersections with the blend. Click the icon. Select Area in the scrolling list, click the New parameter of type button, rename the parameter to Total_Intersection_Areas and click the Add formula button. The Formula editor opens.
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Click the List (Intersections in this scenario) in the specification tree: the name of the list is displayed in the editor. Under Dictionary, select List, and double-click List.Sum(): Real in the Members of List area. Click OK twice.
The area of the 3 planes intersections with the blend is automatically calculated.
(Click the graphic to enlarge it) 9. Edit the list content and re-compute the total area. o Double-click the list (Intersections) in the specification tree: the List edition window opens. Select Area_Intersect3, click the Remove button, and click OK. Right-click the Total_Intersection_Areas parameter and select Local Update. The area of the remaining 2 planes intersections with the blend is automatically calculated. (Click the graphic to enlarge it) Click here to display the result of this scenario.
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Working with the Loop Feature
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Working with the Loop Feature
Select the Loop icon to create a loop. Introducing the Loop Feature Getting Familiar with the Loop Edition Window Creating a Loop Creating a Power Copy containing a Loop Using the Scripting Language Reference
Introducing the Loop Feature
Note that a KWA license is required to execute loops. Loops use the Generative Knowledge language to drive the creation, modification and deletion of a set of features. This functionality enables you to: • • • Select inputs in the definition of the loop Define several contexts in the loop action Include the loop into a Power Copy
It can be accessed by clicking the Loop icon ( • •
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A loop is stored in the resulting model as a feature on its own. A change in its specification will drive the expected modification in the model. A loop can be instantiated through a Power Copy implying a significant simplification of use and re-use.
Getting Familiar with the Loop Edition Window and Menus
• • • The Loop Edition Window The Loop Tools Menu The Loop Contextual Menu
The Loop Edition Window
The Loop Edition window is displayed when you click the Loop icon ( Control Features tool bar. ) in the
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Input(s)
This field enables you to select the features that you want to use in the specification tree or in the geometry. The selected features are those that will be used in the loop body. To deselect items from the Inputs list, click them in the specification tree or in the geometry. The Input Name field enables you to rename the inputs that you selected. In this case, this name will be used in the loop body.
Context
This field enables you to define the application context of the loop. It can be any V5 feature. To select the context, click the Context field once, then click the item in the specification tree.
Iterators
The From ... To fields enable you to define the number of times that the loop will operate. When defining the ranges, you can right-click the From... and the To fields to access the contextual menu. • The Edit formula... command enables you to access the Formulas editor and to create a formula that will apply to the loop operation. To know more, see Creating a Formula. The Add Multiple Values... command enables you to add multiples value. To know more, see Switching between Simple and Multiple Values After Creating a Parameter. The Add Range... command enables you to add a range.
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The Edit Comment... command enables you to add a comment. The Lock... command enables you to lock this parameter. To know more, see Locking and Unlocking a Parameter .
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Note that: • • The step is one in the From... To fields. Both bounds are included when the loop runs.
Editor
The Editor enables you to enter the loop syntax. The language to use in this editor is the scripting language. To find out more about the syntax to be used, see Using the Scripting Language.
The Tools menu
The Tools->Object Browser ... command enables you to access the Object Browser. This browser contains the types and attributes that are part of the scripting syntax. The object browser guides you when writing a script. It allows you to access the keywords, operators and feature attributes that can be used when working with the loop features. The packages displayed in the left part of the browser are those you selected from the Tools->Options... command. To add or remove packages: 1. Select the Tools->Options... command to open the Options window, then select General->Parameters and Measure, and click the Language tab. 2. In the Language field of the Knowledge tab, check Load extended language libraries and select the libraries.
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From this window, you can manipulate the list o objects supported by the script using their attributes... • The left part of the browser displays the available packages.
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The central part displays the list of object belonging to this category.
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The right part displays the attributes allowing you to manipulate these objects any).
... and write loop bodies (see example below): Circle0 isa GSMCircle { CircleType = 0; TypeObject isa GSMCircleCtrRad { Center = object: .. .. .. Construction_Body Support = object:
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.. Construction_Body Radius = 180mm; } StartAngle = -100deg; EndAngle = 100deg; }
Extrude
The Back icon. To return to your last interaction in the wizard. Has no action on the script editor. The Forward icon. To go forward to your next interaction in the wizard when moving through a series of interactions. The Attribute Type icon. This icon is not available in the current version of the product. The Inheritance icon. To return to the root object. The Insert icon. To insert the object name in the script.
The Loop Contextual menu
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knowledgewareAdvisor You can access the Loop contextual menu by right-clicking the loop in the specification tree. • The Definition... command enables you to access the Loop Edition window. The Deactivate... command enables you to deactivate the loop. In this case an icon indicates that the loop is disabled. To enable it, right-click it and select the Loop activate... command. The Hide command enables you to hide the loop. In this case, it will not be displayed in the specification tree. The Reorder... command enables you to reorder the loops.
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Creating a Loop
The task below illustrates how to interactively apply a loop to an existing document.
The KwrLoop1.CATPart is made up of a surface (2) and a solid (1) that symbolizes a hole. This hole is inserted into a User Feature (UDF) for a later instantiation. The User Feature (UDF) has 3 different inputs (a point, an axis and a surface). 2 parameters of the User Feature (UDF) are published (3). • • Clearance=4mm Diameter=8mm
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The KwrLoop2.CATPart is made up of a surface (1) and of 12 points (3) inserted into a list. The Line.7 is the instantiation axis (2).
The aim of this scenario is to instantiate as many holes as existing points. It is divided into the following steps: • You create a loop. • • You instantiate the User Feature (UDF) from the existing .CATPart file. You valuate the required inputs to instantiate the holes.
To create a loop, you have to: 1. Declare input data 2. Define the context 3. Specify iterators 4. Write the body of the action script Before creating a loop in a CATPart document, make sure that the Manual input option is unchecked in the Part Number field of the Tools->Options...>Infrastructure->Product Structure->Product Structure tab. To perform this scenario, you will need the following files: • • KwrLoop1.CATPart KwrLoop2.CATPart
1. Open the KwrLoop2.CATPart
Creating a Loop
2. From the Start->Knowledgeware menu, access the Knowledge Advisor
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workbench. 3. Click the Loop icon ( window is displayed. ) in the Control Features bar. The Loop Edition
4. In the specification tree, select the inputs of the loop. o Expand the Parameters node and select the List_Extract list. In the Input name field, enter the name of the list: PointsList. Expand the Surface node and select the Revolute.1 feature. In the Input name field, enter the name of the list: SurfRef. Expand the Result_Body node and select the Line.9 feature. In the Input name field, enter the name of the list: LineAxis. Note that the name indicated in the Input name field is the one that will be used in the loop body. 5. Select the context, that is to say, in this scenario, the feature that will contain the instantiated holes. o o Click the Context field. Click Result_PartBody in the specification tree.
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6. Indicate the number of holes that you want to instantiate into the surface. o o In the From field, indicate 1. Right-click the To... field and select the Edit formula... command. The Formula Editor is displayed. In the specification tree, click ListSize=12. Click OK when done. The number of instantiated holes is now valuated by a formula based on the list, that is to say on the number of points contained in the list.
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7. Enter the following action script into the Editor. o Use the import keyword to indicate the path of the file containing the User Feature (UDF) to be instantiated. To indicate the path of the file, it is recommended to use the Insert File Path command available in the contextual
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menu to import KwrLoop1.CATPart. (1) o o UDF_$i$ is the name that will be attributed to each instance of the hole. At each iteration, $i$ is replaced with the current iterator. (2)
8. • • • Clearance_Hole_UDF is the name assigned to the User Feature (UDF) in the KwrLoop1.CATPart file. (2)
Position is a point and is also the first input that needs to be valuated when instantiating the holes. PointsList is the name of the List. (3) Clearance_Surface is the second input required and defined when creating the User Feature (UDF) and SurfRef is the revolute into which the holes will be instantiated. (3) Axis is the third input required and defined when creating the User Feature (UDF) and LineAxis is Line.9, that is to say the instantiation axis. (3)
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To find out more about the syntax to be used (;, {}, $i$) in the loop body, see Using the Scripting Language. Click OK when done. The 12 holes are instantiated. (See picture below.)
Creating a Power Copy Containing a Loop
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This task illustrates how to interactively apply a loop to an existing document. In this scenario, you are going to make holes in a pad. To do so, you are going to: • • • Create a loop referencing the inputs of an existing User Feature (UDF) used to make holes in a pad. Save the loop in a Power Copy. Instantiate the Power Copy into an existing document and creates the holes.
To perform the scenario, you will need the following files: The KwrLoop1.CATPart is made up of a surface (2) and a solid (1) that symbolizes a hole. This hole is inserted into a User Feature (UDF) named Clearance_Hole_UDF for a later instantiation. The User Feature (UDF) has 3 different inputs (a point, an axis and a surface). 2 parameters of the User Feature (UDF) are published (3): • • Clearance=4mm Diameter=8mm
The KwrLoop3.CATPart file is made up of a pad and a surface and of 24 points (1) inserted into a list. Line.2 is the instantiation axis (2). This .CATPart file is the one that will contain the loop contained in the Power Copy that will be instantiated into KwrLoop4.CATPart.
The KwrLoop4.CATPart is made up of a pad and a surface (3) and of 17 points (2) inserted into a list. Line.1 is the instantiation axis (1). It will contain the instantiated loop and the holes.
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Before creating a loop in a CATPart document, make sure that the Manual input option is unchecked in the Part Number field of the Tools->Options...>Infrastructure->Product Structure->Product Structure tab. To create a loop, you have to: 1. Declare input data 2. Define the context 3. Specify iterators 4. Write the body of the action script Creating the loop referencing the user feature (UDF) 1. Open the KwrLoop3.CATPart. The following image is displayed.
2. From the Start->Knowledgeware menu, access the Knowledge Advisor workbench. 3. Click the Loop icon ( is displayed. ) in the Control Features bar. The Loop Edition window
4. In the specification tree, select the inputs of the loop. o Expand the Parameters node and click the Lists_PointRef list. In the Input Name field, enter the name of the list: PointsList. Expand the Geometrical Set.1 node and select the Clearance_Surface feature. In the Input name field, enter the name of the feature: SurfRef. Expand the Holes_Points node and select the Line.2 feature. In the Input name field, enter the name of the line: LineAxis. Note that the name indicated in the Input name field is the one that will be used in the loop body. 5. Select the context, that is to say, in this scenario, the feature that will contain the instantiated holes.
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Click the Context field. Click ResultBody in the specification tree.
6. Indicate the number of holes that you want to instantiate into the surface. o o In the From field, indicate 1. (1 corresponds to Extract.1.) Right-click the To... field and select the Edit formula... command. The Formula Editor is displayed. In the specification tree, click ListSize=24. Click OK when done. The number of instantiated holes is now valuated by a formula based on the list, that is to say on the number of points contained in the list.
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7. Enter the following action script into the Editor. o Use the import keyword to indicate the path of the file containing the User Feature (UDF) to be instantiated (KwrLoop1.CATPart) . To indicate the path of the file, it is recommended to use the Insert File Path command available in the contextual menu to import KwrLoop1.CATPart. (1) UDF_$i$ is the name that will be attributed to each instance of the hole. (2) Clearance_Hole_UDF is the name assigned to the User Feature (UDF) in the KwrLoop1.CATPart file. (2)
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when instantiating the holes. PointsList[$i$] is the name of the List. [$i$] corresponds to the nth item of the list. In this case, nth is equal to 24, the number of holes to be instantiated (3). o Clearance_Surface is the second input required and defined when creating the User Feature (UDF) and SurfRef is the revolute into which the holes will be instantiated. (4) Axis is the third input required and defined when creating the User Feature (UDF) and LineAxis is Line.9, that is to say the instantiation axis. (5) Clearance is one of the published parameters of the User Feature (UDF). It is used in the action script because you want the value of the published parameter to be modified. (6)
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To find out more about the syntax to be used (;, {}, $i$) in the loop body, see Using the Scripting Language. 8. Click OK when done. The holes are instantiated (see graphic below.) 9. Click the Update icon ( ) to update the document.
10. Right-click the loop and use the Properties command to rename the loop into Loop_Holes. Click OK when done. 11. In the specification tree, right-click the loop (located below the Relations node) and select the Loop_Holes object->Deactivate command. Saving the loop in a Power Copy 12. Click the root of the specification tree, and from the Start->Mechanical Design menu, access the Part Design workbench. 13. From the Insert->Advanced Replication Tools menu, select the PowerCopy Creation... command. The Power Copy Definition window is displayed. 14. In the specification tree, select the items making up the Power Copy: o o Formula.1 Loop_Holes
Note that the Power Copy will need the following inputs at instantiation time: o o o o o ListSize Line.2 Clearance_Surface List_PointsRef ResultBody
15. Click OK when done. The Power Copy is created and is displayed below the 193 Power Copy node in the specification tree. 16. Save your file and close it.
