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Routing MEP Systems
Table Of Contents
Preface ......................................................................................................... 1 What's New? ................................................................................................. 3 New Functionality ........................................................................................ 3 Enhanced Functionality ................................................................................ 3 Using This Guide ............................................................................................ 5 Getting Started.............................................................................................. 7 Setting up the Environment .......................................................................... 7 Routing a Run............................................................................................. 9 Routing Runs in a controlled environment ......................................................14 Placing Parts on a Run ................................................................................18 Saving Documents .....................................................................................18 Basic Tasks ..................................................................................................21 Managing Systems .....................................................................................21 Creating a System Assembly .....................................................................21 Creating a Logical Assembly ......................................................................22 Creating a Logical Set ..............................................................................23 Creating a Path Reservation ......................................................................24 Routing Runs .............................................................................................29 Routing Runs ..........................................................................................29 Routing from the End of a Routable............................................................35 Routing from an Item Reservation..............................................................36 Auto-route Between Equipment .................................................................37 Routing a Run Within a Pathway ................................................................38
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routingSystems Branching a Run ......................................................................................38 Modifying Runs ..........................................................................................39 Using the Definition Dialog Box..................................................................39 Moving or Deleting a Node ........................................................................41 Fixing Broken Routables ...........................................................................44 Connecting Routables...............................................................................46 Disconnecting Routables ...........................................................................48 Break a Run at a Branch ...........................................................................49 Placing Parts..............................................................................................52 Placing Parts in a CATProduct Drawing........................................................52 Detecting Clash in Parts Placement ............................................................56 Creating a Parent-Child Relationship...........................................................57 Using Quick Translate to Move Objects .......................................................59 Layout Tools ..............................................................................................60 Making an Element Active .........................................................................60 Using the Step Input Box and Construction Elements ....................................61 Using Offset Planes and Advanced Offset Planes...........................................63 Flipping Elements ....................................................................................65 Advanced Tasks ............................................................................................67 Advanced Routing Tasks..............................................................................67 Routing a Run at a Slope ..........................................................................67 Routing in 3D with the Compass ................................................................67 Edgeline: Routing Parallel to a Run.............................................................68 Aligning a Run to an Existing Surface .........................................................70 Routing at an Offset of a Routable..............................................................71
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Table Of Contents Routing Along a Spline .............................................................................72 Routing with Defined Nodes ......................................................................73 Advanced Layout Tasks ...............................................................................74 Snapping Elements ..................................................................................74 Mirroring Elements ..................................................................................83 Aligning Elements ....................................................................................85 Distributing Elements ...............................................................................87 Rearranging the Specifications Tree ...........................................................89 Changing the Current Axis ........................................................................91 Disabling/Enabling Manipulation Handles.....................................................92 Generating Detail Information ...................................................................93 Editing Parts ..............................................................................................94 Changing the Reference File for a Part ........................................................94 Change the Parameters of a Part ...............................................................95 Creating and Modifying Connectors ...............................................................97 Create Connectors ...................................................................................97 Using the Compass to Manipulate Connectors ............................................103 Modifying or Deleting Connectors .............................................................103 Creating Duplicate Connectors.................................................................104 Using the Plane Manipulator ....................................................................106 Working with Bendables ............................................................................107 Extracting Bending Data from Bendable Pipes and Tubes.............................107 Design Checks for Bendable Pipes and Tubes .............................................109 Transfer Elements to New Document...........................................................111 Workbench Description ................................................................................115
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routingSystems Workbench Description .............................................................................115 Toolbars .................................................................................................116 Systems Routing Toolbar ........................................................................116 General Design Toolbar ..........................................................................117 Product Placement Toolbar......................................................................117 General Environment Toolbar ..................................................................118 Project Standards .......................................................................................121 Systems Routing Settings..........................................................................121 General Settings....................................................................................121 Display Settings ....................................................................................123 Design Criteria Settings ..........................................................................124 Working in Cache Mode ..........................................................................125 Customizing the Dictionary of User Types..................................................126 Saving a System Assembly or Logical Assembly as a Separate Document .........129 Creating a Catalog....................................................................................130 Creating Parts .......................................................................................130 Creating a Catalog .................................................................................138 Making a Catalog Accessible ....................................................................139 Catalog Keywords and Values..................................................................142
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Preface
The Systems Routing product enables you to create physical designs of HVAC systems, piping systems and other production systems. The main focus of the product is to provide capabilities for preliminary routing of these systems, but capabilities are also provided to evolve the preliminary routing to the detailed production routing. All of this is accomplished through a very simple and highly intuitive interface which combines traditional 2D layout paradigms with the 3D capabilities to allow you to build a full 3D digital representation of the production routing that capture the design intent within the project. The Systems Routing User's Guide has been designed to show you how to create production routing systems within the project. This book provides an overview of the product and illustrates specific design procedures to aid your system routing efforts. Using This Guide
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What's New?
New Functionality
You can transfer elements in a document to a new document or work package. The import node points command allows you to predefine the node points of a run in a document and route using that document.
Enhanced Functionality
Modifying or deleting connectors on the instance of a part is no longer allowed. You can only perform these tasks on a reference or unique part.
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Using This Guide
This book describes how to use the Systems Routing product. Before you read it, you should be familiar with basic concepts such as document windows, standard tool bars, and view tool bars. To get the most out of this guide, you should start with the tutorial in the Getting Started section. It demonstrates how to create some basic elements of a routing system in a hierarchical structure. The remaining sections of the book describe in detail the procedures for using all of the features of the Systems Routing.
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Getting Started
Setting up the Environment
This task explains the setup tasks involved to use the System Routing workbench. You will be perf following tasks: 1. Cache Mode settings 2. Making Catalogs accessible 3. Setting working units and Grid
1. Cache Mode: Deactivate the option 'Work with cache system'. To do this click Tools in the menu bar and In the dialog box that appears, select Project Center - Project - Cache Management. Uncheck the option Work with cache system. Restart the application for the change to take For more information, refer Working in Cache Mode.
2. Making catalogs accessible: Click Tools-Options, select General and then the Document tab. Select Other folders in the w click Configure.
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routingSystems In the Other Folders dialog box, double-click on the drive where the catalogs you want are located. This will display all directories in the drive. Navigate to the directory that contains the catalog(s), and click Add Tree.
Click OK to save the search order. For more information, refer to Catalog's User Guide.
3. Set Working Units and Grid: Select Tools - Options and expand the General node. Select Parameters and Measure then click the Units tab. Under Magnitudes, select Length and click the drop down arrow to set the unit of measure you will be using; Foot, Meter, etc.
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Getting Started
Now, scroll down the list in Magnitudes and select Area. Select the unit of measure you will be using for area. Note: This is normally consistent with the Length standard.
To set the Grid Step, under Tools - Options, select Engineering - System Routing and click on the General tab. Enter a value for the Grid Step field; for example, 1 ft. The grid step is the increment used for snapping (to grid). Imagine a grid placed over your workspace, consisting of squares. The value you enter in this field becomes the distance between the lines of each square. If you enter 1 ft, then, when routing, the run will extend by 1 ft at a time. Runs begin, end and turn at grid intersections (there are ways of overriding this). Similarly, when placing parts in free space (as opposed to on a run), they will place at grid intersections. Click the OK button to complete the customization of the working units.
The grid step setting will display in the General Environment toolbar at the bottom of the 3-D view change it in the toolbar during your session but the new value will only apply to your current sessi close the application and reopen it, the toolbar will again display the value in the General tab page These will be your default settings and will remain in effect until you change them.
Routing a Run
This tutorial will show you how to use space reservations and route simple runs. The tutorial is div parts. • Creating a network
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routingSystems • Using Space Reservation • Routing a Run
This task assumes the user has setup the environment as described in Setting up the Environmen Creating a network:
1. Start Digital Project and enter "System Routing" workbench. An empty CATProduct docume 2. Click on the Logical Assembly icon on the System Routing toolbar. 3. From the Logical Assembly window, select HVAC Assembly from the dropdown menu. The Assembly system is added to the specification tree.
The Systems and Logical assemblies allow the user in organizing and grouping logical lines. For m information refer Managing Systems. Using Space Reservation: 4. Activate the HVAC Assembly just created by double clicking it in the specification tree.
and browse to the MechanicalSystems.Catalog located 5. Click the Catalog Browser icon $(PrjStdsInsDir)/startup/Catalogs/Systems Routing/, where $(PrjStdsInsDir) = Installation directory of the Project Standards. 6. Select the SpaceReservation object from the Spatial Objects chapter.
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Getting Started
The SpaceReservation object allows you to place a representative model for various equipments a in routing systems. You can place multiple copies of this object to represent the mechanical equip 7. Place one object in space as seen in the image below. You can change the parameters of th SpaceReservation object to customize it to represent different units in the system. (Use the Edit part parameters command to modify the parameters - Refer Edit Part Parame
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routingSystems Routing a Run:
8. Click the Run button The Run dialog box is displayed.
9. From the Type dropdown, select a Hydraulic run. Click on the Section to modify the section Select a Rectangular section and 'Center Center' as the Set Point. Modify the Envelope dim want to. Click OK on the Section dialog box to return to the graphic window. Do not click OK on the box yet. For detailed information, refer Routing Runs.
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Getting Started
10. Move the pointer over the face of the SpaceReservation from which you want to route. Wh arrow appears, click and begin to route.
11. Click in free space to continue creating the run. Click once to define the ending point of a s can change the direction of the run after you click in free space. Click twice to end the run.
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12. Click OK in the Run dialog box to create the run.
The green arrows are the Connectors, used to create logical connections between various objects SpaceReservation object and other parts) used in system routing. For more information, refer Man Connectors.
You have created a HVAC network with one run. You can now create additional runs using the same steps described above (Steps 8-12), or you can go on to the task of placing parts on the run.
Routing Runs in a controlled environment
14
Getting Started
This tutorial will show you how to use VirtualSupports and route runs constrained to the environme controlled environment - floor of a house, for instance. In such a practical project you will have to the run will have to be of certain size and shape. In the example below we will use a sample mode environment. The steps involved in this task are: • Placing a VirtualSupport • Constraining the VirtualSupport • Routing a Run
This task assumes the user has setup the environment as described in Setting up the Environment Routing Runs tutorial in the getting started guide. Placing VirtualSupport:
1. Open the sample model file MEPProduct.CATProduct 2. Two SpaceReservations have been placed in the basement of the model. The goal is to rout basement.
