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Catia v5 Tutorial Advanced - tworzenie konfiguracji (ang)

CATIA V5 Workbook
(Releases 8 & 9)


Richard Cozzens
Southern Utah University



Schroff Development Corporation

Lesson 1


Introduction To CATIA V5 Knowledgeware
This lesson is a little different than the lessons in the CATIA V5 Workbook because Knowledgeware is not one specific CATIA V5 workbench but several workbenches. Some of the tools can be accessed in the Standard tool bar in the Part Design Workbench. Simply put, Knowledgeware is a group of tools that allows you to create, manipulate and check your CATIA V5 creations.

Figure 1.1

Lesson 1 Objectives
This lesson will take you through the process of automating the creation of joggled extrusions as shown in Figure 1.1. At the end of the lesson you should be able to do the following: Create the Extrusion Profile Sketch and Joggle Profile Sketch. Assign variable names to the required constraints. Create the Joggled Extrusion.CATPart using the Rib tool.

1.2 -

Knowledgeware Create a spreadsheet with aluminum extrusion dimensions. Link the spreadsheet to the Joggled Extrusion.CATPart. Apply the spreadsheet to update the Joggled Extrusion.CATPart. Create a Macro. Modify the Marco using VB Script. Create prompt windows for input using VB Script. Check for company/industry standards using the Check tool. Implement the updated Joggled Extrusion.CATPart in a dimensioned drawing.

Figures 1.1 and 1.2 shows an example of the Joggled Extrusion you will create in this lesson. Figure 1.1 shows the standard Joggled Extrusion along with its Specification Tree. Figure 1.2 shows a spreadsheet with the resultant dimensioned drawing. Figure 1.2

Adding Intelligence


Knowledgeware Work Bench Tools And Tool Bars
A combination of six tool bars is used in this lesson from the Knowledgware Product. The Knowledgeware product is made up of the following work benches; Knowledge Advisor, Knowledge Expert, Product Engineering Optimizer, Product Item Optimization and Product Functional Definition. Each of these work benches have a different combinations of tools in each tool bar. If you switch between any of these work benches you may see the same tool in a different tool bar. For example the Formula and Design Table tool is accessible from many workbenches in the bottom tool bar.

The Set of Equations Tool Bar
This tool bar contains only one tool.

Tool Bar

Tool Name
Set of Equations

Tool Definition
This tool allows you to solve a set of equations.

The Knowledge Advisor Tools In the Standard Tool Bar
This tool bar contains 5 tools.

Tool Bar

Tool Name
Formula Comment and URL… Check Design Table Knowledge Inspector

Tool Definition
This tool allows you to create parameters and determine the relationship between parameters.
This tool allows you to add URLs to user parameters. This tool signals when there has been a violation in a check and/or rule.

This tool allows you to create and/or import design tables (spreadsheets). This tool allows you to query a design to determine and preview the results of new parameters.



The Reactive Features Tool Bar
This tool bar has four tools, the first one has been covered previously.

Tool Bar

Tool Name
Rule Editor Check Reactions

Tool Definition
This tool allows you to create a rule and apply it to your document. This tool allows you to create a check and apply it to your document. This tool allows you to create a script that will change feature attributes.

The Tools Tool Bar
This tool bar has two tools.

Tool Bar

Tool Name
Measure Update Update

Tool Definition
This tool allows you to update relationships. This tool allows you to update the CATPart and/or CATProduct.

The Actions Tool Bar
This tool bar has two tools.

Tool Bar

Tool Name
Macro With Arguments Actions

Tool Definition
This tool allows you to open a macro with arguments. This tool allows you to create a script.

Adding Intelligence


The Organise Knowledge Tool Bar
This tool bar has four tools.

Tool Bar

Tool Name
Add Set Of Parameters Add Set Of Relations Parameters Explorer Comment & URLs

Tool Definition
This tool allows you to create a set of parameters. This tool allows you to create a set of relations. This tool allows you to add new parameters to a feature. This tool allows you to add URLs to the user parameters.



The Problem:
One of the many Metalcraft Technologies Inc. fabrication processes is fabricating a joggle in standard and non-standard extrusions. Most of the extrusion requirements are contained in large assembly mylar sheets. Most of the drawings (mylars) were created in the early 1970’s. It is difficult for the engineer/planner to read and/or measure the mylar accurately. It may take the engineer/planner 10 to 30 minutes to verify he/she has found and applied the correct dimensions. It is not productive for the fabricator to also have to go through the same time consuming process. Having the drawing interpreted so many times by so many different people will inevitably introduce more chances for error. It is MTI’s (Metalcraft Technologies, Inc.) policy that the engineer/planner creates an individual drawing for each joggled extrusion to avoid such confusion. MTI has minimized the time required to create the individual drawings by setting up templates and standards. Yet, even with templates and standards this process is still time consuming. Each drawing is basically the same but has to be re-created because of a few simple dimensional differences and/or a different type of extrusion. The goal was to cut this time down by using the intelligence contained in the existing standard extrusion.