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Using the Scripting Language
Using the Scripting Language
Introducing the Scripting Language The Scripting Language is a declarative way of generating V5 Features. It allows you to: • Describe objects using a very simple script language. • Use 3D geometric features (sketches, parts, ...). • Use parameters on features including formulas. • Use related positioning & orientation constraints. • Generate the corresponding V5 models (features, documents, User Features,...) Enter the body of their loops in the Loop Edition window in Knowledge Advisor.
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Action Script Structure Object Properties Operators Keywords Variables Comments Limitations Using the Get... Commands
Action Script Structure
An action script is written in text format and is organized in blocks consisting of related sets of statements. A block consists in an instruction designed to create an object followed by a set of statements surrounded by braces ({ }). Statement blocks can be nested and the most enclosing one within a script corresponds to the document creation. A document is made up of a hierarchy containing objects, their properties and the features they own. An action script reflects this object hierarchy.
Example
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In the script opposite, the inputs and the published parameters (2) of the instantiated UDF "Hole_UDF" (1) are nested between braces {}.
Object Properties
• • • An object is created by default with some property values. These properties are defined or re-defined within the braces just following the object declaration (isa keyword). Unless otherwise specified, the units are IS units. When defining properties, the semicolon ; is a terminator (see example below). The properties might be object attributes (1), attributes needed to define a type displayed in the Object browser (2) or aggregated objects (3).
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In the script above, the properties are the inputs of an instantiated UDF.
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In the script above, the properties are the attributes required to create a point to point line.
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In the script above, the Pad object is aggregated below the OpenBodyFeature object.
Keywords
• • • • • isa keyword context keyword from keyword import Keyword publish keyword
isa Keyword
Definition
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knowledgewareAdvisor Enables you to create a typed object or instantiate an object. Syntax • or • where: • • • ObjectName is the name of the object to be created. ObjectType is the type of the object to be created. InstanceName is the name of the object to be instantiated. ObjectName isa InstanceName ObjectName isa ObjectType
Example import "E: GPS.CATPart"; myGps isa CATPart { myPart isa Part { PartB isa BodyFeature { S0 isa Sketch.0 {} //Instance name pad0 isa Pad("S0") //Object type } } }
context Keyword
Definition Enables you to define in which part of the specification tree the object will be created. The context keyword may be of use in 2 different cases: • It can indicate a context "Mypart.CATPart" document to be used. In MyPart isa Part { } this case, the "..." are used.
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It can reference an object contained in the document. In this case the path needs to be specified (between `...`).
context `My.CATPart CC isa Cylinder { }
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PartBody`
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or • context `My.CATPart MyPart PartBody`
from Keyword
Definition Allows you to copy a document from an existing document without maintaining any link. Syntax DocumentName isa DocumentType from FilePath where: DocumentType is either CATProduct, CATPart or model. FilePath is the full path of the initial document. To enter a file path you can: Use the Insert File Path command from the contextual menu Example See Defining the Context
import Keyword
Definition Specifies a document file (.CATPart or .CATProduct) containing definitions to be reused or redefined in the document to be generated. All the features and feature values in the imported file become available to the document to be generated. Importing a document is: • Of interest whenever you want to retrieve a consistent set of definitions from an already existing document (for a UDF definition for example.) • Required whenever you need to create a feature from a sketch (the script language does not allow you to specify a sketch).
Syntax There are 2 ways to specify the file path:
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knowledgewareAdvisor • import "File path"; : Indicate the path of the file to be imported: import "E: users kwecx Models PartImport.CATPart" ;. Note that you should enclose the path within quotation marks and end the import statement with a semicolon (;). import "File Name"; : Indicate only the name of the file to be imported if this file is located in the same directory as the document containing the loop: import "PartImport.CATPart";. Note that: You should enclose the document name within quotation marks and end the import statement with a semicolon (;). The file to be imported should be located in the same directory as the document containing the loop. The document containing the loop should be saved.
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publish Keyword
Definition Enables you to assign an object a name that will be used in the script. Syntax publish "!xxx" as yyy ; Where: • xxx is the name of the object to be published. To select this object, it is highly recommended to use the contextual menu.
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Example Publi isa CATProduct { Publi isa Product { P isa Product { P1 isa Part { PartBody isa Feature { Pa isa Pad{} } } publish "Publi/P/!Selection_RSur:(Face:(Brp:(Pa;2);None:());Pa)" as mypadface; /*publishes the face of a pad under the name "mypadface"*/ } Q isa Product { Q1 isa Part { PartBody isa Feature { Cy isa Cylinder{} } } publish "Publi/Q/!Selection_RSur:(Face:(Brp:(Cy;2);None:());Cy)" as mycylinderface; //publishes the face of a cylinder under the name "mycylinderface" } assembly constraints: contact("P } } toto","Q tutu");
Variables
Variables are declared explicitly in your script. These variables are displayed as parameters in the specification tree.
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ALPHA = 45 deg;
Unlike in most script languages, a variable scope is not really determined by where you declare it. From anywhere in your action script, you can access a variable by using the .. .. and ? operators. After the script is finished running, the variable declared in your script still exists as a document parameter.
Operators
Arithmetic operators
+ Addition operator (also concatenates strings) - Subtraction operator * Multiplication operator / Division operator ( ) Parentheses (used to group operands in expressions) = Assignment operator
? (Question Mark in Formulas)
Definition In a formula, specifies that the parameter value to be applied is the first parameter value found when scanning the specification tree from the formula to the top of the specification tree. Sample KwrLoopRelativePath.CATPart
(Relative Path in Formulas)
Definition Defines where the value of a parameter used as an argument in a formula is to be read. A single.. exits the statement block where the formula is defined. The
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User Tasks parameter value applied in the formula is then the one defined in the parent feature scope. Sample KwrLoopRelativePath.CATPart
Using The Get... Commands
The commands described in this section are the ones you can access when using the Loop Editor and right-clicking in the Editor window. When creating a loop containing the path of a feature contained in the specification tree, it is highly recommended to use the Get Feature command to retrieve the internal name of this feature. • • • • • Using Using Using Using the the the the Get Get Get Get Axis Command Edge Command Surface Command Feature Command
Using the Insert File Path Command
The 'Get Axis' Command
This task explains how to create a chamfer by using the Get Axis command. This command enables you to interactively capture the generic name of an axis and to insert it into the script instead of keying it in. 1. Click the Loop icon ( ) and enter 1 in the To field.
2. In the Script Editor, enter the following script and click OK. A pad is created. myChamferDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad { } } } }
3. From the Window menu, select Cascade. 4. Under the P isa Pad block, add F isa Chamfer(){}, position the
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cursor between the parenthesis, then right-click to open the contextual menu and select the Get Axis command, and select an edge in your geometrical surface. The script should be as follows: myChamferDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad { } F isa Chamfer("Edge:(Face:(Brp:(P;0:(Brp:(Sketch.1;2))); None:());Face:(Brp:(P;0:(Brp:(Sketch.1;3)));None:()); None:(Limits1:();Limits2:()))"){} } } } 5. Click the OK button. The chamfer is created.
The "Get Edge" Command
This task explains how to create a chamfer by using the Get Edge command. This command enables you to interactively capture the generic name of an edge and to insert it into the script instead of keying it in. 1. Click the Loop icon ( ) and enter 1 in the To field.
2. In the Script Editor, enter the following script and click OK. A pad is created. myChamferDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad { } } } }
3. Under the P isa Pad block, add F isa Chamfer(){}, position the cursor between the parenthesis, then right-click to open the contextual
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menu and select the Get Edge command, and select an edge in your geometrical surface. The script should be as follows: myChamferDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad {} F isa Chamfer("Edge:(Face:(Brp:(P;0:(Brp:(Sketch.1;2))); None:());Face:(Brp:(P;2);None:());None:(Limits1:();Limits2:()))"){} } } } 4. Click the Generate button. The chamfer is created.
The "Get Surface" Command
This task explains how to create a sketch on an existing face by using The Get Surface command. This command enables you to interactively capture the generic name of a surface and to insert it into the script instead of keying it in. 1. Open the KwrGetSurface.CATPart file. 2. Access the Knowledge Advisor workbench, and click the Loop icon. Enter 1 in the To field 3. Enter the following script: import "f: cube.CATPart"; myFaceDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad{} S isa Sketch.1() 4. Position the cursor between the two parentheses of the last line of the above script, right-click to open the contextual menu and select the Get Surface command. 5. Select the face whose name you want to capture. The full name is inserted at the cursor location. Enter the end of your script. In our example, the final script is as follows: import "f: PktGetSurface.CATPart";
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myFaceDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { P isa Pad{} S isa Sketch.1("Face:(Brp:(P;0:(Brp:(Sketch.1;2)));None:())") { } } } } 6.
The "Get Feature" Command
This task explains how to use the Get Feature command. This command enables you to interactively capture the generic name of a surface and to insert it into the script instead of keying it in. In the task below, you are going to generate a line. 1. Open the KwrGetFeature.CATPart file. 2. Double-click the loop located below the Relations node and insert the following code into the editor: Line_Pt_Pt isa GSMLine { LineType = 0; TypeObject isa GSMLinePtPt { FirstPoint = object: // Using GetFeature to Select the FirstPoint (Point.10) SecondPoint = object: // Using GetFeature to Select the SecondPoint (Point.7) } } 3. 4. Position the cursor after FirstPoint = object: and select the Get Feature command in the contextual menu. 5. Click a point in the geometry (Point.10 for example) and add a semi-colon (;) at the end of the line. 6. Position the cursor after SecondPoint = object: and select the Get Feature command in the contextual menu. 7. Click another point in the geometry (Point.7 for example) and add a
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semi-colon (;) at the end of the line. Your script should now look like the one below:
8. Click OK. A new line is generated. 9.
The 'Insert File Path' Command
This task explains how to use the Insert File Path command. This command is one of the methods you can use to specify a path in a script. When writing a script, you have to specify a file path when you import a file, see the import keyword. 1. Access the Script Editor and enter any instruction requiring a file path specification (import in the example below). 2. Position the cursor where the path is to be specified.
3. Right-click and select the Insert File Path command from the contextual menu.
4. In the dialog box which is displayed, select the appropriate file. Click Open to go back to the script editor. 5. The full path is inserted at the cursor place. Check that the statement is ended by a semi-colon.
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Comments
Multi-line comments (/* ... */) are supported. A single-line comment begins with a pair of forward slashes(//). Note that DBCS characters are not supported as comment.
Example
Sphere1 isa Sphere // Creates a sphere { // Valuates the Radius property Radius = 15.0 ; }
Limitations
You should be aware of some restrictions: • Instances of sketch-based features cannot be moved apart from their prototype. • Any parameter used as an argument in a formula should be preceded by the ? symbol. The syntax X = 2 * Y is invalid and should be replaced with X = 2 * ? Y. Unless a formula-defined parameter has not been initialized with the proper units, the value calculated from the formula is dimensionless. Y = 0 kg ; Y=2*?X; A script error stops the reading and the execution of the loop.
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Declaring Input Data
The Input Data are the data that will be used in the body of the loop and potentially be changed when instantiating the loop. To select them, click them in the specification tree or in the geometry.
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The Input Name field enables you to change the name of the input.
Note that the input can be a list made up of strings. It allows to instantiate features whose types are defined by the list items. To get an example see the following files: • • KwrPartUDFs.CATPart: This file contains the 4 UDFs definitions. KwrInstantiateUDFs.CATPart: This file contains the loop that instantiates the features. The inputs of the loop are made up of 2 lists. The first list contains parameters of String type (the names of the UDFs to be instantiated). The second list contains parameters of Length type (to valuate the UDFs published parameters: PosX).
Defining the Context
To create a loop, you need to define the context, that is to say the object (PartBody, Geometrical set, Pad, Relations, Parameters node or any feature) that will contain the items created by the loop. There are 3 different ways to define the context.
Using the Context field
To define the context of the loop, you may use the Context field of the Loop edition window. To do so, click the Context field, and select an object in the specification tree. In the picture opposite, a pad was selected in the specification tree.
Using an existing Document
It is possible to use an existing .CATPart or .CATProduct document.
Using the context keyword
When creating elements that need to be located in different bodies, you can change the context you defined in the Context field and use the Context keyword to define new contexts in the loop body.
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The action script should not start with the context keyword since the first context is defined in the Context field. Sample: KwrLoopMulticontext.CATPart (to launch the loop, activate the loop.)
Solving a Set of Equations
Solving a Set of Equations
This task explains how to solve a set of equations using the operators and functions of the knowledgeware language. This scenario can be run from any document. • • In a set of equations, the semi-colon (;) is used as a separator. Note that the equations set capabilities require the Knowledge Advisor product.
Note that a KWA license is required to execute loops.
1. Create two real type parameters x and y. Both parameters are intended to be used as variables in a se equations.
icon. In the first dialog box which is displaye 2. Access the Knowledge Advisor workbench. Click the enter the name of the relation, a comment and a destination. Then click OK. The Set Of Equations edi is displayed. 3. Enter the set of equations below into the edition box: y - 2 *sqrt(x) ==2; y - 4 *x*x == 0 Now, your editor looks something like this:
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The value of each parameter is display first in the Unknown parameters field, the in the specification tree (see below).