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3. Click the Catalog Browser icon and browse to the MechanicalSystems.Catalog located i Routing/, where $(PrjStdsInsDir) = Installation directory of the Project Standards. 4. Select the VirtualSupport object from the Spatial Objects chapter.
The VirtualSupport object allows you to place constraint points for routing ducts and pipes. The me VirtualSupports to the given environment and route runs through them. These VirtualSupports hav runs through them.
5. Place a VirtualSupport approximately in between the two columns as seen in the image belo
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Getting Started
Constraining the VirtualSupport: 6. Switch to Project workbench. Activate the Constraints toolbar if it is not visible by right clic Constraints toolbar from the contextual menu.
icon on the constraints toolbar. 7. Apply Offset constraint by clicking the 8. Select the vertical plane of the VirtualSupport and the face of the column marked with num 9. Again use the Offset constraint command and select the horizontal plane of the VirtualSupp distance to -1000mm. Change the sign if the support moves below the floor.
Side View Routing Run:
10. Click the Run button . The Run dialog box is displayed. 11. Move the pointer over the face of the AHU_Center unit in the model and select the connecto VirtualSupport. The routing begins. Click on the green arrow of the VirtualSupport pointing to end on the front face of the other AHU by clicking on the green arrow as seen in the ima 12. Click OK to create the duct.
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Thus you have created a duct in a controlled environment. You can later modify the location of the environment, and the duct routing will be updated. More Control can be obtained by placing number of VirtualSupports and constraining them with the
The next task explains you how to place the various mechanical parts and equipments for draw finalized.
Placing Parts on a Run
Now that you have a conveyor run in your network, you can add conveyor parts to the run. 1. Click the Catalog Browser button . 2. Navigate to the Systems Routing/Conveyor directory. 3. Place your parts. See Placing Parts in a CATProduct Drawing for more information on using the Catalog Browser.
Saving Documents
This task contains recommendations on saving your documents.
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Getting Started Ways in which documents are saved are explained in the Infrastructure User's Guide - Creating, Opening and Saving Documents. You must read that documentation because the various methods are not explained here. This task simply suggests the methodology you should follow in specific circumstances. 1. If you are saving a document to a local machine or network drive it is recommended that you use the "Save Management" command initially. The Propagate Directory command (which is in the Save Management dialog box) should not be used routinely. It is meant to be used in specific circumstances, such as when you want to place all the contents of a document in one directory before sending it to another location. 2. If you are saving a document to another site or network you should use the "Send To" command. In this case, you should be careful about the links for documents such as resolved parts folder or line ID. These links could change to reflect the local network drive to which the documents have been sent. You should make sure they point to the original location - using the Reset button in the Save Management dialog box is one way of doing this. 3. You should check the active document before you execute the Save command . The root product must be the active document if you want to save everything under it.
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Basic Tasks
Managing Systems
Creating a System Assembly
This task describes how to create a distribution system. A system assembly is a mechanism for organizing and grouping logical lines. You can create logical lines (such as a Piping Line or HVAC Network) under a system assembly, a logical set under a logical line, and then create runs under them. A system assembly, logical line and logical set will only display in the specifications tree because they are organizational elements. A run will also display in your viewer. In the illustration below, the specifications tree shows a piping system assembly under an area, a logical line (Piping Assembly1) under the piping system assembly, and a run (Pipe Run1) under the logical line. The run can be seen in the area.
1. Click on the System Assembly button. The System Assembly Creation dialog box is displayed. If you want to create the system in a new document see Saving a system assembly or Logical Line as a Separate Document. 2. Click on the down arrow and make a selection in the pull-down menu if you want to designate your system assembly as being of a certain type, i.e. conveyor, piping, power, etc.
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3.
Click OK. If the assembly is not visible in the specification tree, refer Display Settings.
Creating a Logical Assembly
This task describes how to create a logical assembly. A logical assembly is a mechanism used to group runs together. For instance, if you want to organize six runs together you can create a logical assembly and then create the runs under the logical assembly. A logical assembly has a function similar to other lines such as piping and ducts (available under the same menu). A logical assembly is normally created under a system assembly. It can be created under an area if there is no system. 1. Make the appropriate element active in the specifications tree. 2. Select the Logical Assembly icon .
The Logical Assembly Creation dialog box is displayed.
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Basic Tasks
. 3. Select the type of logical assembly you want to create.
4. Click OK.
Creating a Logical Set
This task shows you how to create a logical set. A logical set is a mechanism for organizing and grouping. You can create logical sets under a logical assembly (such as a Raceway Assembly) and then create runs under them. See Creating a System Assembly for more information. 1. Click on the Logical Set button. The Logical Set Creation dialog box is displayed.
2. Click on the down arrow to designate your network as being of a certain
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routingSystems type, i.e. work set. 3. Click OK.
Creating a Path Reservation
This task shows you how to create a path reservation on an area. 1. Make the appropriate area active. See Making an Element Active. 2. Click the Path Reservation button .
The Path Reservation dialog box displays.
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Basic Tasks 3. Define the type of path reservation you want to create.
4. Define the routing mode for the path reservation:
Point-to-point
Orthogonal
Slope
Directional Edgeline Branch at Center: see Branching a Path Reservation In addition, if you place the compass on an object the Use Compass Origin will display. If you click the button and start to route the route button will start from the compass origin. If you are in the middle of routing, the compass origin will serve as a routing point. Click one of the Select Mode buttons - the default is No Filter. The Select Mode buttons allow you to define where you can start routing from. No Filter: No filters are applied and you can route from any routable object or in space.
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In Space: Routing will be in space. This is useful when you have a large object in the background, such as a ship structure, and you want to be able to route in space. Only Part Connectors: Select this to be able to route from part or equipment connectors only. Import Node Points: This allows you to route using predefined node points. See Routing with Defined Nodes for more information.
5. To define Section parameters, do the following: a. Click the Section type button .
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Basic Tasks
The Section dialog box is displayed.
b. Define the section type and the corresponding parameters for each of them:
No Section Rectangular • • • • • Set Point Envelope height Envelope width Display Nominal size
Circular • • • • Set Point Envelope diameter Nominal size Display
Flat Oval. • • • • Set Point Envelope height Envelope width Display
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Radius Corner: Enter or select the: • • • • • Set Point Envelope Height Envelope Width Radius Corner Display
c. The Display buttons allow you to select a display mode of Line/Curve, Solid or Flat.
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Basic Tasks
d. Click the Display Centerline button to show the centerline of the run. This will appear as a dashed yellow line. In addition a dashed blue line will appear to display the Set Point setting. This feature works in all display modes, Line/Curve, Solid and Flat. e. Select OK on the Section dialog box. Instead of entering the type of path reservation, the set point and the height, width or diameter in the Section dialog box, you can select an existing path reservation in your document. Once you select the path reservation the Section dialog box will display the same values as the one you selected. To select, click on the Path Reservation button and then click the left mouse button once on the path reservation whose values you want as the default. Make sure the entire path reservation is selected, and not just one segment or node. It will be easier to select the path reservation in the specifications tree. 6. Optional. Key in a value for the turn radius. 7. Click in the drawing to define the routing points. 8. Double-click the last point to stop routing.
that shows at the beginning of the 9. Click on the Close Loop symbol routable if you want to create a closed loop routable. In a closed loop routable the ends of the routable are joined.
Routing Runs
Routing Runs
This task shows you how to create a run. You can begin routing a run from: • • • • • • Space. An object, such as a tube. The end of a run or middle of a run. A point. Connectors. SpaceReservation face.
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routingSystems 1. Click the Route a Run button The Run dialog box is displayed. .
Click on the down arrow and select the Type of the run. 2. Define the routing mode for the run:
Point-to-point: routing will be directly between two points indicated by clicking.
Orthogonal: routing between two points will proceed first in the X direction, then in the Y direction.
Slope routing: see Slope Routing.
Directional routing: see Routing with a Compass. Edgeline: see Edgeline Routing. Branch at Center: see Branching a Run.
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Basic Tasks
In addition, if you place the compass on an object the Use Compass Origin button will display. If you click the button and start to route the route will start from the compass origin. If you are in the middle of routing, the compass origin will serve as a routing point. Click one of the Select Mode buttons - the default is No Filter. No Filter: No filters are applied and you can route from any routable object or in space. In Space: Routing will be in space. This is useful when you have a large object in the background, such as a building structure, and you want to be able to route in space. Only Part Connectors: Select this to be able to route from part or equipment connectors only. 3. Define the Section parameters: a. Select the Section Type button. The Section dialog box is displayed.
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b. Define the section type and corresponding parameters for each of them:
No Section Rectangular. Enter or select the: • • • • • Set Point Envelope Height Envelope Width Nominal Size Display
Circular. Enter or select the: • • • • Set Point Envelope Diameter Nominal Size Display
Flat Oval: Enter or select the: • • • • • Set Point Envelope Height Envelope Width Nominal Size Display
Radius Corner: Enter or select the: • • • • • • Set Point Envelope Height Envelope Width Radius Corner Nominal Size Display
Double Ridge: Enter or select the: • • • • • Set Point Envelope Height Envelope Width Nominal Size Display
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Basic Tasks The Envelope field refers to the total work area needed.
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routingSystems
c. Select OK on the Section dialog box. The Display buttons allow you to select a display mode of Single, Double or Flat. Click the Display Centerline button to show the centerline of the run. This will appear as a dashed yellow line. In addition, a blue line will appear to display the Set Point setting. This feature works in the Single, Double and Flat display modes. Instead of entering the type of run, the set point and the height, width or diameter in the Section dialog box, you can select an existing run in your document. Once selected, the Section dialog box will display the values for that run. To select, click on the Run button and then click on the run whose values you want as the default. Make sure the entire run is selected - not just a segment or a node. It will be easier to select the run in the specifications tree. If you enter a minimum length or turn radius you will not be able to route correctly unless these values are satisfied. For instance, if you enter a minimum length of 10 feet, you will not be able to complete a segment that is 5 feet. In the illustration below, the green line shows the minimum segment length that will be created, even if you try to make a shorter segment, because the minimum length you entered is longer than the segment you are now trying to create. Similarly, if you enter a value for the turn radius, your run will automatically be adjusted to satisfy the defined turn radius.
6. Click in the drawing to define the routing points. 7 Double-click on the last point to stop routing. You can also click OK in the Run dialog box to stop routing. Click Cancel to abort your routing. 8. Click on the Close Loop symbol that shows at the beginning of the run if you want to create a closed loop run. In a closed loop run the ends of the run are joined.