The Solution:
CATIA V5 Knowledgeware tools allow the user to capture and use the intelligence contained within the standard Joggled Extrusion.CATPart. CATIA V5 macro and scripting capabilities allow the user to be prompted for the critical dimensions. CATIA V5 then takes the information and updates the Joggled Extrusion.CATPart according to the supplied input. CATIA V5 also automatically updates the standard dimensioned drawing (CATDrawing). The dimensioned drawing is ready to be released to the production floor in a matter of minutes instead of 30 to 60 minutes. An additional advantage to this process is adding dimensional checks. If the dimensional values do not match the company and /or industry standards the user will get a warning. The following instructions will take you through the steps of creating the standard Joggled Extrusion.CATPart and then implementing the Knowledgeware solution described above.

Adding Intelligence


Steps To Implementing The Knowledgeware Solution
A parameterized sketch/solid is a basic form of Knowledgeware; it contains intelligence. Prior to parametric applications you would have to create each variation of the extrusion from scratch. Para metrics allow you to modify one constraint and the extrusion (solid) will update to that constraint.

1 Determine The Requirements
The general problem solving skills apply to implementing the Knowledgeware solution. You need to list all that is known and unknown and you need to list all of the variables, for example, what is known. If you are not sure at first, manually go through the process. You must be able to create the process manually.

2 Creating The Extrusion Profile Sketch
Create an Extrusion Profile Sketch on the ZX Plane as shown in Figure 1.3. The 0,0 point is located at the outside left corner of the extrusion. This sketch will be used as the standard; all other extrusions will be derived from this basic sketch. If you have problems or questions on how to create a similar sketch, refer back to Lesson 1 in the CATIA V5 Workbook. When you complete the sketch, exit the Sketcher Workbench but do not use the Pad Tool to create a solid. The solid will be created in Step 8 using a different tool.



Figure 1.3

3 Constraining The Extrusion Profile Sketch
After completing the rough sketch of the Extrusion Profile Sketch as shown in Figure 1.3 you must constrain it similar to the constrains shown in Figure 1.3. If you have problems or questions on how to constrain the sketch, refer back to Lesson 1 in the CATIA V5 Workbook.

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4 Modifying The Constraint Names
The lessons in the CATIA V5 Workbook did not require you to modify the names of the constraints. In this particular step it is critical that you rename the constraints. Understand that it is not absolutely necessary, but it will make this process a lot easier if you rename the constraints with a name that signifies what it is constraining. If you have problems remembering what the constraint name is, write it down; the names will be required to create the spreadsheet later in this lesson. It is suggested that you use the constraint names shown below so your information matches what you will see through the remaining steps to this lesson. Also, change the branch name Sketch.1 to Once you have successfully completed this lesson it is suggested that you try different variations of this process.

Figure 1.4

Offset Constraint = T2 Circle Constraint = R5 Circle Constraint = R1 Offset Constraint = B Circle Constraint = R4 Circle Constraint = R Offset Constraint = T1 Circle Constraint = R2 Offset Constraint = A Circle Constraint = R3



Figure 1.3 shows the constraints in the Specification Tree already renamed. CATIA V5 will automatically give it a name as shown in Figure 1.5 button. Figure 1.5 Constraint by selecting on line (length) Constraint between two entities (distance) Constraint between two entities (distance)

Constraint by selecting the radius

Complete the following steps to rename the constraints. 4.1 Double click on the constraint that you want to rename. This will bring up the Constraint Definition window with the constraint value in it. 4.2 Select the More button; this will bring up a Constraint Definition window as shown in Figure 1.6. 4.3 Edit the current constraint name in the Name box to what you want the new constraint to be named. 4.4 Select OK. The newly renamed constraint will show up in the Specification Tree. Figure 1.6

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5 Creating The Profile Sketch Of The Joggle
This Step, like Step 2, requires you to create another sketch. This sketch is created on the YZ Plane. Use the information in Figure 1.7 to create the Joggle Profile Sketch.

Figure 1.7

Offset Constraint = Transition Offset Constraint = Depth Distance Constraint (length) = Dist. To Endp. Distance Constraint (length) = Length.50

6 Constraining The Joggle Profile Sketch
Create constraints for the Joggle Profile Sketch similar to the ones shown in Figure 1.7.