4. Click here to open the result file. To find out more about the Equations Editor, see Using the Equations Editor.
Using the Equations Editor
In order to improve the use of the Equations solving functions, the Equation Editor was modified. It is made up of two tabs: the Editors tab and the Options tab.
Editors tab
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The Parse arrow is used to identify the variables of the set of constraints. It must be pushed before choosing input and output variables. The left arrow is used to move variables from the Unknown parameters category to the Constant parameters one. The right arrow is used to move variables from the Constant parameters category to the Unknown parameters one. The Switch input/output arrow is used to swap the selected constant and unknown parameters. • • • • • Viewer: enables you to enter the equations that you want to solve. Dictionary: see Using the Rule Editor. Members of Parameters: see Using the Dictionary. Members of All: see Using the Rule Editor. Constant parameters: Constant parameters: The value of constant parameters are set by you and are considered as constants by the solver. This value can be changed directly in the Value column by clicking twice (slowly) in the Value cell. Unknown parameters: The value of unknown parameters will be calculated once the Apply button is pushed.
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Options tab
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Algorithm • Precision: enables you to define the precision of the results (i.e the number of decimal digits after the decimal point.) Use the Gauss method for linear equations: accelerates the solve operation when working with linear equations.
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Termination criteria • Maximal computation time (sec.): enables you to indicate the computation time. If the indicated time is equal to 0, the computation will last until a solution is found. Show 'Stop' dialog: if checked, displays a "Stop" dialog box that will enable you to interrupt the computation.
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Solving a Set of Equations
Using the Knowledge Advisor Language
Using the Knowledge Advisor Language
• Writing Formulas - Rules & Checks - Overview o o o Conditional Statements For Statement While Statement
• • • • • • •
Constants Comments Temporary Variables Units Operators Object Methods Messages and Macros
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Writing Formulas
A formula is a one-line statement that you can write either by typing directly the appropriate syntax in the editor field or by selecting items from the editor dictionary list. The formula syntax is easy to use and learn. The period is generally used as a separator between the whole numbers and the fractional part of a number. Using a comma as a separator in place of the period is not recommended in real values intended to be used directly in relations. Example: Real1 = 2,1 + 5,4 is not allowed whereas Real1 = Real2 + Real3 is allowed regardless of the separator used when valuating Real2 and Real3.
Writing Rules and Checks
Rules and checks are multi-line statements that you can write either by typing directly the appropriate syntax in the editor field or by selecting items from the editor dictionary list. Here is a description of the syntax to be used. The mathematical and trigonometric functions as well as the functions used to manipulate strings are the same as for formulas.
Conditional Statements
Rules
if ... else ... else if Conditionally executes a group of statements, depending on the value of an expression. You can use either block form syntaxes:
if condition statements [else elsestatements ] or
if condition { statements } [else if condition-n [ { elseifstatements } ] ] . . . [else [ { elsestatements } ] ]
You can use the single-line form (first syntax) for short, simple rules. However, the block form (second syntax) provides more structure and
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Checks
statement1 => statement2 (if statement1 then statement2) Displays a message (if type is Warning or Information) and turns to red in the specification tree each time statement2 is invalid as statement1 is fulfilled. OK => KO KO => KO KO => OK OK => OK
For Statement
Note that the For statement is available for Action and Reaction scripts only. The first type of loop is a loop based on the element of a list. See syntax opposite. Where: • • • X is a variable name (of a given type. It may represent an object or a value). List is a variable name of type List or an expression returning a list. X (like any other variable of the language) can be used in the body. It contains the Nth element of the list. For x inside List { Body }
The body is executed Nth times where N is the number of elements of the list. The second type of loop executes until an expression becomes false. See syntax opposite. Where: • • X is a variable name of integer type. It is incremented at the end of each execution of the body. Predicate is a Boolean expression. The body is executed as long as this expression is true. This For x while predicate { Body }
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expression is evaluated before the body. Note that the second for operator can lead to infinite loops.
While Statement
This loop executes until an expression becomes false. See syntax opposite. Where: • • i is a variable name of integer type. It is incremented at the end of each execution of the body. X is a variable for points. let i = 1 let x(Point) for i while i<=parameter.Size() { x = parameter.GetItem(i) if (x.GetAttributeReal("Y") < 0.04) x.SetAttributeReal("Y",0.04) }
Constants
The following constants are specified or recognized by CATIA when programming rules and checks. As a result, they can be used anywhere in a relation in place of the actual values. • • • false - one of the two values that a parameter of type Boolean can have true - one of the two values that a parameter of type Boolean can have PI - 3.14159265358979323846 - The ratio of the circumference of a circle to its diameter. E - The base of natural logarithm - The constant e is approximately 2.718282.
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Comments
The /* and */ comment characters are supported.
/* Rule created by CRE 05/03/99 */ if PartBody { Sketch.1 Radius.3 Radius > 45mm
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User Tasks LaunchMacroFromFile("Macro1.CATScript") } else /* LaunchMacroFromFile("Macro2.CATScript") */ Message("No macro launched")
Temporary Variables
Temporary variables can be declared by using the let keyword. A temporary variable does not persist as a parameter after the rule execution is finished.
/*Rule created by CRE 08/23/99*/ let x = 5 mm if PartBody { PartBody } For non digital values, the type has to be indicated: let S(Surface) S= split (...,...) Temporary variables should be declared at the beginning of the rule, before any conditional instruction is specified. let S1(Surface) let S2(Surface) let S3(Surface) S1 = Split ... S2 = ... S3 = ... Hole.1 Activity = false Hole.1 Diameter > x
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Units
Units are all provided in the dictionary. 1. Pay attention to unit consistency when writing a rule or a check. 2. Units are written with an underscore instead of the usual "/" (example N_m2 instead of N/m2).
Operators
Arithmetic operators
+ Addition operator (also concatenates strings) - Subtraction operator * Multiplication operator / Division operator ( ) Parentheses (used to group operands in expressions) = Assignment operator ** Exponentiation operator
Logical Operators
and Logical conjunction on two expressions or Logical disjunction on two expressions
Comparison Operators
<> Not equal to == Equal to >= Greater or equal to <= Less than or equal to < Less than > Greater than
Object Methods
Description
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Attributes
ID Name UserInfoComment Owner NamedURLs
Methods
• List.1 is the name of the list on which the calculation will be performed. PartBody is the body on which the search will be carried out Hole is the Type. x.Diameter>50mm is the expression.
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AbsoluteId Method GetAttributeInteger GetAttributeString ID Method IsOwnedBy Method IsSupporting Method Query Method SetAttributeBoolean SetAttributeString
AttributeType Method GetAttributeBoolean GetAttributeReal HasAttribute IsOwnedByString Method Name Method SetAttributeInteger SetAttributeReal
Example
1. Create a part with several holes. 2. Add a real type parameter ("Real.1" for example) to one of the hole features. To do this, you must use the Knowledge Advisor product. 3. Create the rule below: /* This rule resets the diameter of the hole */ /* which has "Real.1" as its parameter to the Real.1 value */ (for all) H:Hole if H->HasAttribute("Real.1")
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knowledgewareAdvisor H.Diameter = 1mm*(H->GetAttributeReal("Real.1")) You can use all the GetAttributexxx methods in that way. • • Add one or more drafts to the part. You can write the rule below: (for all) Dr:Draft /* Displays the names of the Drafts which have PartBody as their names */
See also: Using the Dictionary
Attributes
Id Defines the feature identifier, i.e. the name primarily assigned to the feature at creation before any renaming has been done. Owner Defines the parent feature. Name Defines the feature name. NamedURLs Describes the URL that the user can add to a relation by clicking the Comment and URLs icon in the Knowledge Advisor workbench. UserInfoComment Describes the comment that the user can add in the Comment and URLs dialog box when adding a URL to a relation in the Knowledge Advisor workbench.
Object Methods
AbsoluteId Method GetAttributeInteger Method HasAttribute Method IsOwnedByString Method SetAttributeBoolean
AttributeType Method GetAttributeReal Method Id Method IsSupporting SetAttributeReal Method
GetAttributeBoolean Method GetAttributeString Method IsOwnedBy Method Name Method SetAttributeInteger Method
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Method
SetAttributeReal Method
SetAttributeString Method
SetAttributeDimension
AbsoluteId Method
Retrieves the path of a feature. Note that this feature is not NLS (it will not be translated into your language and remains in english.)
Syntax
feature.AbsoluteId(): String
Example
String.2=PartBody
Sample
Pad.1.Id() + PartBody
Pad.1.AbsoluteId()
KwrTopology.CATPart
AttributeType Method
Returns the attribute type in the form of a string.
GetAttributeBoolean Method
Returns the value of a boolean type parameter added to a given feature by using the Knowledge Advisor product. parameterName is the name of the boolean type parameter. It should be put between quotation marks (").This method enables you to read: • • •
Syntax
The attributes added to parameters using the Parameters Explorer. The real attributes added to objects. The User Properties of a product.
feature.GetAttributeBoolean(String): Boolean where the argument is name of the attribute.
Example
Message ("The value of the Boolean.1 attribute of # is #", PartBody PartBody Pad.1.Name(), Pad.1.GetAttributeBoolean("Boolean.1"))
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Sample
KwrObject.CATPart
GetAttributeInteger Method
Returns the value of an integer type parameter added to a given feature by using the Knowledge Advisor product. parameterName is the name of the string type parameter. It should be put between quotation marks ("). This method enables you to read: • • •
Syntax
The attributes added to parameters using the Parameters Explorer. The real attributes added to objects. The User Properties of a product.
feature.GetAttributeInteger(String): Integer where String is name of the attribute. This name should be put between doublequotes.
Example
Integer.3=PartBody
Sample
Hole.1 .GetAttributeInteger("Integer.2")
KwrObject.CATPart
GetAttributeReal Method
Returns the value of a real or Length (in m) type parameter added to a given feature by using the Knowledge Advisor product. parameterName is the name of the string type parameter. It should be put between quotation marks ("). This method enables you to read: • • •
Syntax
The attributes added to parameters using the Parameters Explorer. The real attributes added to objects. The User Properties of a product.
feature.GetAttributeReal(String): String where String is name of the attribute. This name should be put between doublequotes.
GetAttributeString Method
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Syntax
The attributes added to parameters using the Parameters Explorer. The real attributes added to objects. The User Properties of a product.
feature.GetAttributeString(String): String where String is name of the attribute. This name should be put between doublequotes.
Example
String.2 =PartBody
Sample
Pad.1 .GetAttributeString("String.1")
KwrObject.CATPart
HasAttribute Method
Determines whether the attribute specified in the argument belongs to the feature the method is applied to.
Syntax
feature.HasAttribute(String): Boolean where String is name of the attribute. This name should be put between doublequotes.
Example
Boolean.2 = PartBody
Sample
Hole.1.HasAttribute("Real.1")
KwrObject.CATPart
Id Method
Applies to a feature. Retrieves the identifier of a feature.
Syntax
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Example
String.2=PartBody Pad.1.Id() + PartBody Pad.1.AbsoluteId()
Sample
KwrTopology.CATPart
IsOwnedBy Method
Determines whether the feature specified in the argument is the parent of the feature the method is applied to. featureName should be put between quotation marks (").
Syntax
feature.IsOwnedBy(): Boolean
Example
Boolean.1=PartBody
Sample
Hole.1.IsOwnedBy(PartBody)
Topology.CATPart
IsOwnedByString Method
Applies to a feature. Determines whether a feature belongs to another. This method returns a string.
Syntax
feature.IsOwnedByString(): Boolean
IsSupporting
Function indicating if the object passed in argument is supported or not.
Example
H:Hole H->IsSupporting("TaperedHole") == true
Name Method
Applies to a feature. Retrieves the name of a feature. Cannot be used to rename a feature.
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Syntax
feature.Name(): String
Example
String.1=PartBody
Sample
Pad.1.Name()
KwrTopology.CATPart
SetAttributeBoolean Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the boolean type parameter whose value is to be modified. It should be put between quotation marks ("). booleanvalue is either TRUE or FALSE.
Syntax
feature.SetAttributeBoolean(String, Boolean): Void where the first argument is name of the attribute while the second is the value to be assigned to it.
Example
if PartBody PartBody
Sample
Pad.1
Boolean.1 <> true
Pad.1.SetAttributeBoolean("Boolean.1", true)
KwrObject.CATPart
SetAttributeReal Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the real type parameter whose value is to be modified. parameterName should be put between quotation marks (").
Syntax
feature.SetAttributeReal(String, Real): Void where String is name of the attribute and Real the value to be assigned to the parameter.
Example
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if PartBody PartBody
Sample
Hole.1
Real.1 <> 3
Hole.1 .SetAttributeReal("Real.1",3)
KwrObject.CATPart
SetAttributeString Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the string type parameter whose value is to be modified. parameterName and stringvalue should be put between quotation marks (").