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Basic Tasks
Routing from the End of a Routable
This task explains how to route from the end of a routable. If you route an element with the same type and parameter values as the "source" element (i.e., the element from which the routable is routed), you can specify whether the new element is a continuation of the source element or a separate element. If you want to use the "Continue" option, be sure that the parent for the source element is active before you begin. 1. Select the Route a Run button . The Routing dialog box is displayed.
2. Define the routing parameters. See Routing a Run for instructions.
3. Move the pointer to the end from which you want to route. When a green arrow appears, click and begin to route. Double click to end routing.
4. Once you begin routing the following buttons are added to the Routing dialog box:
Continue Routing: If you select this the run you create will be part of the run from which you are routing.
Create New Route: If you select this the run you create will be a new run. 5. When starting a run that is a continuation of an existing run, a branch from an existing run, or routing from an object or equipment (nozzle) use either or both of the following buttons as applicable: Get Size/Spec from Selection: If you select this button the run you create will be a new run but will assume the size and specification attributes
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routingSystems of the run or object you are routing from. Get Line ID from Selection: If you select this button the run you create will assume the same line ID as the run or object from which you are routing. If you de-select it, the new run will belong to the line ID displayed in the menu bar.
Routing from an Item Reservation
This task shows you how to route from an item reservation. Click the Route a Run button. 1. 2. Click on the face of the item reservation from which you want to route. 3. Begin routing.
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Basic Tasks The point on the item reservation face from which the run will start depends on the set point of the run. In the illustration above the set point is set at Center Center. If the set point was set at Bottom Center the run would have started at the bottom center edge of the item reservation. To change the set point, click button in the Run dialog box and select the Set Point on the Section Type from the drop down list in the Section dialog box that
displays.
Auto-route Between Equipment
This task shows you how to auto-route a run between two pieces of equipment or two connectors. 1. Make the appropriate element (area, system or line) active by doubleclicking in the specifications tree. 2. Place the two pieces of equipment you want to connect on your area. 3. Click on the Route a Run button and enter parameters in the dialog box that displays. 4. Move the cursor to the first equipment - an arrow displays at the connector point. If the equipment has more than one connector point the arrow will display at different points as you move your cursor.
5. Click to select the starting point of the run. 6. Move the cursor to the second equipment, where the arrow will also display, and click to select the ending point of the run. The run is created over the 37
routingSystems shortest possible path. 7. Press the shift key to see other possible routes for the run between the two objects.
Routing a Run Within a Pathway
This task shows you how to route a run within a pathway.
. The Run dialog bo 1. With your pathway model open, click the Route Thru a Pathway button 2. Click the Section button to open the Section dialog box. Select the type of run, the set point an
3. Click on the pathway in which you want to route your run. This displays set points on the pathw clicking on one of the points. For example, if you select Top Center the run will align to the top Apply in the Run dialog box to see how the run looks and to try different positions. Click OK wh
Branching a Run
This task explains how to branch a run from any of these elements: • • • Another run Boundary Contour
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Basic Tasks • Pathway
If the "source" element (i.e., the element from which the run branches) is moved or resized, the run is adjusted accordingly. 1.With your document open, select the Route a Run button. The Routing dialog box is displayed. 2.Define the parameters for the run. See Routing a Run for instructions. 3. Select the element from which you want to route the run and begin routing. 4. If you want to branch from the center of the segment, click the Branch at Center button in the Run dialog box. The branch will begin from the center of the segment, irrespective of the point in the segment that you route from. If you want to create a run that "branches" from the end of a run, see Routing from the End of a Routable.
Modifying Runs
Using the Definition Dialog Box
This task gives you an overview of the definition dialog box. You can make modifications to a routable using the functions contained in this box. Specific task-oriented modifications are explained elsewhere in this section. You should be familiar with the concepts explained in Routing a Run to be able to take full advantage of these functions. 1. Right click on a routable and, in the drop down menus that display, select the routable and then Definition.
2. This brings up the Definition dialog box.
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3. The Name field allows you to change the routable's instance name. 4. The Section button lets you change section parameters, as explained in Routing a Run. 5. Click one of the Turn Type buttons if you want to change the turn type. • • • 6. No Turn: The turn radius for all turns is changed to 0. The Turn Radius field is not displayed. Uniform Turn: All turns in the run have the same turn radius. Mixed Turn: Turns in the run can have different turn radius.
The Display Error Report button is green
when there is no error in the
run. It turns red when you insert a value or make some other change to cause an error. Click the button to display a report. This error function checks to make sure that the turn radius and minimum length conform to the design rule. 8. The Turn Radius field displays the turn radius. To change it you need to display the Node Definition dialog box (see Moving Nodes) and enter a value. If you introduce an invalid turn radius, by entering a value in the Node Definition dialog box, then the Display Error Report button will turn red. (You can also introduce a turn radius error by shortening the length of one or both segments.) A red arc will also display on your run. The ends of the arc are the minimum point to which each segment should be routed for a valid turn. In the example below, the segment is not long enough to support the turn radius value entered by the user.
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Basic Tasks
9. The Node Edit Table button displays a table containing node values - see Moving Nodes. 10. The Minimum Length field displays the minimum length of each segment. You cannot change the value in this field if you are using design rules. 11. The Total Length field displays the total length of the run. You cannot change the value in this field.
Moving or Deleting a Node
This task shows you how to move the nodes on a path reservation, boundary, or run. In the example below a node will be moved in a pipe run. 1. Place your mouse pointer over the element and click the right mouse button.
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routingSystems 2. From the menu that displays, select the Definition option. This will bring up the Definition dialog box. Symbols are displayed on the pipe run to show the location of nodes: asterisks represent non-connected nodes, and Os (circles) represent connected nodes.
3. To move a node by entering coordinates, do one of the following: • Right-click the node symbol and select Definition from the pop-up menu. The Node Definition dialog box displays.
OR Bring up the (run) Definition dialog box and click the Node Edit Table button to display the Node Edit Table and make changes to values in the table.
• •
Key in new values for X, Y, or Z. Click OK in the Node Definition dialog box.
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Basic Tasks 4.
To move the node using the cursor, place the cursor over the node symbol and drag it to a new location. A line is displayed to show the new location for the segment.
5. Click OK in the Definition dialog box to complete the change. A node will move parallel to the compass base plane, which is normally XY. To move a node vertical to the base, change the compass base to the XZ plane. 6. To move a node parallel to the compass Z axis. • • • Bring up the Definition box for the routable. Place the compass on a 3-D object where it can be manipulated. Change the Z axis to the desired direction. Click on the square around the node and move it with the mouse button depressed. It will only move parallel to the compass Z axis. If you click on the node itself you will be able to move it in any direction.
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routingSystems 7. To move a node of a routable to the origin of the compass. This allows you to move the compass to a specific point on a routable or resource, and then move the node to it. To do this: • • • • Bring up the Definition box for the routable which has the node you want to move. Move the compass to the point where you want the node to move. Bring up the Definition box for the node that will be moved. . The node will move to the Click the Compass Origin button compass base, as shown in the image.
8. To delete a node right-click on the node and select Delete Node from the pop-up menu that displays.
Fixing Broken Routables
This task shows you how to fix - or rejoin - routables in which segments have become separated. In the illustration below, the dotted line - the broken routable indicator - shows that a run has become separated at that point.
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Basic Tasks
You can re-join the run in one of several ways, depending on the nature of the break and your requirements. The methods are as follows: 1.Bring up the Definition dialog box for the run, then place the mouse pointer over the broken routable indicator and click the right mouse button. This will display a pop-up menu. Click Create Segment. 2.Bring up the Definition dialog box, then drag one of the segment handles to re-join the run. 3.Bring up the Definition dialog box. An arrow will display at each end of the broken routable indicator. Drag one of the arrows (depending on circumstances) to re-join the run. In the illustration below, one segment of the run has been moved to connect to the portion of the run still connected to the pump.
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4.In certain cases you will see the Auto Route option beneath the Create Segment option in the pop-up menu (See Step 1). This can happen when a segment connecting two parallel routables (on different X-Y planes) is broken. • Select Auto Route. The Auto Route dialog box will display.
• •
Click on the Toggle button. Options for re-joining the run will be shown as a dotted line. Click OK to make your selection.
Connecting Routables
This task shows you how to connect a routable to another routable. Routables are path reservations, space reservation, boundaries, or runs.
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Basic Tasks
There are two kinds of connections: branch and end-to-end. In a branch connection the end of one element connects to the middle of another. In an end-to-end connection two ends are connected together. In the examples below the two runs will be connected to each other, first as a branch and then as an end-to-end connection.
When you connect two elements one becomes the Employee and the other becomes the Manager. In the example above, if you make the run on the right the Employee and the one on the left the Manager, after you connect them, the Slave will follow the Manager to maintain the connection. The direct method to connect the routable is as follows: Click the Connect button and select one of the elements you want to connect. The element selected first will be the employee and will move to join the manager element. You must click on one of the connector indicators on the employee run. Select the manager element. The first run will move to connect to the manager and the connection symbol will display. Alternatively, you can follow these steps in particular scenarios. 1. Place the mouse pointer over the element you want to designate the Slave and click the right mouse button. 2. From the pull-down menu that displays, select the element you want to modify, in this case Run, and select the Connect Routes option.
3. Select the Master Connector. To select, move your mouse pointer over the run you wish to designate the Master and click on either the support or center line connector. See Information below.
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When you move the mouse pointer over the routable you will see two lines alternatively, as you move the pointer from bottom to top. The solid line is the support line connector, and the dashed line is the center line connector (illustrated below). The second routable will connect to whichever line you select. Select the line by clicking.
4. Select which end of the Slave you want to connect to the Master. The Slave will connect with the Master after you click.
The two elements will connect at the point where the two support or center lines would intersect. If you want to change the position, see Moving Nodes. 5. To make an end-to-end connection replace Step 3 above with the following: Select the Master Connector. To select, move your mouse pointer over the run you wish to designate the Master and click on the arrow that displays at whichever end you want to connect.
Disconnecting Routables
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Basic Tasks This task shows you how to disconnect a routable that is connected to another routable. Routables are path reservations, space reservations, boundaries or runs. 1. If it is a branch connection select the Slave element. If it is an end-to-end connection you can select either Master or Slave. 2. Right click on the element you selected. From the pull-down menu, select the element (XXX.object) you want to modify, in this case Raceway Run, and select the Definition option. The Definition dialog box is displayed, and a small, circular node symbol is displayed at the point where the two runs are connected.