7 Modifying the Constraint Names
Modify the constraint names you created in Step 6 to match the constraint names shown in Figure 1.7. Step 4 describes the process of renaming constraints. NOTE: It is important that the constraint names be consistent throughout this lesson. The names will be used to link the information to a table in the next few steps. If you deviate from the naming convention used in this lesson the remaining steps will not work as described.

8 Creating A Solid Of The Joggled Extrusion
Now that both sketches are created you are ready to create the solid. This will be accomplished by using the Rib tool found in the Part Design Work Bench. To create the solid complete the following Steps. 8.1 Select the Extrusion Profile Sketch created in Step 2. Make sure it is highlighted. 8.2 Select the Rib Tool found in the Part Design Work Bench. This will bring up the Rib Definition Window as shown in Figure X.8. The Prompt Zone will prompt you to “Define The Profile.” The Extrusion Profile will be listed in the Profile Box. 8.3 Select the Center Curve Box so it is highlighted, then select the Joggled Profile either from the geometry or the Specification Tree. CATIA V5 will give you a preview of the Extrusion Profile being extruded along lines that define the Joggled Profile Sketch.

Figure 1.8

Extrusion Profile Sketch

Joggled Profile Sketch

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8.4 If the preview looks similar to the joggled extrusion shown in Figure X.1 select the OK button to complete the operation. The Joggled Extrusion will be made into a solid.

Now that you have a solid created “Joggled Extrusion” you are ready to go on to the next step, creating a table of different types of extrusions.

9 Creating An Extrusion Table
Figure X.9 is an Excel (spread Sheet) that contains the dimensions to four different types Aluminum Extrusions. The extrusions and their dimensions were taken from the Tierany Metals Catalog. You might recognize the extrusion on row 5; it is the one you created in the previous steps. If you wanted to create the extrusion in row 2 you would have to start from step one again or you could go back to the Extrusion Profile Sketch and revise the constraints. Obviously revising the constraints would be the quickest and easiest method to creating the new extrusion. CATIA V5 Knowledgeware tools can make this process even quicker and easier. This is accomplished by linking the Excel File to the CATPart. You can use an existing spreadsheet if it is available. If it is not available you will have to create your own. The spreadsheet does not have to be in the Excel program, any spreadsheet program will work. Each column requires a header. The header will be used as a variable link later in the lesson. Notice the column headers used in Figure X.9 match the constraint names used in the previous steps to create the Extrusion Profile Sketch. This is not absolutely necessary but it does make the linking process much more intuitive. Figure 1.9

To complete this step go into the spreadsheet program of your choice and enter the information in as shown in Figure X.9. Save the file preferably in the same directory that your CATPart file exists. Remember the file name and where it exists, you will need that information in the following step.



10 Importing The Extrusion Table
CATIA V5 allows you to create a design table inside CATIA V5 or import an existing design table. This step will show you how to import the design table create in Step 7. As you go through the process of importing a design table you will be able to observe how CATIA V5 allows you the opportunity to create and modify a design table inside of CATIA V5. To Import a design table complete the following steps. 10.1 In the Part Design Workbench double click on the Design Table tool. The Design Table Tool is located in the Standard Tool Bar at the bottom of the CATIA V5 screen. The Design Table tool icon is shown in Figure X.10. This will bring up the Creation Of A Design Table Window as shown in Figure X.11. Name the Design Table “Extrusion Table,” using the Name Box shown in Figure X.11. Figure 1.11

10.2 Figure 1.10


The Comment Box will automatically place the date of creation. You can modify this box to any text that might help. This is just a comment box and will not have any effect on the following steps. Select the “Create a Design Table From A Pre-Existing File.” Although you will not use the other choice in this lesson it is important that you know that the other choice is available. The other choice is “Create A Design Table With Current Parameter Values.” This choice allows you to create a Design Table inside CATIA V5.


Adding Intelligence 10.5 Select the OK Button. This will bring up Browser Window labeled “Select The Design Table File.” This is the standard Windows File Browser. Reference Figure X.12.



Select the Directory and the file that you want to import in the “Select The Design Table File” Window. For this step you will want to select the “Extrusion Table” created in Step 9, as shown in Figure X.12. Select the OPEN Button. This will bring up an Automatic Association window as shown in Figure X.12. The prompt window asks if you want to automatically associate the parameters. Select Yes. This will bring up the Design Table. Active Window as shown in Figure X.13. Note that Figure X13 is shown with the Associations Tab selected not the Configurations Tab. If there are no Associations listed in the Configurations Box CATIA V5 was not able to automatically associate any of the Constraints Parameters and Extrusion Table Columns Headings.