Syntax
feature.SetAttributeString(String, String): Void where the first argument is name of the attribute while the second is the value to be assigned to it.
Example
if PartBody PartBody
Pad.1.GetAttributeString("String.1") <> "String1" Pad.1 .SetAttributeString("String.1","This is a test")
Another syntax for the same rule is: if PartBody PartBody
Sample
Pad.1
String.1 <> "String1"
Pad.1.SetAttributeString("String.1","This is a test")
KwrObject.CATPart
SetAttributeInteger Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the integer type parameter whose value is to be modified. parameterName should be put between quotation marks (").
Syntax
feature.SetAttributeInteger(String, Integer): Void where the first argument is name of the attribute while the second is the value to be assigned to it.
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Example
if PartBody PartBody
Sample
Hole.1
Integer.1 <> 3
Hole.1 .SetAttributeInteger("Integer.1", 3)
KwrObject.CATPart
SetAttributeDimension Method
Assigns the value specified in the second argument to the parameter whose name is specified in the first argument. parameterName is the name of the parameter whose value is to be modified. parameterName should be put between quotation marks ("). The unit used is the current one.
Syntax
feature.SetAttributeDimension(String, Real, String): Void Type where the first argument is name of the attribute, the second is the value to be assigned to it and the third is the type.
Example
H:Hole H->SetAttributeDimension("Myhole",5,"Length")
Messages and macros
LaunchMacroFromDoc Function Question Function LaunchMacroFromFile Function VBScriptRun Message Function
LaunchMacroFromDoc Function
Executes a macro stored in a document from a rule. A macro is stored in a document when you don't specify any external file before recording it. Warning: It is up to you to check that the macro which is run is not going to cause an infinite loop or result in a system crash.
Syntax
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Example
LaunchMacroFromDoc("Macro1")
Question Function
Displays a message in a dialog box, waits for you to click a button and returns a value indicating which button you clicked (true if Yes was clicked, false if No was clicked)
Syntax
Question(String [# String1 # String2 ..., Param1Name, Param2Name, ...] ): Boolean The Question function takes one required argument and several optional arguments depending on whether parameter values are to be displayed in the message. Arguments String # String1, Param1Name... Description Required. String to be displayed in the dialog box (should be put in quotes). Optional. When parameter values are to be displayed within the message, the arguments should be specified as follows: • one string in quotes including a # symbol wherever a parameter value is to be displayed as many [, parameter name] statements as parameter values declared with a "#" in the message.
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Use the "|" symbol to insert a carriage return in a prompt.
Example
Boolean2 = Question("SketchRadius is # | Do you want to change this value ?", PartBody Sketch.1 Radius.3 Radius )
Note that you can use the Question function together with the BuildMessageNLS function for your question to display in your language. To
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use this function, use the following syntax: question(BuildMessageNLS ("x","xx",a,b)) • • • x corresponds to the name of the CATXXX.CATNls file where you will find the NLS message (it is the CATXXX name without the CATNls extension). xx corresponds to the key name in this catalog. a and b are the arguments (values that will be replaced in the message)
LaunchMacrofromFile Function
Executes a macro CATScript from a rule. Warning: It is up to you to check that the macro which is run is not going to cause an infinite loop or result in a system crash.
Syntax
LaunchMacroFromFile("MacroName.CATScript" )
Example
LaunchMacroFromFile("Macro1.CATScript")
Run Method
Runs a macro with arguments. Warning: It is up to you to check that the macro which is run is not going to cause an infinite loop or result in a system crash.
Syntax
VB Script.Run(valueOrFeature:ObjectType,...): Void where valueOrFeature is the macro argument name. There can be several arguments.
Example
You must have created the VB Script.1 macro prior to creating the rule below: if PartBody Pad.1.HasAttribute("String.1") == true Pad.1 Pad.1.Name() )
`VB Script.1` .Run(PartBody
.GetAttributeString("String.1"),PartBody
Sample
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Message Function
Displays a message in an information box. The message can include one or more parameter values.
Syntax
Message(String [# String1 # String2 ..., Param1Name, Param2Name, ...] ) : Void The Message function takes one required argument and several optional arguments depending on whether parameter values are to be displayed in the message. Arguments String # String1, Param1Name... Description Required. String to be displayed in the information box (should be put in quotes). Optional. When parameter values are to be displayed within the message, the arguments should be specified as follows: • one string in quotes including a # symbol wherever a parameter value is to be displayed as many [, parameter name] statements as parameter values declared with a "#" in the message.
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Use the "|" symbol to insert a carriage return in a message.
Example 1
Message("External radius is: # | Internal Radius is: #", PartBody PartBody Sketch.1 Hole.1 Radius.3 Diameter) Radius,
Example 2
Note that this function can be used along with the buildMessageNLS function Message (BuildMessageNLS("KwrCATCatalog.CATNls","Zero")) Where x,y,z are parameters.
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Note that you can use the Message function together with the BuildMessageNLS function for your question to display in your language. To use this function, use the following syntax: Message(BuildMessageNLS ("x","xx",a,b)) • • • x corresponds to the name of the CATXXX.CATNls file where you will find the NLS message (it is the CATXXX name without the CATNls extension). xx corresponds to the key name in this catalog. a and b are the arguments (values that will be replaced in the message)
Limitations
Parameters and Formulas
• • The output parameter (the one that is valuated) of a formula can not be a publication. The bypass is to use a rule. If you want to edit a formula located in another document (not the UI active one) in the Formula editor, a warning is displayed and the formula editor is grayed out.
Design Tables
When working with design tables in .xls format, the Undo command may not work properly.
Rules
• • Geometrical features valuated by a rule should not be used as the construction support of sub-elements. If you create a rule driving formulas activity, you might encounter update problems.
Sets of Equations
In set of equations, there is no control of units coherence (like in rule, check, formula).
Macros with Arguments
It is not possible to use the InputBox Visual Basic function in the definition of macros with arguments on unix. The SelectElement method on Selection object does not work either (on all Operating Systems).
Loops
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A loop can only generate items in the document it belongs to. So, in the graphic opposite, the loop cannot generate items in Product3. this restriction applies also to assemblies made up of different parts. A loop located in one of the Parts cannot generate items in another Part of the assembly.
Useful Tips
Relations
When using some objects, you need to indicate the destination of the formulas and the rules that valuate the parameters of these objects. If you valuate a time parameter in a kinematic simulation for example, the relation will not be located below the Relations set but in the mechanisms and commands tree of the simulation.
Hiding relations
You can hide a knowledge relation (formula, rule, check, ..) by right-clicking this relation in the specification tree and by selecting the Hide command. • A visual indicator located at the Relations set level indicates that the set contains hidden relations. Note that this indicator is not recursive. If you try to delete a relations set containing hidden relations, a message is displayed asking you if you want to delete the relations set that contains hidden relations. Note that if you try to delete a relations set containing another relations set with hidden relations, the message will be displayed.
•
Relations Updates
The evaluation of relations containing measures can be integrated to the Part update only. In a .CATProduct or in a .CATProcess file, to create a parameter
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User Tasks • • which value is the result of a relation containing measures updated when modifying the measure inputs:
1. Create the relation containing the measure at the Part level. 2. Integrate the relation evaluation to the Part update. 3. At the Product or the Process level, create a relation that valuates the parameter by using the result parameter of the relation created at the Part level. To get an example, see KwrUpdate.CATProduct. 4. Perform a local update at the Relations level.
Syntax errors in relations message
When loading a document, the message opposite can appear. It means that during the load, some relations appeared as broken. These relations use functions that are not recognized by the dictionary because the library containing the definition of the function is not still loaded. That's why you are asked if you want to load all the libraries containing functions definition. But loading all libraries may have an impact on performances. So, we recommend you to load only the libraries you are interested by. To do so, select the required libraries in the Language tab (Tools>Options->General>Knowledge->Language.)
Rules
Geometrical Features and Rules
In a rule using features that need the geometry to return the type (such as extrudes), when the feature is deactivated, the type cannot be returned. To solve the problem, use the Set command to indicate the type in the rule. To know more, see the KwrSetType.CATPart file.
Rules and Update Cycle
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This configuration is allowed since a modification of the parameter activity does not impact the formula update. But: • • • In such a case, it is highly recommended to use the reaction feature. If you want to use a rule, do not deactivate and reactivate the activity parameter. When working with a UDF feature, make sure that you have inserted the relation set when defining the UDF.
Parameters
• You can add properties to a .CATPart or a .CATProduct document by using the Properties command from the contextual menu. You just have to click the Define other properties... button in the Product tab then click New parameter of type. The dialog is similar to the f(x) dialog. See the Product Structure User's Guide for more information. The properties you define that way are also displayed in the parameter list of the f(x) dialog box. Parameters belonging to a parameter set can be reordered by using the Reorder... command from the contextual menu. Parameters added by using the Parameters Explorer are displayed right below the feature they are assigned. CATIA users working with non-latin characters should check the Tools>Options>Knowledge->Parameter Names->Surrounded by' option. Otherwise, parameter names should have to be renamed in latin characters when used in formulas. You can specify that a parameter is constant by using the Properties command from the contextual menu. This command also enables you to hide a parameter. When copying parameters sets containing hidden parameters, these parameters are automatically pasted when pasting the parameters sets and appear as hidden parameters. Parameters have 2 different names: The local one and the global one. o The local name is the name attributed to the parameter when it was created in the Formula Editor or in the Parameters Explorer. Note that this name will not be modified if you perform a Reorder using the contextual menu.
•
•
•
• •
•
This name can be modified using the Parameters Explorer and the Edit>Properties command. o The global name (name) is the name attributed to the parameter by Knowledge Advisor. It is the path of the parameter + its type. If you select
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the parameter and reorder it, the path contained in the name will be modified. If you double-click the parameter in the specification tree, and enter a new name in the Edit Parameter dialog box, the global name will be changed. If, after renaming the parameter in the Edit Parameter dialog box, you reorder the parameter the path will not appear any more. This name can be modified in the Edit Parameter dialog box. • • When renaming parameters using the Edit->Properties command, do not apply names similar to the parameters types available in the Formula Editor. For example, if you rename a Length parameter into Time, the name will be converted into Time.1. Deleting parameters used in a relation: If you delete a parameter used in a relation, a "clone" parameter will be created. Applying the same formula to several parameters: If you want to apply the same formula to several parameters, use the Equivalent Dimensions feature and value this feature by a formula. To know more, see Using the Equivalent Dimensions Feature.
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Formulas
• The Incremental option of the formula editor :The Incremental option allows you to restrict the list of parameters displayed in the dictionary. Select a feature either in the tree or in the geometry area. Only the first level of objects right below the selected feature will be displayed in the dictionary. If the Incremental option is unchecked, all the objects below the selected feature are displayed. The Incremental mode is useful when you work with large documents and when the parameter lists are long. Tips about the formula editor: To help you write a formula, the formula editor provides you with a dictionary. This dictionary exposes the list of parameters and functions you can use to define a formula. Depending on the category of objects to be referred to in the formula, the dictionary is divided into two or three parts. To insert any definition in the formula editor, just double-click the object either in the dictionary or in the tree. If you doubleclick a function in the dictionary, its signature is carried forward to the formula editor. Only the argument definitions are missing.
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Design Tables
• A design table can only be created from non-constrained parameters, i.e.
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Anytime you modify a design table, the relations that refer to this design table detect the modification and turn to a to-be-updated status.
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As long as a design table is active, the parameters which are declared in it are constrained parameters and you are not allowed to modify them. Double-clicking a design table in the specification tree displays the design table with its set of configurations and allows you to select a new configuration.
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Only parameters which are not already constrained by any other relation or by any other design table can be used to create a design table. If a parameter is already constrained, it does not appear in the Parameters to insert list in the design table dialog box.
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Selecting the parameters to be inserted in a design table The Filter Name and Filter Type filters can be used to restrict the display of a parameter list. If you specify x in the Filter Name field of the Select parameters to insert dialog box, you will display all the parameters with the letter x in their name (xA, xB, xC, xD, xE). If you select the Renamed Parameters in the Filter Type list, you will display all the parameters you have renamed in the Formulas dialog box (yA, xB, xA, yC, xC, yB, yD, xD, yE, xE, TangE). Parameters to be inserted can be multi-selected. You just have to keep on pressing the Ctrl key while you select parameters. If you do this, the group of multi-selected parameters will be carried forward onto the Inserted parameters list in the order in which they are displayed in the initial list. When the design table is created, the rank of the columns fits the rank of the parameters in the Inserted parameters list. If you want to have columns ordered in a given way in the design table, you must insert the parameters one by one.
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Accessing the functions related to the design table Once in the formula (rule or check) editor, select the Design Table item in the dictionary, the list of the methods that can be applied to a design table is displayed. Select a method, then click F1 to display the associated documentation.