3. Right-click the node symbol. A pop-up menu shows. Select Disconnect.
4. Click OK on the Definition dialog box. The two elements are disconnected. As an alternative, click the Disconnect button where the two runs are connected. , then click the connection symbol
Break a Run at a Branch
This task shows you how to break a run at a branch.
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routingSystems There may be times when you want to move all the segments of a connection at the same time. Breaking runs at branch intersections is one way. When you break runs at branch intersections you create what is called a star connection. In this type of connection (recognizable by a square or diamond-shaped symbol), all the segments joined at a connection will move if you move the connection. In a master-slave connection, the slave will maintain a connection with the master if you move the master. The illustrations below show 1) a run with a star connection; 2) the star connection is moved by dragging with the mouse; and 3) all nodes connected to the star connection move to the new star connection location in order to maintain that connection.
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Basic Tasks
1. Click on the Star Connection button. 2. Click on the routable, system or network you want to convert to star connection. A branch connection symbol connections in the selected element. will display at all branch
A pop-up panel will ask: OK to continue? Click Yes. The connection will be converted. The illustrations below show a branch connection converted to a star connection, with the diamond-shaped star connection showing.
The illustration on the left shows that the main section consists of one segment. But after conversion to a star connection it is broken at the
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routingSystems connection into two segments.
Placing Parts
Placing Parts in a CATProduct Drawing
1. Click on the Browser button. 2. Navigate to the catalog from which you want to select a part.
This task shows you how to place a part from a catalog into a CATProduct drawing. See also Detec
If you want to define a new search path then click Tools-Options, select General and then the Doc search order by clicking on Export, in which case they will stored in a file in a directory you spec
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Basic Tasks
3.
Double-click on directories , to navigate to the page containing the parts. Then double-click on a
4. Click at one or more locations to place the part. NOTE: To place a part, you can also select an e selected. 5.
The different scenarios are discussed: Placing Reducers (straight and branched): You can place reducers (straight and branched) dimension run to get correct orientation of the reducer.
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Placing Reducing Turns: Turns can be placed on runs oriented at 90 degrees. After the turn has connector of the smaller run to get correct orientation of the reducer.
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Basic Tasks
Placing Transitional Reducers: For the transitional reducers provided (round to Rectangular), pla Placing Valves: The same rules as those for straight reducers apply for valves.
Placing Equipments: Equipments will be placed at the end of runs. Some may replace the space
Sometimes the following message will display:
This means that there is more than one type of the selected part in the catalog. The difference ma wanted to place a tee that was 9.6 inches in diameter. If there are two tees in the catalog, one 9 i Part Parameters function. You may also use Flip Part Position if the orientation of the part is reversed.
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Some parts have restrictions attached to them that will not allow you to place them in certain loca
You can choose to display or hide a "preview" of the part you are placing. To do this select Tools obtain the effect you want.
By default, when you click (in free space) to place a part the center of that part will be placed at th to place the origin of the part at the point where you click. To do this click on Tools - Options, sele
No parts can be placed on the run itself. They must be placed either at the ends or at connections. • • To place a part inside an item reservation, press the shift key and click the mouse button. To place a part on a face of an item reservation, click the mouse button.
Detecting Clash in Parts Placement
This task shows how you can detect clashes between parts when you are moving parts in a document. This function only works when you are placing/moving parts in free space. It will not work if the parts have been placed on a run, for instance. Three modes are available: Clash Detection Off; Clash Detection On, and Clash Detection Stop. 1. To turn clash detection off click the Clash Detection (off) button . This is the default mode. 2. . To turn clash detection on click the Clash Detection (On) button When you move a part in such a way that it interferes with another part, a red outline will display, as in the images below. (If your part displays red highlights and you want to change the color you can do so by clicking Tools-Options-Display and selecting another color.)
3.
To change to the stop mode click the Clash Detection (Stop) button . When this mode is on you will not be able to move a part to a position in which it interferes with another part. In the first image below the pump
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Basic Tasks has been stopped because it interferes with the heat exchanger. However, when the user moves his pointer to the other side, and there is enough room for the pump, the pump will appear on the other side of the exchanger.
Creating a Parent-Child Relationship
This task shows you how to create a parent-child relationship between two elements. This function can be used to create a relationship between resources, between a resource and an element like an area; or between products in a process. The example below uses electrical parts and robots. The procedure is the same for all types of objects and elements. 1. Click the Attach button 2. Select the parent (or master) element. 3. Select the child (or slave) element. The attachment is created. If you move the child, the connection between the two will remain; however, unlike a master-slave relationship, the child element will not snap back to its original position. If you move the parent the child will follow.
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4. To hide all the Parent/Child symbols and text (attachments) in a product, click the Hide Attachment button, then click the Product in the specifications tree. All attachments in the product will disappear.
To hide individual attachments, click the Hide Attachment button, then click the object. The attachment will be hidden. If a local Attachment is selected, e.g., an attachment between two elements in a product, only that attachment is hidden or shown. If a Product is selected you not only Hide/Show all attachments of the selected product but also all attachments to the children of the selected product. If you open a product and don't know if there are existing attachments, click the Swap Visible Space button been hidden. to reveal any attachments that may have
5. To show all previously hidden attachments, click the Show Attachment button, then click the Product in the specifications tree. All attachments will be shown. To show a previously hidden "local" attachment, click the Show Attachment button, then click the object or select it in the specification tree. The attachment will be shown. 6. To delete an attachment select it and use the delete key.
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Basic Tasks
Using Quick Translate to Move Objects
This task shows you how to use the Quick Translate command to move elements. This function allows the user to transfer an element relative to a location on another element by any of the following alignment methods: • • • • • • Point-to-Point Point-to-Line Point-to-Plane Plane-to-Plane Plane-to-Point Line-to-Point
An object or element moved using this command does not rotate. 1. With your document open, click on the Quick Translate button . The Translate dialog box opens. Depending upon which From element you select the available To elements will either be grayed out or become active.
2. Select the type of transfer, Point-to-Point, Point-to-Plane, etc. Using the Point-to-Plane method as an example, select a point on the From element in your document and select a plane on the To element.
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3. The transfer occurs when you click on the To element. Click the Update button, if necessary. In this case, the object or element has moved, aligning the selected point with the selected plane.
4. The function works similarly with the other From/To selection methods and may be applied as the design dictates.
Layout Tools
Making an Element Active
This task shows you how to make an element in a drawing active. An element is active when it is highlighted in blue in the specification tree, as shown below.
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Basic Tasks
1.
You can make an element active by following any of these steps: • Double-click the element in the drawing or in the specification tree.
• • •
Select Activate Parent button parent active.
to make the active element's
and then To activate an area, select the Activate Area button select any element under the area. To activate a network, distribution system or logical set, select the Activate Network button the network. and then select any element under
2.
Optional. You can change the display of elements that arenot active using the Toggle Dimming Mode button on the General Environment Toolbar: When Dimming Mode is on, elements that are not active are dimmed. When Dimming Mode is off, inactive elements are not dimmed.
Using the Step Input Box and Construction Elements
This task shows you how to use the step input box and construction elements for more control over routing and placing of resources and item reservations. The value entered in the step input box is used for accurate routing and resource placement. You can only route in multiples of the value in the step input box. If the value is 0.25 meters you cannot create a run that is 0.33 meters in length, but you can create runs that are 0.50, 0.75 meters and so on. The value in the step input box works with some of the construction elements to further refine your routing and resource placement, as explained below.
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routingSystems 1. To enter a value in the step input box, select the increment field and key in a value. You can also click on the down arrow and select a value, if it is appropriate for your task. The following sections explain how the step input box is used together with some of the construction elements. 2. Click on the down arrow and select Snap to steps off current axis button. This allows you to snap to points that are multiples of the value entered in the step input box measured from the current axis (also called origin). As you move your mouse pointer a label will show the distances (coordinates) from the current axis in multiples of the value entered in the step input box. In the illustration below, the label is showing that the distance is 500 mm from the axis along the X axis, and 500 mm from the axis along the Y axis. When routing you will only be able to create segments whose length is in multiples of 500 mm. Similarly, you will only be able to place (or move) a resource at points that are measured in multiples of 500 mm from the axis. You can change the value in the step input box at any time.
3. Snap to steps off last position . This will allow you to snap to points that are multiples of the value in the step input box measured from the last point at which you clicked. When you select this option the label will first show the distances from the current axis. After you click, it will show the distances from the last point where you clicked. You can change the value in the step input box after a click if you want to route a segment of a certain length, or place a resource an exact distance away from where you last clicked. 4. . This option allows you to snap to the Snap to XY construction planes XY grids on a construction plane. You first create a grid using the Construction Planes command. If you have an XY grid you will only be able to place resources at, or route to, the intersections of X and Y grids. If you have only X or Y grids you will only be able to place resources at, or route to, the grid lines. 5. Snap to all construction planes snap to the X, Y or Z grids. 6. Snap to elevation planes . Selecting this option allows you to snap to the elevation planes of a Z grid. In the illustration below the user is routing on the Z axis and snapping to the elevation planes of the Z grid. . Choosing this option allows you to
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7. Snap to Drafting elements . This option is used when attaching the drafting view of a 2D drawing to an area. By using this option you will be able to snap to the elements of the 2D drawing. For instance, if you are attaching the 2D drawing of a conveyor belt to an area, by choosing this option you will be able to use the Conveyor Reservation function to select the drawing (you select by clicking on different elements of the drawing). This will allow creation of an identical conveyor layout in 3D.
Using Offset Planes and Advanced Offset Planes
This task shows you how to define a plane to use as a temporary reference for positioning other elements. The second part of the document explains the use of an advanced offset plane, which allows you to define origin, orientation and other parameters. 1. Select the Offset Plane icon . 2. Define the reference plane by doing the following: a. Place your cursor over a geometric element that defines the plane (e.g., a construction plane, boundary, area contour, item reservation). As you move the cursor, a small white rectangle is displayed to show the selectable planes, as shown below.
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If you do not see the white rectangle, zoom out from the drawing. The white rectangle cannot be displayed if the element under your cursor is displayed too small. b. Click to select the plane. The white rectangle changes to a blue rectangle, and remains displayed on the reference element, as shown below.
The reference plane can now be used as a reference to position other elements. 3. Use the advanced offset plane feature to set your plane reference, origin and orientation settings as follows: a. Click the Advanced Offset Plane button. The Define Plane dialog box will display.
b. The Define Plane button is selected by default. However, you can select any button in the
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Define Plane box. Click when you have found a location. The plane manipulator displays.