Figure 1.12


When CATIA V5 is not able to automatically associate the two together you will have to manually associate them. To manually associate them select the Associations Tab in the Extrusion Table Active Window as shown in Figure X13.


Knowledgeware 10.10 The Parameters Box lists all the parameters CATIA V5 created in the Extrusion Profile Sketch. A CATIA V5 sketch contains a lot of parameters that the users are not usually aware of. What makes it more difficult is the CATIA V5 naming convention. It is difficult to identify a CATIA V5 Parameter listed in this box to an actual parameter in Extrusion Profile Sketch. This is where renaming the Constraints in the previous steps will prove to be beneficial. You should be able to scroll through the Parameters Box and identify the constraints you renamed. All the Parameters are represented on two separate lines. For this lesson you will use the line that ends with a type of measurement such as Radius, Offset or Length. You will not use the line ending in “Activity.” For this step scroll through the Parameters list verify the Constraints you renamed in Step 4 are listed.

Figure 1.13

10.11 Select “A” from the Columns Box. 10.12 From the Parameters Box find and select the line “…PartBody/\Extrusion Profile\A\ Offset.”

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10.13 Select the Associate Button. Your two selections from the Parameter and Columns Boxes will show up in the “Associations Between Parameters and Columns Box.” This means that they were successfully associated. 10.14 Continue this process until all the variables in the Columns Box except for “Extrusion Number” is matched up to the appropriate Parameter. 10.15 Now you can take care of the Extrusion Number Column heading. The Extrusion Profile Sketch has no associative value to the Extrusion Number that was created in the Extrusion Table. You can assign it one by selecting the Extrusion Number in the Column Box. 10.16 Select the Create Parameters… Button. This will bring up the “Ok Creates Parameters For Selected Lines” Window as shown in Figure X.14. Figure 1.14

10.17 Select the “Extrusion Number” in the Name Box and then the “String” in the Type Box. 10.18 Select the OK Button. This will create an association of a string type to the “Extrusion Number” Heading. The association will be displayed in the Extrusion Table Active Window under the Association Tab along with all the other Associations you created in this step. What this really does for you is allows the Specification Tree to show the Extrusion Number. Figure X.1 under the Parameters Branch displays the ‘Extrusion Number’ =60-10677. The string of numbers “60-10677” is linked from the specific row in the Extrusion Table. If you select another row (Extrusion) from the Extrusion Table the Specification Tree will reflect the change just as the solid does. NOTE: In order for the Parameters to show up in the Specification Tree you must have the Options set correctly. Step 13 will show you how to set the correct options.


Knowledgeware 10.19 Select the Configurations Tab in the Extrusion Table Active Window. If you correctly associated the Parameters and Columns it should look similar to the table shown in Figure X.15. If your Window looks similar to the one shown in Figure X.15 select the OK Button to complete the association process. 10.20 The will make the window disappear and the Extrusion Table.1 shows up on your Relations Branch of the Specification Tree. You may wonder what else is different. What did you just accomplish? Step 11 will show you the advantages of what you just accomplished.

11 Applying The Extrusion Table To The Joggled Extrusion
The purpose for linking a design table to then CATPart file is to update the part without having to redraw and/or revise the constraints manually. To test this, complete the following steps. Figure 1.15


Double click on the ExtrusionTable Branch of the Specification Tree. This will bring up the ExtrustionTable window as shown in Figure X.15. The data in row 4 is currently the active row. There are several methods to tell which row of data is active.

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a.) The window label contains the information, it has “ExtrusionTable active, configuration row: 4.” b.) Line <4> has brackets around it. The inactive lines do not have the brackets around it. c.) One other method is to check the data against actual Extrusion dimensions. Figure X.1 and the entire figure in the previous steps represent the data that is contained in row 4. 11.2 To make row 3, Extrusion Number 60-13028 active select the row. The existing extrusion will turn red signifying it needs to be updated. Select the OK button. This will update your active extrusion to the data contained in row 4. Figure X16 shows the row 3 extrusion. Compare the differences between the extrusion represented in Figure X.1 and X.16. Verify the extrusions with the dimensions in the ExtrusionTable (design table).


NOTE: If your extrusion does not automatically update you will have to select the Update button in the Standard Tool Bar section to force the solid to update. If you want CATIA V5 to automatically update select Tools, Options, Mechanical Design Branch, Part Design Branch, General Tab, Update Section and select the Automatic Button. Once you link your Design Table to your CATPart updating is quite simple. Click on the Design Table in the Specification Tree to bring the design table up. Select the row of data you want to apply to the CATPart and select OK.

1.20 Figure 1.16