Loops
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Generic Naming: Generic naming is a CATIA technique which creates a label whenever an element has been selected interactively. This label is a coded description of the selected element. When you specify a fillet to be applied to a face, you must select interactively the face definition but prior to doing this you must of course have generated the face to be filleted. This is why scripts requiring face, point or edge definitions cannot be generated in one shot. You don't have to mind about the generic naming itself as it is automatically captured from the geometry area. The thing you have to mind about is the order your instructions are to be written and executed in the script. Message "property does not exist...": Check in the browser that the attribute name is correct. For attributes of list type (Fillets and Chamfers), check the indexes. The indexes specified must be consecutive from 1 to n without any gaps. Specifying a File Path (2 methods)
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• Syntax
There are 2 ways to specify the file path: • import "File path"; : Indicate the path of the file to be imported: import "E: users kwecx Models PartImport.CATPart" ;. Note that you should enclose the path within quotation marks and end the import statement with a semicolon (;). import "File Name"; : Indicate only the name of the file to be imported if this file is located in the same directory as the document containing the loop: import "PartImport.CATPart";. Note that: o You should enclose the document name within quotation marks and end the import statement with a semicolon (;). The file to be imported should be located in the same directory as the document containing the loop. The document containing the loop should be saved.
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To specify a file to be imported, you can use the 'Insert File Path' command from the contextual menu. Selecting this command displays a file selection window. Quotation marks are automatically included but not the semicolon • Importing Sketches: Recommendation
When designing a document to be generated by a script, it is better to group all the required sketches in a single file. That way: • you minimize the overall size of your sketch-related data • no matter the method used to specify the input file, you just have to specify
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the path once • the design of the final document is made easier. You get a global view of the sketches on which the other features rely. Specifying Strings: Recommendation: Double quotation marks as well as single quotation marks of apostrophe type (`) can be used to delimit strings. Single quotations marks (`) must be used to enclose character strings which contain other strings.
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Reactions
There are 2 ways to react to parameter changes using the reaction feature: • Or • Select the feature (that owns the attribute corresponding to your parameter) and react to the Attribute Modification event. Note that this method does not work in all cases. Select the parameter and react to its Value Changed event
Use Cases
Use Cases
Link Bar 5
The Ball Bearing
The Ball Bearing
A bearing is defined by parameters such as its principal dimensions, its basic load ratings, its limiting speeds and its mass. It belongs to a category which corresponds a certain range of its parameter values. In a catalogue, a bearing is referred to by a designation. Bearing types are described by tables which define the bearing parameter values including the designation. The bearing example has been chosen here because the bearing tables given in distributor and retailer catalogues illustrate quite well the design table principles. The bearing itself is a good example of how components within a mechanical part can be constrained by relations. In the scenario below, you start from an existing document inspired by a deep groove ball bearing. This document contains already a number knowledgeware relations, others are added to control the document design.
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Link Bar 4
Before you Start
Here is the data required to perform the scenario. They are all delivered with the Knowledge Advisor product but can be rebuilt from the information given below. See the Infrastructure User's Guide for how to specify the material library settings (you must use the Tools->Options...->Infrastructure->Material Library command from the standard menu bar).
The Initial Document
The initial document is the KwrBallBearing1.CATPart document.
The bearing rings are coaxial shafts created from the Sketch.1 and Sketch.2 features. The balls are shafts created from the Sketch.3 feature.
The Outer Ring
The outer ring is a shaft generated by rotating the Sketch.1 highlighted in figure below around an axis coaxial to V. Note that you must create this axis as a construction element, otherwise CATIA won't let you create the Shaft. The lower part of the sketch is the symmetry of the upper part with respect to the H axis.
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Here are the constraints defined on this sketch: d1 L1 B1 R1 b1 D1 2.1 mm 3 mm 5 mm ring width half height of the non - hollowed inner surface half height of the outer surface
2.759 mm groove radius 0 mm 13 mm ordinate of the groove center external diameter
The Inner Ring
The inner ring is a shaft generated by rotating the Sketch.2 highlighted in figure below around an axis coaxial to V.
Here are the constraints defined on this sketch:
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d2 L2 B2 R2 b2 D2
2.1 mm 3 mm 5 mm
ring width half height of the non - hollowed inner surface half height of the outer surface
2.759 mm groove radius 0 mm 7.1 mm ordinate of the groove center internal diameter
The Balls
A ball is a shaft created by rotating half a circle (sketch.3) around the H axis. The circle must be closed before being rotated.
The parameters of the circular pattern which is created to build the set of balls are constrained by the formulas below: • BallNumber = int(3* D3 / BallRadius) • AngStep = 3.6deg / BallNumber D3 being the abscissa of the ball center.
The Import File
In the scenario, you have to import the text file below which is delivered under the KwrBallBearingImport.txt name.
Temperature 100Kdeg Pressure
Maximum temperature allowed
190N_m2 Maximum pressure allowed L1*D3*B1*0.005 required lubricant volume
LubricantVolume 0mm3
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If you modify this file, pay attention to the column format, use the Tab key to skip from one column to the other.
The Excel Table which Controls the Bearing Design
You must download the KwrBearingDesignTable.xls Excel table in your environment.
The CATScript Macro
The KwrBearing.CATScript macro just creates a circular pad. You can record this macro on your own in the Part Design workbench or use the one supplied with the KnowledgeAdvisor samples. When creating Rule.2 in your own environment, you should replace the pathname given as the argument of the LaunchMacroFromFile function with the pathname corresponding to the file where the macro has been downloaded.
Step-by-Step Procedure
Controlling the Bearing Design with a Design Table
A design table is created from a pre-existing file. The data set contained in this pre-existing file is quite similar to the data set which identifies a bearing in a catalogue. The design table which is created defines a number of configurations. Applying a new configuration results in a bearing modification. 1. Open the KwrBallBearing1.CATPart document. 2. Click the Design Table icon in the standard toolbar.
3. Check the Create a design table from a pre-existing file option. Click OK. 4. Select the KwrBearingDesignTable.xls file and associate automatically the design table columns with the document parameters (i.e. click YES in the "Automatic Associations?" dialog box). 5. In the Design table dialog box, select the configuration 3 (Line 3) and click Apply. Your ball bearing has changed. It is now a bronze bearing with 21 balls. You can tell the difference when you look at the geometry area. The bearing width is also modified. Click OK to exit the Design Table dialog box. 6. Keep your document open and proceed to the next task.
Creating a Check
A combined check using the => syntax is created. This check is intended to display a message whenever the check is not satisfied. 1. Access the Knowledge Advisor workbench
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icon then click OK in the first Check Editor dialog box. The 2. Click the check editor is displayed. 3. In the Check Editor, select the Warning type and enter the string "BallNumber is too small" in the message field. Then enter the D3 >= 6mm => BallNumber > 6 relation in the edition box. 4. Click OK to create your check and exit the editor. At this stage, no particular message is displayed. The check is added to the specification tree with a green icon. For the configuration 3 of the design table, this is the status of the check relations: OK => OK 5. In the specification tree, double-click the design table and select the configuration 1. Click OK. The message "BallNumber is too small" is displayed. For the configuration 1 of the design table, this is the status of the check relations: OK => KO 6. Keep your document open and proceed to the next task
Creating a Multiple Value Parameter
A multiple value parameter is created. Depending on this parameter value, a rule which is created in the next task will display either a message or launch a macro. 1. Click the icon.
2. In the Formulas dialog box, select String in the New Parameter of type list. Select Multiple values in the with list, then click 'New Parameter of type'. 3. In the Value List of String dialog box, enter one-by-one the step1, step2 and step3 values. Click OK. 4. In Edit name or value of the current parameter, replace the String.1 string with Status, then click OK. The Status parameter is added to the specification tree.
Creating a Rule
This task creates a rule which displays a message prompting you to import a file or launches a macro.
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1. In the specification tree, double-click the design table feature and select the configuration 3 in the table which is displayed. You are back to 21 ball bearing. 2. Access the Knowledge Advisor workbench 3. Click the icon.
4. Enter the Rule.2 string in the Name field of the first dialog box. Click OK. 5. Copy/Paste the code below into the rule edition box (modify the macro path):
if Status == "step2" Message("Import the KwrBallBearingImport text file") else if Status == "step3" LaunchMacroFromFile("e:/tmp/KwrBearing.CATScript") 6. Click OK to add the rule to the document and execute it. icon. In the "Formulas" dialog box, select the Status parameter 7. Click the and replace its step1 value with step2. Click OK. A message asks you to import the KwrBallBearingImport text file. 8. Click Import and select the KwrBallBearingImport.txt file. Three parameters are then added to the document. Click OK in the dialog box displaying the parameters and formulas to be imported. 9. Select the Status parameter and replace the step2 value with step3. Click OK. The KwrBearing.CATScript is executed and a circular pad is created.
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System of Three Equations in Three Variables
When designing a product, you may come across a system of equations to be solved. Whatever these equations (linear or not), CATIA provides you with resolution methods. These methods are the Simulated Annealing algorithm and the "SetOfEquations" capability. Can you use either method ? If your set of equations is purely mathematical, the answer is yes. Otherwise, no. The SetOfEquations capability cannot solve systems using CATIA functions such as measures. To solve a system of equations using measures, you must use the Simulated Annealing algorithm. The Simulated Annealing algorithm is provided with the Product Engineering Optimizer product. The set of equations is to be specified as constraints and the variables are to be specified as free parameters. This resolution method is quite good although sometimes a bit long and you can use it to solve a broad range of cases. The trick about this algorithm is to adjust the precision and the other algorithm parameters. The example developed below works well with both methods. Just to illustrate a system that cannot be solved by both methods, you can draw a cube and create two user parameters: CubeSurface (of Area type) and CubeVolume (of Volume type). To calculate CubeSurface and CubeVolume, you can write either: CubeSurface = smartWetarea ( PartBody CubeVolume = smartVolume ( PartBody or CubeVolume = smartVolume ( PartBody Pad.1 ) Pad.1 ) Pad.1 )
Solving the System of Equations by a Simulated Annealing
1. Open a new part document. 2. Create six real type parameters by using the f(x) capabilities. Name these parameters x1, y1, z1 and x2, y2, z2. 3. Access the Product Engineering Optimizer product and click the icon.
4. In the Constraints tab, specify the three constraints (enter the constraints one-by-one) x1 + y1 - z1 == 0 x1*y1 - z1 == 0 sin(x1*1rad)**2 - y1 - 1 == 0 Specify a precision of 0.01 for all three constraints. If need be, see the Product Engineering Optimizer User's Guide. 5. In the Problem tab, specify x1, y1, z1 as free parameters and 1 as Step value for all three parameters. 6. Run the optimization process in Simulated Annealing mode. You can use the default termination criteria. After the process has finished running, the x1, y1 and z1 values are close to the one below:
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x1 = 0.454 y1 = -0.807 z1 = -0.363 Keep your document open and proceed to the next task.
Solving the System of Equations by the "SetOfEquations" Capability
1. Access the Knowledge Advisor workbench, then click the icon. 2. In the "Set of Equations" editor, enter the set of equations below: x2 + y2 == z2 ; x2*y2 == z2; sin(x2*1rad)**2 == y2 +1 Specify x2, y2 and z2 as Unknown parameters by using the Parse arrow button ( ).
3. Click OK. The system of equations is solved. The values below are displayed in the specification tree x2 = 0.448043478 y2 = -0.812335288 z2 = -0.364229828
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Reference
The packages listed below are those displayed in the Browser when specifying a loop body. Basic Wireframe Package GSD Shared Package Mechanical Modeler Part Shared Package GSD Package Knowledge Expert Part Design Standard
Basic Wireframe Package
GSMPoint
Definition:
A GSMPoint is a point: • • generated by the Generative Shape Design product available in the BasicWireFrame Package.
To find out more about points, see the Generative Shape Design User's Guide.
Attributes:
PointType A point is defined by its type. The attribute to use is PointType. The syntax to be used is: PointType = i, i corresponding to the type of point that you want to create.
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Please find below a table listing the existing types of points that you can create and the digit to indicate. PlaneType in GSD Coordinates On surface On curve On plane Circle center Plane Type in the Package GSMPointCoord GSMPointOnSurface GSMPointOnCurve GSMPointOnPlane GSMPointCenter 0 1 2 3 4 Corresponding digit
As mentionned above, you may create 5 different point sub-types. Please find below a description of each sub-type, as well as its attributes and the syntax to use.
Coordinates (GSMPointCoord)
The sub-type to be used in this case is GSMPointCoord which enables you to create a coordinate point. The following attributes are available for this sub-type: • RefPoint (Reference point, optional). If specified, x, y, and z are indicated in a mark whose origin is this reference point. X (First coordinate) Y (Second coordinate) Z (Third coordinate)
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These attributes can be combined as follows: Combination • • • • RefPoint (Reference point, optional) X which is defined by the syntax below: X = 10mm; Y which is defined by the syntax below: Y = 10mm; Y which is defined by the syntax below: Z = 10mm;
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On surface (GSMPointOnSurface)
The sub-type to be used in this case is GSMPointOnSurface which creates a point on a plane. The following attributes are available for this sub-type: • Direction: Element taking its orientation as reference direction or a plane taking its normal as reference direction RefPoint: Reference point. By default, the surface middle point is taken as reference. Support: Surface where the point is to be created. Values: Distance along the reference direction used to display a point.