Click on the buttons in the Define Plane dialog box to make your selections. See Creating Connectors on using the buttons. c. Click OK when done. The reference plane will be created.
Flipping Elements
This task shows you how to flip a part that has been placed in a document. 1. 2. Click the Flip Part Position button. Select the part you want to flip. The part is flipped.
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Advanced Tasks
Advanced Routing Tasks
Routing a Run at a Slope
This task shows you how to route a run at a slope. 1. At the point in your run at which you want to slope it click the Slope button in the Run dialog box. 2. Enter the degrees of slope you want.
Click the Section button and enter data about the type and size of run. 4. Continue creating your run. Click once to define the ending point of a segment. Click twice to end the run.
3.
Routing in 3D with the Compass
This task shows you how to use the compass to route in any direction. Click the Route a Run button. 1. The Routing dialog box is displayed.
2. Click the Directional Routing button. Select the type of run and enter other values. See Routing a Run for more 3. details.
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routingSystems 4. Click at the point where you want to start your run from. This places the compass at that point.
To begin routing click and drag the compass so that its Z axis (it may read W) is pointing in the direction in which you want to route. To change direction, drag the Z (or W) axis of the compass, or press the Shift key repeatedly until the desired axis is highlighted.
5. Double click, or click OK to end your routing. You can also double click on the compass to bring up the Compass Manipulation dialog box, which allows you to enter values to modify compass direction and/or location.
Edgeline: Routing Parallel to a Run
This task shows you how to route parallel to, or at an offset of, a routable. See also Routing at an Offset of a Routable and Position Segment Relative to Plane. This function is used when you have an existing run and want to route parallel to it, or at a certain clearance from it. It is sometimes known as edgeline routing. You can also place an offset plane on a surface and use it as a reference point. 1. Display the run you want to route parallel to and click the Run button . The Run dialog box displays. 2. Click the Edgeline button . The Distance field will display and the Offset and Clearance buttons will appear in the Run dialog box.
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If you click the Offset button the distance between the two runs will be measured from centerline to centerline. If you click the Clearance button the distance between the two nearest edges will be measured. If there is a part on a piping or tubing line the distance will be measured from the part. If there is no part the distance will be measured from the line. 3. Enter the distance between the two runs. If you enter 0 and click the clearance button, the two runs will touch at the edges. 4. Click at the starting point. The compass will display at that point. 5. Move the compass so that the Z axis points in the direction that you want to route, which should be in the direction of the run that you want to parallel. You can do this by moving it manually, or by clicking the second mouse button once and then toggling the shift key. 6. Once the direction is selected, route toward the run you want to parallel. When the centerline of the target run is highlighted, press the Shift key to toggle between various "solutions," or various sides. In the images below there are only two solutions and you can route on two sides of the target run.
7. Select the target run after you have decided which side you are routing on.
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routingSystems 8. Begin routing and double click to end. The finished run is shown below.
You can place an offset plane on a surface and use it as a reference to route parallel to, or to keep a certain clearance from. After placing the offset plane use the procedure described above.
Aligning a Run to an Existing Surface
This task shows how to align a run to an existing surface or edge while in directional routing mode. This function uses the compass to align a run to the surface or edge. It is assumed that you have taken the steps necessary to start a run. See Routing a Run on an Area. 1. In the directional routing mode move the compass that shows at the end of the run to the edge whose angle you want to emulate.
2. 3.
The Z axis of the compass (it may read W) assumes the angle of the edge against which it is held. At the same time the last segment of your run assumes the angle of the
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Advanced Tasks compass' Z axis. Click once at the end of the segment to move the compass back to it. You can repeat the action to make the run align with any other edge or surface in the area. Double click to end the run.
4.
5.
Routing at an Offset of a Routable
This task shows you how to route a run at an offset of a routable. This function allows you to create a run paralleling an existing run, a defined distance apart. 1. Click the Create an Offset Route button. The Run dialog box displays.
2. Select a segment of the run to which you want an offset. The compass is placed on the segment. 3. The direction in which the Z axis of the compass is pointed determines where the new run will be placed: you can place the new run or runs to the inside, to the outside or stacked on top of the existing run by adjusting the compass. 4. Enter your options in the Run dialog box. or Constant Clearance button. If Click either the Constant Radius you click the Constant Radius button the radius of the turns will be maintained but the offset may vary. If you click the Constant Clearance button the offset will be maintained but the radius of the turns may change. Select one of the Offset Between buttons to indicate whether you want the offset measured from outside edge to outside edge, center line to center line or center line to outside edge.
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A negative offset may be entered to offset in the opposite direction to the compass Z direction. 5. Click OK. The offset run(s) will be created. In the illustration below the run has been created with the Constant Clearance option.
Routing Along a Spline
This task shows you how to route along a spline. This process applies to all routables, such as runs, pathways, and functional path reservations. 1. Import the model which contains the spline into the Piping Design workbench.
2. Click on the Route from Spline button. 3. Select type of run and enter other options. Note: The SAG option is used to define the maximum distance a segment can be from the spline. The run that is created consists of straight segments, as you can see in the illustration below. The smaller the SAG number entered, the closer the run will resemble the spline. But this will also cause more segments to be created. 4. Select Create connection to curve if you want a connection between the run and the spline. If this option is checked the run will move if the spline is moved. 5. Click on the spline. The run is created.
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Advanced Tasks
Routing with Defined Nodes
This task shows you how to route a run with predefined node points. You can create a run by predefining the node points. This means you do not need to route the run by clicking the mouse pointer in the 3D window, as explained below. See Routing a Run for basic information. 1. Create a text file, using a text editor like Wordpad, with column headings as shown below, and define the node sequence, X/Y/Z coordinates and bend radius of the node points. A sample file is provided with this application to help you define the text file. The file name is RunInputNodeData.txt and the location is: ...intel_a\startup\EquipmentandSystems\MultiDiscipline\SampleData. The file is reproduced below to show you the column headings and layout. (It has been opened in Excel to make it easier to distinguish columns.
You can see that there are two sets of node numbers, ranging from 1 to 4. Whenever the application reads the node number 1 it will start a new run. So, based on the file above, two runs will be created.
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routingSystems 2.
. The Open the Run dialog box and click the Import Node Points button File Selection dialog box displays. Navigate to the location of your file and select it. The runs will be created.
Advanced Layout Tasks
Snapping Elements
Snap Resources Together
This task shows you how to snap two resources together. Resources can be joined at existing connectors, you can create new connectors to join them, or you can snap them together without using connectors. All procedures are described below, beginning with the procedure for snapping resources in which you create connectors. To snap resources together by creating new connectors, click the Snap . 1. button 2. Click one of the resources you want to snap together. The resource changes
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Advanced Tasks color and the Define Reference Plane (From) dialog box displays.
By default the Define Plane button is selected, allowing you to select a plane for the connector you will create. See Creating Connectors for information about using the Define Plane functions. The two resources will have a Master-Slave relationship to each other - but only if you choose to add a constraint (see below). If you add a constraint the first object you select becomes the slave, and the second object becomes the master. Also note that the first resource you select will move to snap - the second resource you select remains stationary. 3. Select the second resource. The Define Reference Plane (To) box will display - make your selections as explained above. You can also select an existing connector. Click OK when done. The two resources will snap together and 75
routingSystems the Constraint Options dialog box will display. 4. You can clear the Align, Face and Orientation check boxes and click OK if you want the two resources to remain snapped together without any new connectors being created. To add one or more constraints - which will also result in creating connectors - follow the steps given below. 5. Make your selections in the Snap Options box.
Align: You can increase distance between the two resources, but if you change the alignment the slave will snap back to the original alignment. In the image below the distance is increased but the alignment remains the same.
Face: The two resources will maintain the face if you move one of them. In the image below the two maintain the same face, though the alignment has changed.
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Orientation: The two connectors will maintain the same orientation if you move them, i.e. the red arrows visible in the connectors will align. It is therefore important to make sure that the red arrows in the connectors are pointed correctly and oriented correctly with reference to the part. The red arrow is usually set to the "Up" position of the resource, which means that on both resources they should point in the Up direction. If the red arrow points "down" in one resource and "up" in the other, then the resources will snap together incorrectly. You can toggle the position of the red arrow by clicking on the green arrow that is parallel to the plane. Fix in space: If you select this option the position of the master resource is fixed - if it is moved it will snap back to its original position. Attach: Checking this option allows you to attach the two objects. Place manipulator at snapped location: Check this if you want to rotate the snapped object after placing it. The manipulator is placed on the object if you check this. You can then click on the bottom curve of the manipulator (see image below) and rotate the object. It will rotate in increments, based on the value entered in the Snap Angle field. In the image above it is 45 degrees.
To remove a constraint select it in the specifications tree and delete it. To remove the 'Fix in space' option right click on the Fix line in the specifications tree, click Properties, go to the Constraints tab, and uncheck the Fix in space box. 6. Click OK when done. 7. To snap resources together using preexisting connectors: a. Click the Snap button. b. Move the pointer over the first resource - the connectors will display.
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routingSystems Select the connector. c. Move the pointer over the second resource - the connectors will display. Select the connector and the two resources will snap together. d. The Snap Options box will display. Make your selections and click OK.
Quick Snap Resources
This task shows you how to Quick Snap two resources together. The Quick Snap procedure allows you to snap two resources together using one of three selection methods. You can select the snapping point on one of the resources using one of these methods. On the other resource the snapping point will either be its origin, or at a connector, as described in Step 2. The three selection methods are: • • • Center of three points (on a circle): the snapping will be the center of three points indicated by you. Center of polygon: the snapping point will be the center of any surface indicated by you. Surface: the snapping point is at any point indicated by you.
The three methods are described below. To snap resources together using the center of three points on a circle 1. method, click the Snap Three Points button .
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Advanced Tasks 2. Click the resource that you want to move. Note: • • • If you click the resource at a connector it will snap to the other resource at that connector. You can create a connector if you want to. If you click the resource at a point other than a connector it will join to the other resource at its origin. If the resource was preselected when you clicked the snap command you will not be able to select a connector.
These points apply to all three methods of Quick Snap. In the image below the user wants the paint gun to snap to the robot arm. After he clicks the paint gun the compass displays at the origin of the paint gun to show that the part will snap at that location. You can choose not to display the compass at the snap location by unchecking the option Place compass at snapping point in the Snap Options dialog box. The box displays when you click on any of the Quick Snap buttons. Placing the compass at the snapping location allows you to rotate the resource after it has snapped.
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routingSystems 3. Define the point on the robot where you want the paint gun to snap, in this case the end of the robot arm, by clicking on three points. You can only select your defining points on the edges of a circle. Only points on the ends of edges are selectable. Note: If you click the three points clockwise the paint gun will attach "inward" as shown in the image below:
If you click counter clockwise then the paint gun will attach "outward", which is the correct position in this example.
4. To Quick Snap using the center of polygon method, click the Snap Center of Polygon button and perform the action detailed in Step 2.
5. Select the snapping point on the second resource by clicking on a surface. The resource will be placed in the center of the polygon.
6.
To Quick Snap using the surface method, click the Snap Surface and perform the action detailed in Step 2.
button
7. Select the snapping point on the second resource by clicking on any surface. The resource will be placed at the point you click. If you double click a command you will be in repeat mode. This allows you to snap a resource to a different location, using a different selection method if you want.
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Advanced Tasks
Snap and Rotate a Resource
This task shows you how to rotate a resource after snapping it to another resource. 1. With both resources on the screen, click on the Snap resource. The orientation symbol will appear. button and then on a
2. Click on the second resource. A white square will appear. Move the pointer over the resource and click when the white square is at the location where you want to snap the two resources. The orientation symbol will appear at the location and the Define Reference Plane dialog box will display.
3.
Click on the Define plane using compass button . The compass will be placed at the location where you want to snap the two resources.
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4. Click OK on the Define Reference Plane box. The two resources will snap together.
5. Click on the Select button to exit the Snap command. Click on the resource you want to rotate, then grab one of the handles on the compass with your pointer and move it. Different handles will move/rotate the resource in different directions.
You can also double click on the compass to bring up the Compass Manipulation dialog box and enter the required figure in the Angle field. Click on the + or - sign next to the Z axis to rotate it.
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Mirroring Elements
This task shows you how to move one or more elements to the opposite side of a selected plane, as a mirror image. It also shows how to copy one or more elements to the opposite side. 1. Select the element(s) you want to move. (You can also select after Step 2.) 2. Click on the Mirror button . 3. The Reference panel will display if you already have a reference plane defined (by having used the offset plane command).
Click the New Reference Plane button and follow Step 4 if you want to define a new reference plane. Follow Step 4b if you want to use the existing reference plane. The Reference panel will not display if you do not have a reference plane already defined. 4. Define a reference plane across which to mirror the element by doing the following:
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routingSystems 1. Place your cursor over a geometric element that defines the plane (e.g., a construction plane, boundary, area contour, item reservation). As you move the cursor, a small white rectangle is displayed to show the selectable planes, as shown below. If you do not see the white rectangle, zoom out from the drawing. The white rectangle cannot be displayed if the element under your cursor is displayed too small.
b. Click to select the plane. The selected elements are mirrored to the other side of the plane, as shown below.
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5. To Mirror and Copy the elements, follow the steps outlined above and then click the Mirror and Copy icon . The selected elements will be copied to the other side of the plane. In the illustration above, the selected elements will stay where they are and two similar elements will be added to the other side of the plane.
Aligning Elements
This task shows you how to align elements in your layout. You can align the center or the sides of an element to a user defined reference plane that you define. You can also rotate an element to align it with a reference plane. 1. Select the element(s) that you want to align. 2. Select the icon for the type of alignment you want to perform:
Align Sides: aligns the sides of two or more elements
Align Center: aligns along the centerlines of two or more elements
Rotate to Align: rotates elements on the axis to align them
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Align Planes: aligns selected planes
Distribute: See Distributing elements 3. Define the plane to use as a reference for the alignment. If you have an offset plane already defined it will be used as the reference plane. If you do not already have the offset plane defined do the following: a. Place your cursor over a geometric element that defines the plane (e.g., a construction plane, boundary, area contour, item reservation). As you move the cursor, a small white rectangle is displayed to show the selectable planes, as shown below. A line normal to the rectangle shows the direction in which the alignment will be performed.
If you do not see the white rectangle, zoom out from the drawing. The white rectangle cannot be displayed if the element under your cursor is displayed too small. b. Click to select the plane. The selected elements are aligned along the plane.
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4. Using the Align Planes command allows you to select any plane on an item reservation or part. After you select the first plane to which to align to, you can only select a plane that is parallel to it. For instance, if you select the the top of an item reservation you need to select the top or bottom of the second item reservation - you cannot select the sides. Click any button in one of the tool bars to exit the alignment command. If you want to continue with the alignment command using the same reference plane then select another element in the model.
Distributing Elements
This task shows you how to distribute elements within parameters that you define. 1. Select the elements you want to move. 2. Click the Distribute button . 3. Define a reference plane for the distribution by doing the following: a. Place your cursor over a geometric element that defines the plane (e.g., a construction plane, boundary, area contour, item reservation). As you move the cursor, a small white rectangle is displayed to show the selectable planes, as shown below. A line perpendicular to the rectangle shows the direction in which the distribution will be performed.
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routingSystems If you do not see the white rectangle, zoom out from the drawing. The white rectangle cannot be displayed if the element under your cursor is displayed too small.
b. Click to select the plane. The selected elements are distributed along a line perpendicular to the plane, as shown below.
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Advanced Tasks
Rearranging the Specifications Tree
This task shows you how to transfer elements in your layout from one level of the specifications tree to another. 1. Make the appropriate element active.
You must make active an element that is at least one level higher than both the source element (i.e., the one that is being transferred) and the target element. For example, in order to transfer ArrBox5, ArrBox6, ArrBox7, ArrBox 8, and ArrBox9 to ArrArea3, shown below, ArrArea1 or Product1 must be active.
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2. Select the elements you want to transfer.
Select the Transfer Elements in Tree button . 4. Select the element to which you want the elements transferred. The target element must also be a child of the active element.
3.
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The elements you select in Step 2 become children of (i.e., subordinate to) the element you select in Step 4.
Changing the Current Axis
This task shows you how to change the current axis. When you activate an object, the current axis is reset to the axis of that object. Changing the current axis changes the reference point by which elements are 91
routingSystems routed and placed. . 1. Click the Change Current Axis icon 2. Select the object you want to use as a reference. The axis for the selected object is displayed. 3. You can also change the current axis and place the compass on the object. The compass allows you to manipulate that object. To do this click the Change Current Axis and Snap Compass button The axis and compass are both placed. and select the object.
Disabling/Enabling Manipulation Handles
This task shows you how to disable or enable manipulator handles using the Toggle Manipulator Handle Mode command. The default is for the manipulation handles to be enabled. If you are working on a large document, however, displaying the handles on each part can take up time. If you do not need the handles then you can use this feature to disable the display. It is a toggle button, so clicking it again will enable the handles. This feature can be used with parts placed in-line or in free space. To disable display of the manipulation 'handles' click the Toggle Manipulation 1. Handle Mode button . To enable them again click the button once more. The handles look like a green box on parts placed in free space. On parts placed in line they look like the image below.
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Advanced Tasks
Generating Detail Information
This task shows you how to display detailed information about objects as you move the pointer over them. The Analyze Item command displays information about an object when the pointer passes over it. This information can include line IDs, nominal size of runs and parts, XYZ coordinates of connectors, etc. The type of information shown will depend on the object and the product you are using. See also Display Information About Routables. From Release 13 the angle of routables from the x,y,z axis will also display, as in the image below.
1.
With your document open, click the Analyze Item button . 2. Move the pointer in the document highlighting various objects. Attributes and their values are displayed, depending on the type of object highlighted. In the illustration below the pointer is on a tubing tee.
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3. When you click again the feature will be disabled.
Editing Parts
Changing the Reference File for a Part
This task shows you how to change the reference file for a part. When you place a part in a document, each part has a reference file associated with it. This file contains data about that part. To save disk space, the application normally uses one reference file for all similar parts - an elbow that has been placed nine times in a document will have one reference file for it. It also means that you cannot change the dimensions of one or more of those elbows. This function allows you to create a unique reference file for one or more parts, allowing you to assign unique parameters to them. Using this function you can: • • 1. With your document open, click the Change Part Reference button Change Reference dialog box will display. . The Assign a unique reference file to a part. Assign a part the unique reference file (and parameters) of another part.
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2. If you have already selected a part a file name will display in the file name field; if not it will display when you select a part. If you want to change the file name make sure you have not already assigned it. 3. Click OK. 4. To assign an existing unique reference file to a part: If one of the parts in your document already has a unique reference file you can assign it to other parts. Select the part or parts to which you want to assign a reference file; click the Select New Reference button in the Change Reference box; then select the part that has the unique reference file. You will see the file name change to the unique reference file name in the specifications tree.
Change the Parameters of a Part
This task shows you how to change the parameters of a part.
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routingSystems 1. Select the part, in this case an elbow, at the end of a run and click the Edit Part Parameters button . This will display the Parameter Explorer dialog box.
2. The box will display a list of parameters that can be edited for the part you selected. Select one of the parameters. 3. If it is possible to change this parameter by entering a value in the Parameter Value field then do so. If the Value field is grayed out then click the button to the right of it
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4. A dialog box will display, displaying the values that can be selected. Select one of the values.
5. Click OK to exit the dialog boxes. These are the only commands relevant to the change part parameter procedure. Other buttons and fields on the Parameter Explorer dialog box are meant for other functions and should not be used.
Creating and Modifying Connectors
Create Connectors
This task shows you how to create a connector. Connectors can only be created on objects that have existing geometry that satisfies the rules of connector creation. If existing geometry is not present, you will have to create the geometry. 1. If the resource is not active, make it active by double-clicking in the specifications tree. Click the Build Connector button. This will bring up the Manage Connectors 2. dialog box. You will not be able to add a connector on the instance of a part using the Add command in the Manage Connectors dialog box. You can only add connectors on the reference of a part (the part in the master catalog), using the Create Part command. However, you can add a connector to a unique part using the Manage Connectors dialog box. The Manage Connectors dialog box will list all connectors on the selected part. To see a connector and its associated geometry on the part, select a connector from the list. Adding a connector is explained below; Delete, Modify and Duplicate are explained elsewhere in this section. To Publish a connector means you are
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routingSystems allowing people who do not have write access to your document to establish a connection. This is explained further in Using Work Packages. You can Publish or Unpublish connectors using the two buttons.