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• •
These attributes can be combined as follows: Combination • • • Direction which is defined by the syntax below: Direction = object: .. Line.1; Support which is defined by the syntax below: Support= object: .. Extrude.1; Values which is defined by the syntax below: Values = 12mm;
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On curve (GSMPointOnCurve)
The sub-type to be used in this case is GSMPointOnCurve which enables you to create a point on a curve. The following attributes are available for this sub-type: • • • • Boundary: Not available. RefPoint: Reference point. If not specified, it is the extremity of the curve. Support: Curve Values: Distance between the reference point and this point. Combination • • • Refpoint which is defined by the syntax below: RefPoint= object: .. Point.1; Support which is defined by the syntax below: Support = object: .. Line.1; Values which is defined by the syntax below: Values = 12mm;
On plane (GSMPointOnPlane)
The sub-type to be used in this case is GSMPointOnPlane. It creates a point on a plane. The following attributes are available for this sub-type: • • • Direction (optional). When specified, indicates the direction H: Vector. RefPoint: point used to define a reference for computing coordinates in the plane. Support: Plane on which the point will be created.
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V: Vector.
The attributes should be used as follows: Combination • • • • • Direction which is defined by the syntax below: Direction = object: .. Line.1; H which is defined by the syntax below: H = 150mm; RefPoint which is defined by the syntax below: RefPoint= object: .. Point.1; Support which is defined by the syntax below: Support = object: 'xy plane' V which is defined by the syntax below: V = 150mm;
Circle Center (GSMPointCenter)
The sub-type to be used in this case is GSMPointCenter which enables you to define the center of a circle. • Curve: circle, circular arc, or ellipse.
This attribute is to be used as follows: Combination • Curve which is defined by the syntax below: Curve = object: .. Extrude.1;
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GSMLine
Definition:
A GSMLine is a line : • • generated by the Generative Shape Design product. available in the BasicWireFrame Package.
To find out more about lines, see the Generative Shape Design User's Guide.
Attributes:
LineType A line is defined by its type. The attribute to be used is LineType. The syntax to be used is: LineType = i, i corresponding to the type of line that you want to create. Please find below an equivalence table listing the existing types of lines that you can create and the digit to indicate. Line Type in GSD Point to Point Point-Direction Angle to Curve Tangent to Curve Normal to surface Line Type in the Package GSMLinePtPt GSMLinePtDir GSMLineAngle GSMLineTangency GSMLineNormal 0 1 2 3 4 Corresponding digit
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Intersection betw. 2 planes
GSMLineBiTangent
5
As mentioned above, you may create 7 different line sub-types. Please find below a description of each sub-type, as well as its attributes and the syntax to use.
Point to Point Line (GSMLinePtpt)
The sub-type to be used in this case is GSMLinePtpt which defines the line extremities. The following attributes are available for this sub-type: • • • • • FirstPoint (feature) SecondPoint (feature) Support (feature) Length1 (length, optional for both combinations) Length2 (length, optional for both combinations)
These attributes can be combined as follows: 1st combination • the FirstPoint which is defined by the syntax below: FirstPoint = object: .. .. theFirstPoint; the SecondPoint which is defined by the syntax below: SecondPoint = object: .. .. theSecondPoint; Length1 which is defined by the syntax below: Length1=200mm; Length2 which is defined by the syntax below: Length2=150mm; • 2nd combination the FirstPoint which is defined by the syntax below: FirstPoint = object: .. .. theFirstPoint; the SecondPoint which is defined by the syntax below: SecondPoint = object: .. .. theSecondPoint; the Support
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Point-Direction (GSMLinePtDir)
The sub-type to be used in this case is GSMLinePtDir which defines the line direction. The following attributes are available for this sub-type: • • • • • • Length1 Length2 Direction Orientation RefPoint Support
These attributes can be combined as follows: Combination • • • • • Length1 which is defined by the syntax below: Length1 = 100mm; Length2 which is defined by the syntax below: Length2 = 10mm; Direction which is defined by the syntax below: Direction = object: .. .. Plane.2; RefPoint which is defined by the syntax below: RefPoint = object: .. .. Point.2; Support which is defined by the syntax below: SecondPoint = object: .. .. 'xy plane';
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Tangent to Curve (GSMLineTangency)
The sub-type to be used in this case is GSMLineTangency. The following attributes are available for this sub-type: • • • • • • Curve: Reference curve used to define the tangency. Length1 Length2 Orientation RefPoint: Reference point used to define the tangency. Support
These attributes can be combined as follows: Combination • • • • • Curve which is defined by the syntax below: Curve = object: .. .. Spline.2; Length1 which is defined by the syntax below: Length1 = 100mm; Length2 which is defined by the syntax below: Length2 = 10mm; RefPoint which is defined by the syntax below: RefPoint = object: .. .. Point.2; Support which is defined by the syntax below: SecondPoint = object: .. .. 'xy plane';
Normal to surface (GSMLineNormal)
The sub-type to be used in this case is GSMLineNormal. The following attributes are available for this sub-type:
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• • •
Orientation RefPoint RefSkin
These attributes can be combined as follows: Combination • • RefPoint which is defined by the syntax below: RefPoint = object: .. .. Point.2; Support which is defined by the syntax below: RefSkin = object: .. .. Extrude.1;
GSMPlane
Definition:
A GSMPlane is a plane: • • generated by the Generative Shape Design product. available in the BasicWireFrame Package.
To find out more about planes, see the Generative Shape Design User's Guide.
Attributes:
PlaneType A plane is defined by its type. The attribute to use is PlaneType. The syntax to be used is: PlaneType = i, i corresponding to the type of plane that you want to create. Please find below a table listing the existing types of planes that you can
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create and the digit to indicate. PlaneType in GSD Equation Through 3 points Through 2 lines Through a point and a line Normal to a curve Tangent to a surface Normal to a plane Plane Type in the Package GSMPlaneEquation GSMPlane3Points GSMPlane2Lines GSMPlane1line1Pt GSMPlane1Curve GSMPlaneTangent GSMPlaneNormal 0 1 2 3 4 5 6 Corresponding digit
As mentionned above, you may create 7 different plane sub-types. Please find below a description of each sub-type, as well as its attributes and the syntax to use.
Equation (GSMPlaneEquation)
The sub-type to be used in this case is GSMPlaneEquation which enables you to create a plane by using an equation. The following attributes are available for this sub-type: • • • • • A (First component of the equation) B (Second component of the equation) C (Third component of the equation) Length RefPoint (point used to position the plane through this point)
These attributes can be combined as follows: 1st Combination • • • • A which is defined by the syntax below: A=31; //A value is required B which is defined by the syntax below: B=-47; //A value is required C which is defined by the syntax below: C=-24; //A value is required Length: enables the user to indicate the required length. It is defined by the syntax below: • • • • 2nd Combination A which is defined by the syntax below: A=31; //A value is required B which is defined by the syntax below: B=-47; //A value is required C which is defined by the syntax below: C=-24; //A value is required RefPoint which is defined by the syntax below: RefPOint = object: .. Point ;
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Length=24mm
Through 3 points (GSMPlane3Points)
The sub-type to be used in this case is GSMPlane3Points which creates a plane passing through 3 points. The following attributes are available for this sub-type: • • • Element1 (First point) Element2 (Second point) Element3 (Third point)
These attributes can be combined as follows: Combination • • • Element1 which is defined by the syntax below: Element1 = object: .. Point.1; Element2 which is defined by the syntax below: Element2 = object: .. Point.2; Element3 which is defined by the syntax below: Element3 = object: .. Point.3;
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Through 2 Lines (GSMPlane2Lines)
The sub-type to be used in this case is GSMPlane2Lines which enables you to create a plane passing through 2 lines. The following attributes are available for this sub-type: • • Element1 (First line) Element2 (Second line)
Combination • • Element1 which is defined by the syntax below: Element1 = object: .. Line.1; Element2 which is defined by the syntax below: Element2 = object: .. Line.2;
Through a Point and a Line (GSMPlane1line1Pt)
The sub-type to be used in this case is GSMPlane1Line1Pt which enables you to create a plane passing through a line and a point. The following attributes are available for this sub-type:
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• •
Line: Line used to create the plane. RefPoint: Point used to create the plane.
The attributes should be used as follows: Combination • • Line which is defined by the syntax below: Line = object: .. Line.1; RefPoint which is defined by the syntax below: RefPoint = object: .. Point.2;
Normal to a Curve (GSMPlane1Curve)
The sub-type to be used in this case is GSMPlane1Curve which enables you to create a plane normal to a curve at a specified point. • Element1: Line
This attribute is to be used as follows: Combination • Line which is defined by the syntax below: Line = object: .. Spline.1;
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Tangent to a Surface (GSMPlaneTangent)
The sub-type to be used in this case is GSMPlaneTangent which enables you to create a plane tangent to a surface at a specified point. The following attributes are available for this sub-type: • • RefPoint (Point) Support (Surface)
These attributes are to be used as follows: Combination • Support which is defined by the syntax below: Support = object: .. • Spline.1;
RefPoint which is defined by the syntax below: RefPoint = object: .. Point.4;
Normal to a Plane (GSMPlaneNormal)
The sub-type to be used in this case is GSMPlaneNormal. The following attributes are available for this sub-type: • • Curve: Reference curve used to create the plane. RefPoint: Reference point used to create the plane.
These attributes are to be used as follows: Combination
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•
Curve which is defined by the syntax below: Curve = object: .. Spline.1;
•
RefPoint which is defined by the syntax below: RefPoint = object: .. Point.4;
GSMCircle
Definition:
A GSMCircle is a circle: • • generated by the Generative Shape Design product. available in the BasicWireFrame Package.
To find out more about circles, see the Generative Shape Design User's Guide.
Attributes:
PointType A point is defined by the following attributes: • CircleType: The syntax to be used is CircleType = i, i corresponding to the type of circle that you want to create.
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• • •
CircleRelimitation: The syntax to be used is CircleRelimitation =. EndAngle: The syntax to be used is EndAngle = xxxdeg. StartAngle: The syntax to be used is StartAngle =xxxdeg.
Please find below a table listing the existing types of circles that you can create and the digit to indicate. PlaneType in GSD Three Points Center and Radius Center and Point Plane Type in the Package GSMPCircle3Points GSMCircleCtrRad GSMCircleCtrPt 3 0 1 Corresponding digit
As mentionned above, you may create 3 different circle sub-types. Please find below a description of each sub-type, as well as its attributes and the syntax to use.
Three Points (GSMCircle3Points)
The sub-type to be used in this case is GSMCircle3Points which enables you to create a circle passing through 3 points. The following attributes are available for this sub-type: • • • • Element1: First point Element2: Second point Element3: Third point Support: Support surface onto which the circle will be projected (optional)
These attributes can be combined as follows: Combination • • • • Element1 which is defined by the syntax below: Element1 = object: .. Point.1; Element2 which is defined by the syntax below: Element2 = object: .. Point.2; Element3 which is defined by the syntax below: Element3 = object: .. Point.3; Support which is defined by the syntax below: Support = object: .. Extrude.1;
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Center and Radius (GSMCircleCtrRad)
The sub-type to be used in this case is GSMCircleCtrRad which enables you to create a circle by indicating its center and its radius. The following attributes are available for this sub-type: • • • • • Center: Point that will be the center of the circle. FirstDirection Geodesic Radius: Radius of the circle. Support: Support plane or surface onto which the circle is to be created.
These attributes can be combined as follows: Combination • • • Center which is defined by the syntax below: Center = object: .. Point.1; Radius which is defined by the syntax below: Radius = 120mm; Support which is defined by the syntax below: Support = object: .. Extrude.1;
Center and point (GSMCircleCtrPt)
The sub-type to be used in this case is GSMCircleCtrPt which enables you to create a circle by indicating its center and a point. The following attributes are available for this sub-type: • • • • Center: Point used as the center of the circle. Geodesic: Curve. RefPoint: Second point used to create the circle. Support: Support plane or surface where the circle is to be created. Combination • Center which is defined by the syntax below:
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• •
Center = object: .. Point.1; RefPoint which is defined by the syntax below: RefPoint = object: .. Point.1; Support which is defined by the syntax below: Support = object: .. Extrude.1;
Part Design Package
Please find below a table listing the types available in the Part Design package. Box Counterbored Hole Cylinder Pocket Shaft SoldCombine Thickness Chamfer Counterdrilled Hole Hole RemoveFace Shell Split ThickSurface Cone Countersunk Hole Pad ReplaceFace SimpleHole TaperedHole Torus
Box
Definition:
A box is a pad extruded from a rectangular sketch.
Attributes:
A box is defined by the following attributes: • • • Length which is the pad first limit. The syntax to be used is Length = 10mm. Width which is the pad width. The syntax to be used is Width = 20mm. Height which is the pad height. The syntax to be used is Height = 12mm.
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MyBox isa CATPart { BoxPart isa Part { PartBody isa BodyFeature { // Create a box Box1 isa Box { // Specify the box properties Width = 20.0 mm ; Height = 25.0 mm ; Length = 15.0 mm ; } } } }
Chamfer
Definition:
A cut through the thickness of the feature at an angle, giving a sloping edge.
Attributes:
A chamfer is defined by the following attributes: • • • Angle. The syntax to be used is Angle = 20 deg; Length1. The syntax to be used is Length1 = 5 mm; Length2. The syntax to be used is Length2 = 5 mm;
Important Notes: • A chamfer has a Length2 attribute which is the default chamfer length. You don't have to manipulate this attribute in a script.
To specify a chamfer within your script, you must have a part open, then: 1. Create a Chamfer by using the isa function Chamfer1 isa Chamfer ( ) { } 2. Right-click anywhere inside the parentheses and select the 'Get Edge' or the 'Get Surface' command from the contextual menu. Then, in the geometry
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area, select the edge or surface to be chamfered. MyBox isa CATPart { BoxPart isa Part { PartBody isa BodyFeature { // Create a box Box1 isa Box { Width = 20.0 mm ; Height = 25.0 mm ; Length = 15.0 mm ; } // Create a chamfer // The edge definition must be captured // from the geometry area // Use the Get Edge command from the // contextual menu Chamfer1 isa Chamfer (Edge Definition) { Angle = 20 deg; Length1 = 5 mm ; } Chamfer2 isa Chamfer (Edge Definition) { Angle = 30 deg; Length1 = 10 mm ; } } } }
Cone
Definition:
A cone is a shaft created by rotating a triangular sketch.
Attributes:
A cone is defined by the following attributes: • • Length. The syntax to be used is Length = 15.0 mm ;. Radius. The syntax to be used is Radius = 20.0 mm ;.
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MyCone isa CATPart { ConePart isa Part { PartBody isa BodyFeature { // Create a cone Cone1 isa Cone { Radius = 20.0 mm ; Length = 15.0 mm ; } } } }
Counterbored Hole
Definition:
A mechanical feature of Hole type you create when you click icon in the Part Design the workbench. For more information, refer to the Part Design User's Guide.
Attributes:
A counterbored hole is defined by the following attributes: • • CounterboreDepth. The syntax to be used is CounterboreDepth =12mm. CounterboreDiameter: The syntax to be used is CounterboreDiameter =15mm.
Counterdrilled Hole
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Definition:
A mechanical feature of Hole type you create when you click icon in the Part Design the workbench. For more information, refer to the Part Design User's Guide.
Attributes:
A counterdrilled hole is defined by the following attributes: • • • CounterdrillAngle. The syntax to be used is CounterdrillAngle = 22deg. CounterdrillDiameter. The syntax to be used is CounterdrillDiameter =12mm. CounterdrillDepth. The syntax to be used is CounterdrillDepth =12mm.
Countersunk Hole
Definition:
A mechanical feature of Hole type you create when you click icon in the Part Design the workbench. For more information, refer to the Part Design User's Guide.
Attributes:
A countersunk hole is defined by the following attributes:
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• • •
CountersinkAngle. The syntax to be used is CountersinkAngle = 12deg. CountersinkDepth. The syntax to be used is CountersinkDepth =15mm. CountersinkDiameter. The syntax to be used is CountersinkDiameter =15mm.
Cylinder
Definition:
A cylinder is a pad created by extruding a circular sketch.
Attributes:
A cynlinder is defined by the following attributes: • • EndLimit Length. The syntax to be used is Length =12mm. Radius: The syntax to be used is Radius =5mm.
Cylinder1 isa CATPart { Part isa Part { PartBody isa BodyFeature { // Create a cylinder Cyl1 isa Cylinder { Radius=15.0 mm; EndLimit=20.0 mm; } } } }
Hole
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Definition:
A is an opening through a feature.
Attributes:
A hole is defined by the following attributes: • • • • • • • • • • • • BottomAngle BottomType Depth Diameter DiameterThread HoleType LimitType Pitch TapSide Threaded ThreadingDepth Radius
To specify a hole within your script, you have to use one of the holes listed below. Hole is the father type and cannot be used. • • • • Counterbored Hole Countersunk Hole Counterdrilled Hole Tapered Hole
Pad
Definition:
A pad is a feature created by extruding a sketch.
Attributes:
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A pad is defined by the following attributes: • • • the sketch the pad is extruded from. the FirstLimit the SecondLimit Length (or StartLimit Length ( or EndLimit Length) Length).
A limit which is not specified is set by default to zero. // Use the Insert File Path command from the // contextual menu to specify the path of the file // to be imported import PktSketchToImport.CATPart;/*In the script above, the P0 pad is created from the Sketch.1 sketch which is imported from the document.*/
myDocument isa CATPart { myPart isa Part { PartBody isa BodyFeature { Sketch isa Sketch.1 {} P0 isa Pad("Sketch") { SecondLimit } } } } Length=40.0mm;
Shaft
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Attributes:
A shaft has two attributes: • • • • • • • The The The The The The The StartAngle. The syntax to be used is StartAngle=12deg. EndAngle. The syntax to be used is EndAngle=23deg. MergeEnd NeutralFiber Thickness1 Thickness2 Thinmode
The sketch to be rotated must be imported from an external CATPart document. This external document must also include a rotation axis. /* Use the Insert File Path command from the contextual menu to select the the sketch to be imported */ import //Use the Insert File Path command to insert the Pktsketch_shaft.CATPart file. MyShaft isa CATPart { myPart isa Part { PartBody isa BodyFeature { Sketch isa Sketch.1 {} S0 isa Shaft("Sketch") { StartAngle = 20 deg ; EndAngle = 300 deg ; } } } }
Shell
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Definition:
A shell is a hollowed out feature.
Attributes:
A shell is defined by the following attributes: • • DefaultInsideThickness. The syntax to be used is DefaultInsideThickness = 2mm. DefaultOutsideThickness: The syntax to be used is DefaultOutsideThickness = 1mm.
To specify a shell within your script, you must have a part open, then: 1. create a Shell by using the isa function Shell1 isa Shell ( ) { } 2. right-click anywhere inside the parentheses and select the 'Get Surface' function from the contextual menu. Then, in the geometry area, select the face to be hollowed out. A 1mm thick shell is created by default. MyBox isa CATPart { BoxPart isa Part { PartBody isa BodyFeature { Box1 isa Box { Width = 20.0 mm; Height = 25.0 mm; Length = 15.0 mm; } Shell1 isa Shell (face definition) { DefaultInsideThickness = 2mm; DefaultOutsideThickness = 1mm; } } } }
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SimpleHole
Definition:
A mechanical feature of Hole type you create when you click the icon in the Part Design workbench. For more information, refer to the Part Design User's Guide..
Attributes:
Hole1 isa CATPart { Part isa Part { PartBody isa BodyFeature { P isa Pad { } F isa SimpleHole("Use the Get Edge command to select the edge") { } } } }
Sphere
Definition:
A sphere is a shaft created by rotating half a circle around an axis passing through the arc extremities. The only property is the Radius.
Attributes:
A sphere is defined by the following attribute: • Radius. The syntax to be used is: Radius = 20.0 mm.
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MySphere isa CATPart { SpherePart isa Part { PartBody isa BodyFeature { Sphere1 isa Sphere { Radius = 20.0 mm ; } } } }
Tapered Hole
Definition:
A mechanical feature of Hole type you create when you click icon in the Part Design the workbench. For more information, refer to the Part Design User's Guide.
Attributes
A tapered hole is defined by the following attribute: • TaperAngle:
Thickness
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Definition:
A thick
Attributes
A thickness is defined by the following attribute: • DefaultThickness:
ThickSurface
Definition:
A thicksurface is a surface to which material was added in two opposite directions.
Attributes:
A thicksurface is defined by the following attributes: • • TopOffset, the thickness in one direction. The syntax to be used is TopOffset = 0.5mm. the BotOffset, the thickness in the one direction. The syntax to be used is BotOffset = 10 mm.
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myThickSurface isa CATPart { myPart isa Part { OpenBody1 isa OpenBodyFeature { P1 isa GSMPoint { PointType = 0; TypeObject isa GSMPointCoord { X = 0mm; Y = 0mm; Z = 0mm; } } C isa GSMCircle { CircleType = 0; TypeObject isa GSMCircleCtrRad { Center = object : .. object : .. .. .. .. P1; Support = `xy-plane`; Radius = } StartAngle = EndAngle = } Fi isa GSMFill { Boundary = object : .. } } PartBody isa BodyFeature { Thick1 isa ThickSurface { TopOffset = 0.5mm; C;
150mm; 0deg; 360deg;
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BotOffset = 10 mm; Surface = object : .. } } } .. } OpenBody1 Fi;
Torus
Definition:
A torus is a shaft created by rotating a circular sketch around an axis.
Attributes:
A torus is defined by the following attributes: • • InnerRadius SectionRadius
BodyDoc isa CATPart { BodyPart isa Part { Body isa BodyFeature { // Create a sphere Sphere1 isa Sphere { Radius = 15.0 mm; } // Create a torus Torus1 isa Torus { InnerRadius = 20.0 mm ; SectionRadius = 10.0 mm ; } } } }
Part Shared Package
Fillet Object
Definition
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Describes the feature you create when you click the icon in the Part Design workbench. For more information, please refer to the Part Design User's Guide. It is defined by one property: • Radius
There are 3 different types of fillets: • ConstantEdgeFillet • • FaceFillet TriTangentFillet
Constant Edge Fillet Object
Definition
A fillet is a curved surface of a constant or variable radius that is tangent to, and that joins two surfaces. Together, these three surfaces form either an inside corner or an outside corner. Important Note: To specify a fillet within your script, you must have a part open, then: 1. Create a Fillet by using the isa keyword. Fillet1 isa ConstantEdgeFillet ( ) { } 2. Right-click anywhere inside the parentheses and select the 'Get Edge' or the 'Get Surface' function from the contextual menu. Then, in the geometry area, select the edge or the face to be filleted.
Example
Box1 isa CATPart { BoxPart isa Part { PartBody isa BodyFeature { Box1 isa Box { Width = 20.0 mm ; Height = 25.0 mm ; Length = 15.0 mm ; } // Use the Get Edge or Get Surface command // from the contextual menu to retrieve // the edge or face to be filleted
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Pattern
Definition
A pattern is a set of similar features repeated in the same part. Two types of patterns can be created with CATIA: the rectangular patterns and the circular patterns. At present, only rectangular patterns can be generated from a script. A rectangular pattern is defined by the following properties: • Nb1, the number of elements to be replicated along the first direction • • • • Nb2, the number of elements to be replicated along the second direction Step1, the element spacing along the first direction Step2, the element spacing along the second direction Activity.
Syntax
pattern1 isa pattern [Nb1,Nb2] of feature_to_be_repeated
Example
MyBox isa CATPart { BoxPart isa Part {
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PartBody isa BodyFeature { Box1 isa Box { Width = 20 mm ; Height = 20 mm ; Length = 20 mm ; }
// Use the Get Surface command from the // contextual menu to specify the hole // anchor Hole1 isa SimpleHole ("Face:(Brp:(Pad.1;2);None:();Cf9:())") { Diameter = 15 mm; } Pattern1 isa Pattern[3,4] of Hole1 { Step1 = 50 mm; Step2 = 50 mm; } } } }
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Standard Package
Old Types Names Old Attributes New Types Names Feature New Attributes Id Name Owner Color Layer Pick Show
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List Visualizable
GSD Shared Package
Types Names GSMAffinity Attributes AxisFirstDirection AxisOrigin AxisPlane Ratio
GSMAxisToAxis GSMRotate GSMScaling GSMSymetry GSMTransformation GSMTranslate Angle Axis Ratio Reference Reference Activity ToTransfor Direction Distance
GSD Package
Please find below a table listing the types contained in the GSD package: GSM3DCurveOffset GSMBlend GSMConic GSMCurve GSMCylinder GSMExtractContour GSMExtremumPolar GSMAssemble GSMBoundary GSMConnect GSMCurvePar GSMDirection GSMExtrapol GSMExtrude GSMAxisToAxis GSMCombine GSMCorner GSMCurveSmooth GSMExtract GSMExtremum GSMFill
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GSMFillet GSMHelix GSMLawDistProj GSMNear GSMReflectLine GSMSpine GSMSweep GSMSweepSegment GSMUnfold GSOJunction GSOVariableOffset
GSMFilletBiTangent GSMIntersect GSMLineCorner GSMOffset GSMRevol GSMSpiral GSMSweepCircle GSMSweepSketch GSMWSupport GSOSeatDiabolo GSOWrapCurve
GSMHealing GSMInverse GSMLoft GSMProject GSMSphere GSMSplit GSMSweepConic GSMTrim GSOBump GSPShapeMorphing GSOWrapSurface
GSMAssemble
Definition:
A GSMAssemble is an object which joins at least two surfaces or two curves. The surfaces or curves to be joined must be adjacent. See the Generative Shape Design User's Guide for more information.
Attributes:
Click here to open the GSMAssembleScript script file.