3. Click the Add button. The Add Connectors box displays.
Select the type of connector - piping, HVAC, etc. In some applications the flow direction field will be available. The piping (or tubing) part connector has flow direction built in and you must select a flow direction also from the drop down menu. The mechanical part connector has no flow direction. 98
Advanced Tasks
Another type of connector - the nozzle connector - will be available if you are placing a connector on a nozzle. A nozzle connector must be placed on the end of the nozzle that connects to equipment. A part connector is placed on the end that connects to the pipe or duct. An electrical part connector should only be placed on a socket. The electrical part connector should be placed on the end of the socket that connects to equipment. A cableway part connector should be placed on the free end of the socket that does not connect to equipment. When you are placing a connector on a Bendable, such as a bendable pipe, you must use the Define New Geometry option. You must not use existing geometry to place the connector. You can name each connector by selecting in the Name field. This is useful for some functions, such as designing using a schematic. The concept of Publishing or Unpublishing a connector is explained above. Check the checkbox as necessary. Face, orientation and alignment are explained below. The orientation, alignment and face must be defined correctly before a connector can be created. To explain what these are, the face is the surface to which you attach a connector. As an example, if you want to attach a clock to your office wall, the wall is the face. You want the numeral "12" to be up, so you orient the clock accordingly. This is the orientation. The alignment is the direction in which the clock face is pointed - normally it would be perpendicular to the wall. When creating a connector, the alignment always has to be perpendicular to the face. The face is generally defined using a face of the part, such as the end of a pipe. Alignment is usually defined using a line, such as the not-shown line along the centerline of a pipe. Orientation is defined using the xy plane, or another plane or face to define an "up" direction. In the illustration below the Z axis indicates the alignment of the connector. It also indicates the direction in which routing will occur. The X and Y axis together define the orientation. They are useful when attaching two resources.
It is necessary to select geometry in the part to which you want to attach a connector so that these three characteristics are correctly defined. If the part does not have the necessary geometry then you must create it.
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routingSystems 4. If you want to create a connector using the part's existing geometry click the Use existing geometry option. Click the Select Face button to select a face. Selectable faces will highlight as you move your pointer over the part.
Click this button to select the alignment. You will only be able to indicate the alignment by selecting a line - from the construction geometry, or elsewhere in the part if there is one. You can only select a line that is perpendicular to the face plane. Click this button to select the orientation. You will only be able to select a plane that is perpendicular to the face you selected. If you cannot find a plane to select, click the Swap Visible Space button (see below) to make the construction geometry visible, and select a plane.
Some connector types require you to place a datum point. The datum point is placed by clicking this button and then clicking a 3-D point on the part. The datum point is used as follows: • • • Lofted reservation section: Datum is used to define where the spline will start and end when creating lofted reservations. Tubing & waveguide parts: Datum is used to define where the spline will start and end when creating flexible tubes. Hangers: See Hanger Design documentation.
You can display the part construction geometry, if there is any, to make it easier to select existing geometry. Do this by: • • • Right click on the part entry in the specifications tree. Click Hide/Show. The part will disappear from the screen. . The part will reappear on Click the Swap Visible Space button your screen with the construction geometry visible. Clicking the button again will toggle you back.
5. The fields under Classify Connector will become available after you have successfully selected the geometry explained in Step 4. Click on the down arrows to make your selection. Select a type.
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For Flow direction, select In, Out, InOut or None. Select the Face type. A Hole connection allows a routable to pass through it it is useful for placing parts like clamps along a run without cutting a tube. A Face connection will stop a routable and not allow it to pass through. Select an alignment. Choose an orientation: Circular will allow the connector to attach to another connector at any orientation; round ducts and pipes, for instance, do not need a well-defined "up" direction because they can rotate. A Rectangular orientation is used for parts like rectangular ducts; they do not have a strict ''up" direction. Up allows the connector to attach to another connector or part in the up position: horizontal trays, for instance, require a well-defined "up" position. You can also use the "up" orientation for a hole connector. In the image below, the connector on the right has the up orientation, the connector on the left does not.
The number in the Number field is assigned by the application. This can be significant because when you are creating a new connector, you have the option of using the alignment and orientation used in the previous connector after you select the face. You can choose to do this, or select a new alignment and/or orientation. 6. Click OK. The new connector will be listed in the Manage Connectors box. 7. To define new geometry for placing a connector, select the option Define new geometry, then click on the Select plane button will display. . The Define Plane box
8. Use the functions provided by the Define Plane box to reposition the connector, if necessary, as explained below. (The colors of the buttons may be slightly different in some applications.)
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Click the Define Plane button to redefine the plane as well as the origin by clicking once on the face. Click the Define Plane using Compass button to redefine the plane using the compass. Click the Define 3-point Plane button to define the plane by clicking on any three points with your pointer. The connector will be placed on the first point you click. Click the Define Line-Point Plane button to select the plane by clicking on a point and a line, like an edge. The connector will be placed on the first point you click. Click the Define Line-Line button to select the plane by clicking on two lines. The plane will be defined by the first line selected. But if the two lines are parallel the plane will be defined as the plane in which both lines exist. Click the Define plane at center of circle button to select the plane by clicking three points on the edge of a circle. This method is used for multiCAD documents, usually for CGR circles. You can click at points where two lines meet or in the center of a face. The Z axis of the plane manipulator will be placed according to the right hand rule. If you click clockwise the Z axis will point into the object. If you click counter clockwise the Z axis will point out from the object. Click the Define plane at product origin button and then the object to place the plane manipulator on the origin of the object. The plane manipulator axis will match that of the product. Click the Define Orientation button to change the orientation. Click the button and then click a point or a line. If you click a point the X axis will point to it. If you click a line the X axis will become parallel to the line.
Define Origin at Plane Use the Move Origin buttons to define the plane. or Compass allows you to define the origin using the compass or plane command. You use the compass or plane as the base plane along which the
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origin can be selected.
Define Origin at Point or Center of Face lets you
Define Origin at Center of select the origin by clicking on a point or face. Circle allows to select the origin by clicking at three points - the origin will be placed in the center of an imaginary circle drawn using those three points. The plane and orientation will not change when using this command. 9. Click OK. The connector will be placed and the Add Connector dialog box will display again.< 10.Make your selections in the fields under Classify Connector as described in Step 5. Click OK.
Using the Compass to Manipulate Connectors
This task shows you how to use the compass to manipulate connectors placed on resolved parts. You can use the compass to manipulate connectors placed on resolved parts only. Use this method when adding a new connector, or by using the Modify command. Both are explained below. 1. To manipulate while adding a connector, drag the compass and place it over the connector while the Define Plane box is displayed. 2. To manipulate using the Modify command, select the resource, click the Manage Connectors button and, in the Manage Connectors dialog box, select the connector in the connectors list. Click the Modify button. 3. The Modify Connectors box will display. You can now drag the compass and place it over the connector. 4. Click on one of the handles on the compass and manipulate the connector to the desired position. You can change alignment, orientation and origin using the compass.
5. Click OK on the Modify Connector or the Define Plane dialog box when done. Remove the compass from the connector by dragging it to the axis.
Modifying or Deleting Connectors
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routingSystems This task shows you how to modify or delete connectors. You will not be able to modify or delete a connector that has constraints or connections. You will not be able to modify or delete a connector on the instance of a part using the Modify or Delete commands in the Manage Connectors dialog box. You can only modify or delete connectors on the reference of a part (the part in the master catalog). You need to use the Create Part command to modify a reference part. However, you can modify or delete a unique part using the Manage Connectors dialog box. 1. To delete a connector select the resource by double clicking in the specifications tree and click the Build Connectors button. This will display the Manage Connectors dialog box. 2. Select the connector in the connectors list and click the Delete button. The connector will be deleted. 3. To modify a connector click the Modify button in the Manage Connectors box. The Modify Connectors dialog box displays.
4. Follow the procedures described in Step 4 and subsequent of Creating Connectors.
Creating Duplicate Connectors
This task shows you how to create one or more duplicate connectors.
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Advanced Tasks You can only make duplicate connectors on a resolved part. Connectors can only be duplicated on the same part. With your resolved part displayed, click the Build Connectors button. This will open 1. the Manage Connectors dialog box. 2. Select the part. This will display all connectors on it and also display a list in the dialog box.
3. Select the connector you want to duplicate and click Duplicate in the Manage Connectors dialog box. The Duplicate Connectors dialog box displays.
4. Enter the spacing between the connectors and the number of connectors you want.
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routingSystems 5. Drag the compass and place it on a surface with the Z axis pointing toward the direction in which you want the new connectors located. The two illustrations below show how you can change the location of the new connectors by changing the direction of the Z axis.
6. Click OK.
Using the Plane Manipulator
This task shows you how to use the plane manipulator. You can use the plane manipulator to change the orientation, alignment, plane and location of the plane you propose to create. The X and Y axis indicate the orientation and the Z axis indicates the alignment. For example, if you create a connector and route from it, routing will occur in the direction indicated by the Z axis.
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1. To change the orientation of an axis, click on the dot at the end of it. It will flip 180 degrees.
2. To move the manipulator along any axis, click and drag on that axis. The manipulator will move and the distance will display. 3. Click on the origin (red square) and drag to move the manipulator to a new plane. 4. To change the orientation you can also click and drag any of the arcs in the manipulator to rotate it. It will rotate in increments, which is 15 degrees in the image below.
To change the degree of rotation click Tools-Options, select Equipments & Systems and select the General tab. Enter the degree of rotation in the Snap Angle field. For instance, if you enter 45, the manipulator will snap in increments of 45 degrees, counting its starting position as 0. It will snap to the nearest 45 degree step - if you move it to 88 degrees from its starting position it will snap to 90 degrees.
Working with Bendables
Extracting Bending Data from Bendable Pipes and Tubes
This task shows you how to extract bending data from Bendable Pipes and Tubes and transfer it into a Microsoft Excel worksheet. Bending data can be fed into Bending machines to precisely create bends in bendable tubes and pipes. • The standard macro supplied with this product displays bending data in a sample format. However, a user with some Microsoft VBScript experience can change the script supplied to change the format.
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routingSystems • • The sample script assumes that the bendable objects are placed on a run under a distribution system or a logical line. For more information on placing parts, see Placing Parts in a CATProduct Drawing. command subdirectory.
1.
Using Windows Explorer, locate the intel_a
code
2. Copy the files PslTubingExtract.CATScript and PslTubingExtractTemplate.xls
to C: temp (with read-write access). Select the two files and click the right mouse button. Click Properties in the drop-down menu that displays. The
Properties dialog box will display. Uncheck the Read-Only option.
3. In the specifications tree, select the logical line or distribution system under which the run containing the bendable objects has been placed.