GSMCurve
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Definition:
A GSMCurve is an object generated by the Generative Shape Design product. You can create a corner by ) clicking the Corner icon ( in the Generative Shape Design workbench. Click here to open the GSMCurveScript script file.
GSMCurvePar
Definition:
An GSMCurvePar object is a Generative Shape Design parallel curve.
Attributes: A GSMCurvePar is defined by the following attributes: • • • • • • • • • • InvertLaw. Length1. Length2. Mode. Offset. Orientation. PassingPoint. Support. TMDeviation. Type.
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Click here to open the GSMCurveParScript script file.
GSMExtrude
Definition:
A surface created by extruding a profile along a given direction. You can create an extruded surface by clicking the Extrude ) in the Generative icon ( Shape Design workbench. Attributes: A GSMExtrude is defined by the following attributes: • • • • • Direction. Element1. Length1. Length2. Orientation.
Click here to open the GSMSplit script file.
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GSMFillet
Definition:
An GSMFillet object is curved surface of a constant or variable radius that is tangent to and joins two surfaces. Together these three surfaces form either an inner or outer corner. Attributes: A GSMFillet is defined by the following attributes: • • • Element1. Element2. Radius.
Click here to open the GSMFilletScript.CATGScript file.
GSMProject
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Definition:
A Generative Shape Design projection. See the Generative Shape Design User's Guide for more information.
Attributes: A GSMProject is defined by the following attributes: • • • • • • Direction. Normal which corresponds to the Projection type field in the Projection Definition dialog box ( Normal = 1 for an orthogonal projection - otherwise specify a direction, a GSMLine for example). SolutionType. TMDeviation. ToProject which corresponds to the Projected field in the Projection Definition dialog box. Support which corresponds to the Support field in the Projection Definition dialog box.
Click here to open the GSMSplit script file.
GSMSplit
Definition:
A surface or wireframe element that was split by means of a cutting element. You can split: • a wireframe element by a point, another wireframe element or a surface a surface by a
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wireframe element or another surface. You can split geometry by ) in clicking the Split icon ( the Generative Shape Design workbench. Click here to open the GSMSplit script file.
GSMSweepSegment
Definition:
Attributes: A GSMSweepSegment is defined by the following attributes: • • • • • • • Angle. GuideCrv. GuideSurf. Length. Length1. Length2. Spine.
Click here to open the GMSweepSegmentScript file.
Knowledge Expert Package
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knowledgewareAdvisor Please find below a table listing the types contained in the Knowledge Expert package: KWECheck KWEGenericRuleBaseComponent KWERule KWERuleBaseComponent
KWERuleBase KWERuleSet
KWECheck
Definition:
Expert Checks are features generated by the Knowledge Expert product. Checks are regrouped into rule sets. Rule sets belong to a rule base. When writing a script with checks you must comply with the Rule Base/Rule Set hierarchy. Refer to the Knowledge Expert User's Guide for more information on the concepts behind the expert rules and checks. Click here to open the KnowledgeExpertScript file.
KWERule
Definition:
Expert Rules are features generated by the Knowledge Expert product. Rules are regrouped into rule sets. Rule sets belong to a rule base. When writing a script with rules you must comply with the Rule Base/Rule Set hierarchy. Refer to the Knowledge Expert User's Guide for more information on the concepts behind the expert rules and checks.
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Click here to open the KnowledgeExpertScript file.
KWERuleBase
Definition:
Rule bases are features generated by the Knowledge Expert product. Refer to the Knowledge Expert User's Guide for more information on the concepts behind this type of feature. Click here to open the KnowledgeExpertScript file.
KWERuleSet
Definition:
Rule sets are features generated by the Knowledge Expert product. Refer to the Knowledge Expert User's Guide for more information on the concepts behind this type of feature. Click here to open the KnowledgeExpertScript file.
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Mechanical Modeler Package
Some types and attributes were changed. Please find below a conversion table listing the old types, their attributes, their new names (if any) as well as their attributes: BodyFeature MechanicalFeature OpenBodyFeature GeometryFeature OpenBodyFeature
BodyFeature
Definition:
A body is the combination of several features within a part. For more information, see the Part Design User's Guide.
BodyDoc isa CATPart { BodyPart isa Part { Body isa BodyFeature { // Create a sphere Sphere1 isa Sphere { Radius = 15.0 mm; } // Create a torus Torus1 isa Torus { InnerRadius = 20.0 mm ; SectionRadius = 10.0 mm ; } } } }
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Workbench Description
Workbench Description
This section contains the description of the icons and menus specific to the Knowledge Advisor workbench. The Knowledge Advisor workbench is shown below. Click the sensitive areas (toolbars) to access the related documentation.
Knowledge Advisor Menu Bar Knowledge Toolbar Reactive Features Toolbar Control Features Toolbar Organize Knowledge Toolbar Actions Toolbar Tools Toolbar Set of Equations Toolbar
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Toolbars
Knowledge Toolbar
The Knowledge toolbar contains the following tools
See Creating a Parameter and Creating a Formula. See Associating URLs and Comments with Parameters or Relations. See Creating a Design Table from Current Values and Creating a Design Table from a Pre-Existing File. See Creating a Law. See Using the Knowledge Inspector. See Using the Equivalent Dimensions Feature. See Locking and Unlocking a Parameter.
Reactive Features Toolbar
The Reactive Features Toolbar contains the following tools:
See Creating a Rule. See Creating a Check. See Creating a Reaction: DragAndDrop Event.
Organize Knowledge Toolbar
The Organize Knowledge Toolbar contains the following tools:
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Workbench Description
See Creating Sets of Parameters. See Creating Sets of Relations. See Adding a Parameter to a Feature. See Adding a Parameter to an Edge. See Associating URLs and Comments with Parameters or Relations.
Control Features Toolbar
The Control Features Toolbar contains the following tools:
Here is a brief description of each icon. See Creating a List. See Creating a Loop.
Actions Toolbar
The Control Features Toolbar contains the following tools:
See Launching a VB macro with Argument. See Using the Knowledge Advisor Action Feature.
Tools Toolbar
The Tools Toolbar contains the following tools: 293
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See Updating Relations Using Measures. Select the Update icon to update a document without exiting the Knowledge Advisor workbench.
Set of Equations Toolbar
The Tools Toolbar contains the following tools:
See Solving a Set of Equations.
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Customizing for Knowledge Advisor
Customizing
Before you start your first working session, you can customize the way you work to suit your habits. This type of customization is stored in permanent setting files: these settings will not be lost if you end your session 1. Select the Tools -> Options command. The Options dialog box is displayed. 2. Choose the General category in the left-hand box. 3. Click the Parameters and measure tab. The following tabs are displayed.
This tab lets you define: o o o the Knowledge settings the libraries you want to load the report settings
4. Two other tabs, located in the Infrastructure category, in the Part Infrastructure workbench, also interfere with Knowledgeware applications.
o o
General Display
5. Change these options according to your needs. 6. Click OK when done to validate your settings.
Knowledge
This page deals with these categories of options:
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knowledgewareAdvisor • • • • Parameter Tree View Parameter names Relations update in part context Design Tables
Parameter Tree View
There are 2 types of items that you can display in the specification tree.
With value
Displays the parameter values in the specification tree. By default, this option is unchecked.
With formula
Displays the formulas constraining the parameter in the specification tree. By default, this option is unchecked.
Parameter names
This option should be checked if you work with non-Latin characters. If this option is unchecked, parameter names should have to be renamed in Latin characters when used in formulas. By default, this option is unchecked.
Relations update in part context
Before V5R12, Knowledge relations (formulas, rules, checks, design tables, and sets of equations) used to execute as soon as one of their inputs was modified. The user can now choose, when creating the relation, if it will be synchronous (i.e. the evaluation will be launched as soon as one of its parameters is modified) or 296
Project Standards asynchronous (i.e. the evaluation will be launched when the Part is updated). Each relation can therefore be synchronous or asynchronous. The 2 following options enable the user to create synchronous or asynchronous relations.
Creation of synchronous relations
Enables the user to create synchronous relations, that is to say relations that will be immediately updated if one of their parameters/inputs is modified. Relations based on parameters are the only one that can be synchronous. By default, this option is unchecked
Creation of relations evaluated during the global update
Enables the user to associate the evaluation of asynchronous relations with the global update. The relations can be asynchronous for 2 reasons: • • • • • The user wants the relations to be asynchronous The relation contains measures. Relations based on parameters: These relations can be synchronous or asynchronous. Relations based on geometry: These relations can only be asynchronous. Relations based on parameters and on geometry: For the part of the relations containing parameters, the user decides if he wants the update to be synchronous or not. For the other part of the relations, the update occurs when the global update is launched. Note that the user can also decide if already existing relations are synchronous or asynchronous. To know more, see Controlling Relations Update in the Infrastructure User's Guide. •
By default, this option is checked.
Design Tables
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There are 2 types of items that you can set up.
Automatic Synchronization at Load
When loading a model containing user design tables, if the design table files have been modified and the external file data is contained in the model, the design table will be synchronized automatically if this radio button is checked. By default, this option is checked.
Interactive Synchronization at Load
When loading a model containing user design tables whose external source file was deleted, this option enables the user to select a new source file or to save the data contained in the design tables in a new file. By default, this option is unchecked.
Manual Synchronization
When loading a model containing user design tables, if the design table files have been modified and the external file data is contained in the model, the design table will be synchronized if this radio button is checked. To synchronize both files, rightclick the design table in the specification tree and select the DesignTable object>Synchronize command or the Edit->Links command. By default, this option is unchecked.
Default Mode: Copy Data Into Model
If checked, the data contained in the external source file will be copied into the model. By default, this option is unchecked.
Default Mode: Do Not Copy Data Into Model
If checked, the data contained in the external source file will not be copied into the
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model. By default, this option is checked.
Language
This page deals with the following categories of options: • • Language Reference Directory for Types
Language
This field is to be used when using measures in relations or user functions. Measures are specific functions to be used in formulas and rules. The Knowledge Advisor User's Guide provides you with tasks explaining how to use measures. For how to create and use user functions, see the CATIA Application Architecture documentation.
Load extended language libraries
If checked, enables the user to select the packages he wants to load under Packages (if he wants to load a limited number of packages.)
This option is particularly useful for the administrator to limit the number of packages used by the user. It is also very useful to improve performances since only the required libraries are loaded.
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•
When you open a document and some relations are broken, you might need to load all libraries to solve the error, which may take quite a long time. It is strongly recommended to identify the packages you will need and to select them.
•
By default, this option is unchecked.
All packages
Enables the user to select all packages.
Reference Directory For Types
Reference Directory For Types
Enables the user to save the CATGScript file in the Directory indicated in the Reference Directory for Types field for later re-user (To know more, see the PKT User's Guide). By default, this option is not available.
Report Generation
This page explains how to customize the reports generated by the Global Check Analysis tool in the Knowledge Advisor and Knowledge Expert workbenches. It deals with the following categories of options: • • • • • Configuration of the Check Report Input XSL Report content Output directory HTML Options
Configuration of the Check Report
Html
Enables the user to generate a HTML report.
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Xml
Enables the user to generate a XML report. By default, the HTML option is enabled.
Input XSL
Note that this option is available only if the XML configuration setting is set.
Input XSL
Enables the user to select the XSL style sheet that will be applied to the generated XML report. The StyleSheet.xsl file is the default XSL file, but you can use your own template.
Report content
Failed Checks
If checked, the generated report will contain information about the failed checks only. By default, this option is unchecked.
All Checks
If checked, the generated report will contain information about all the checks contained in the document. By default, this option is checked.
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Check Advisor
If checked, the generated report will contain information about all the Knowledge Advisor checks contained in the document. By default, this option is checked.
Parameters information
Not available
Check Expert
If checked, the generated report will contain information about all the Knowledge Expert checks contained in the document. By default, this option is checked.
Passed objects
If checked, the generated report will contain information about the objects that passed the Expert checks as well as information about the parameters of these objects (diameter, depth, pitch,...). By default, this option is checked.
Objects information
Not available
Output directory
Output directory
Enables the user to select the output directory that will contain the generated report. By default, this option is available.
HTML Options
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Open HTML browser into CATIA Session
This option is available for Windows only. It enables the user to define if the report will be opened in a CATIA session (in this case, the check box should be checked) or if it will be opened in an Internet Explorer session (in this case, the check box should remain unchecked.) Note that it is highly recommended not to use this report as a basis for macros or for other applications. It is only provided for information purposes. By default, this option is checked.
Part Infrastructure for Knowledgeware Applications
This page deals with the options concerning: • • the external references: Keep link with selected object the specification tree display
Part Infrastructure General option
Keep link with selected object
You need to select this option to take advantage of the associativity. Click here to know more about the Part Infrastructure General options.
Part Infrastructure Display option
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knowledgewareAdvisor
Parameters
Select this option to display the parameters when working in a CATProduct context. By default, this option is unchecked.
Relations
Select this option to display the relations when working in a CATProduct context. By default, this option is unchecked. Click here to know more about the Part Infrastructure Display options.
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