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4. Click Tools - Macro - Macros. The Macro dialog box will display. Select External File from the drop down list, select PslTubingExtract.CATScript and click Select. The Select External File dialog box will display. Select PslTubingExtract.CATScript and click Open. This will again display the Macro dialog box. Select PslTubingExtract.CATScript and click Run. Data will be extracted from the bendable objects and displayed in an Excel worksheet, part of which is displayed below. (CATIA will create the table, but you must have Excel installed!)
Design Checks for Bendable Pipes and Tubes
This task shows you how to perform design checks on bendable pipes and tubes. The design checks will tell you whether the radius of a bend, the total length of the run and the rest length are within prescribed limits. The rest length is the straight segment between two nodes (with bend radius). Click the Update button whenever you see it active (not greyed out) during this process. Also, don't forget that you need to have the Knowledge Expert product installed for this process. In the following example the maximum bend radius will be checked.
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routingSystems 1. Click Start - Infrastructure - Knowledge Expert to enter the Knowledge Expert workbench. 2. Set up your options correctly or you will not be able to do the following steps correctly. • • • • • Click Tools - Options and select General from the left column of the window. Click the General tab. Select Automatic for the Update function. Click Product in the left column of the window and scroll to the Product Structure tab. Under the Specification Tree function make sure the Relations and Automatic Expand options are selected.
3. Make the run active. 4.
Click the Insert Rules button directory.
and navigate to the KnowledgeRules
5. Select Bendable_CheckMaxBendRadius.CATProduct and click Open. 6. If the desired bend radius violates the bend radius rules, a red light will show against the relevant CATProduct line icon in the specifications tree, in this case CATKWEBendRadiusCheck.1. If there is no violation then a green light will show next to it. In the illustration below the red button is showing (with the mouse pointer pointed at it).
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Advanced Tasks 7. To change the maximum bend radius do the following: Each check has a parameter element beneath it in the specifications tree - in this case it is MaxBendRadius. Double-click on the element to display the Edit Parameter dialog box. Enter your maximum bend radius in this box. To check for rest length and total run length select the appropriate CATProduct in the Load Report dialog box. Make sure it has the word "check" in it.
Transfer Elements to New Document
This task shows you how to transfer elements to a new document. You can use this function to transfer elements to documents or work packages that are under the same Product. See also Transfer Run to Another Document. This function removes selected elements from a document and moves them to a new document. You cannot move them to an existing document. 1. With your document open, click the Transfer Elements button . The Transfer Elements dialog box displays. In the image below it displays equipment that has been selected.
2. You can select elements to transfer in various ways: • • Click the element you want to transfer. Click the Select Elements in Range button and make your selection in the Analyze Networks dialog box that displays.
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• •
Click the Select Spools Selection List. Click the Select Line IDs Selection List.
button and make your selection in the button and make your selection in the
3. If you do not want to transfer some elements in the Selection List, select the element(s) and click Remove. Remove All removes all elements. 4. Make your selections. Spools and Lines will display the existing name in the File Name field. You can edit this name, or add a Prefix or Suffix (or both) to distinguish it from the original name. Elements do not display any name you need to enter a name. In this example it is TestTransfer. The image below shows the entries in the specifications tree, with the Equipments node expanded, before the transfer.
5. The vessel has been selected for transfer (the associated nozzle will automatically be selected). Click Apply or OK. Apply allows you to transfer more elements. OK exits you from the command. The image below shows the transferred equipment.
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Workbench Description
Workbench Description
The Systems Routing workbench includes the following toolbars:
Systems Routing Toolbar
General Design Toolbar
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General Environment Toolbar
Product Placement Toolbar
Update the System
Toolbars
Systems Routing Toolbar
The Systems Routing Toolbar contains the following tools:
See Creating a Logical Assembly.
See Creating a System Assembly See Creating a Logical Set See Routing Runs and Modifying Runs. See Route a Run Along a Spline See Route a Run at an Offset of a Routable See Route a Run within a Pathway See Create an Offset Connection between Segments See Disconnecting a Run See Connecting a Run See Breaking Run at a Branch
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Workbench Description
See Creating a Pathway
General Design Toolbar
The General Design Toolbar contains the following tools:
Align Toolbar See Aligning Elements See Aligning elements See Aligning elements See Distributing Elements See Aligning elements Snap Toolbar See Snap Resources Together Snap Three Points: See Quick Snap Resources Snap Center of Polygon: See Quick Snap Resources Snap Surface: See Quick Snap Resources See Create Parent-Child Relationship See Mirroring Elements. See Mirroring Elements See Rearranging Elements in the Specification Tree. See Connectors
Product Placement Toolbar
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routingSystems The Product Placement Toolbar contains the following tools:
See Catalog Browser See Placing Multiple Parts in a Run See Flipping Elements See Change the Reference File for a Part See Change the Parameters of a Part
General Environment Toolbar
The General Environment Toolbar contains the following tools:
See Changing the Current Axis.
See Generating Detail Information See Using Offset Planes
Advanced Offset Plane See Using a Step Grid for these icons: Snap to steps off current axis Snap to steps off last position Snap to XY construction plane Snap to all construction planes Snap to elevation (Z) construction plane
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Workbench Description
Snap to Drafting elements See Making an Element Active.
See Manipulation Handle Mode See Making an Element Active for these icons: Activate Parent Activate Area Activate Network/Logical Line
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Project Standards
Systems Routing Settings
General Settings
This task is to inform you about the settings in the General tab. The General tab provides settings for General Environment, Resolved Part Storage path, Resource Attributes and Catalog Placement Options. 1. Click Tools - Options - Equipment & Systems and select the General tab.
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routingSystems 2. General Environment: • Grid Step. This is the default grid step setting that displays in the General Environment toolbar at the bottom of the 3-D viewer. Even if you change the value in the toolbar during your session, the value entered in the Grid Step field will re-appear when you open a new session. Enter your preference for the Grid Step. Note: The Units (unit of measure) is set in the Units tab under Tools - Options - General - Parameters and Measure. See also Set Correct Working Units and Grid. The Snap Angle sets the degree of rotation of the plane manipulator. See Using the Plane Manipulator for more information.
•
3. Resolved Part Storage for Spatial Objects: • Directory. This is the location where resolved Spatial objects unique to the Plant Layout, Systems Routing and Systems Space Reservations products are stored. Click the Open file button and navigate in the Resolved Part Storage Directory Browser window to set or change the location for the directory.
4. Resource Attributes: • Automatic creation of resource attributes. Certain attributes accompany Spatial objects (those created in Plant Layout, Systems Routing and Systems Space Reservations); objects such as item reservations, areas, runs, etc. These attributes, or properties, are generated specifically for the Delmia product line and cannot be assigned or changed in other product lines.
Although you will not be making use of these resource properties, their creation will have no affect on the product you are working in. If you do not want these properties to be created, uncheck the box Automatic creation of resource attributes and click OK. 5. Catalog Placement Options: • Display image while placing catalog object in 3-D viewer. You can choose to hide or display a "preview" of the part you are placing. Check or uncheck the box Display image while placing catalog object in 3D viewer to obtain the effect you want. Place at component's origin when placing in free space. By default, when you click (in free space) to place a part, the center of the part will be placed at that location. The application determines the center of the part by creating a box around it and selecting the center of the base of the box. You can also choose to place the origin of the part at the point where you click. To do this check the box Place at component's origin when placing in free space.
•
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Project Standards
Display Settings
This task is to inform you about the options available in the Display tab. The Display tab provides display options for Analysis Mode, Specifications Tree, 3-D Viewer Display and Routable Display options. 1.Go to Tools - Options - Equipment & Systems and click the Display tab.
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Analysis Mode: Check the box in Analysis Mode to display information about routables. It works only when you are performing an action with a routable, such as placing a part, branching a run or creating an offset route. Specification Tree: In Application objects check the box Show application grouping to organize the objects in the tree by application, e.g. Piping objects, Equipment, etc. Under Spatial objects check the boxes of the items you want to appear in the specifications tree. Spatial objects may only be placed using the Systems Routing, Systems Space Reservation and Plant Layout workbenches.
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3-D Viewer Display Options: Check or uncheck the boxes to set the connection and connector display options as desired. Set the color of the connection and connector symbols using the drop down color palette. Routable Display Options: Increase the Twist Smoothness Factor to increase the smoothness of a run at a twisting turn.
Design Criteria Settings
This task is to inform you about the settings in the Design Criteria tab. The Design Criteria tab allows you to toggle settings for ID Management, 3D Design, and 3D Placement. 1. Click Tools - Options - Equipment & Systems and select the Design Criteria tab.
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ID Management: Update ID on property change. When the object naming convention (ID schema) includes an attribute, e.g. nominal size, and you change its value using the Properties dialog box, the name of the object will change to reflect the new value of the attribute. 3D Design: Check Schematic Driven if you are placing parts from a schematic into a 3D design document. Used with Piping Design, Tubing Design, HVAC Design and Waveguide Design applications. 3D Placement Options: When the Place automatic parts box is checked you can place an object such as a valve (e.g., in Piping Design); the flanges, gaskets and welds will be placed automatically when you place the pipe.
Working in Cache Mode
This task discusses steps you should take to design efficiently in cache mode. Cache mode refers to designing without loading all the technological data of objects in your document. It is recommended because it allows quicker loading of documents and execution of commands. However, you may need to take certain steps to design efficiently in this mode, which are discussed here. This task also explains ways of executing certain commands while in cache mode.
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routingSystems 1. When you are using the command Place Object from Catalog while you are in cache mode you will not be able to place a part on a connector because connectors are not loaded. To change that part to design mode click the button and then click the part. That part will be Analyze Item converted to design mode and connectors will be visible. 2. It is recommended that you redefine the location of the CATCache directory. This directory is used to store certain design elements (cgr files) that are used when visualizing a document in cache mode. If the file name of an element is too long then the visualization will not be correct - this is a Windows limitation. Because the full path name is used in the file name, you should redefine the location so that the path name is short - as short as you can make it. To redefine the path name click Tools - Options Infrastructure - Product Structure and select the Cache Management tab. Enter the new path in the Path to the Local Cache field.
3. Wireframe geometry, such as the sections on trapeze hangers, are not visible in cache mode, which also means they cannot be selected. If you want to be able to see them in cache mode then check the option Save Lineic Elements in CGR. You can find it in Tools - Options - Infrastructure Product Structure and the CGR Management tab.
Customizing the Dictionary of User Types
Customizing the Dictionary of User Types
This task explains how to customize the list of types that are displayed when you create any of these elements:
• • •
System assembly Logical assembly Runs
A basic dictionary of these element types is provided with the product. You can add entries to or delete entries from the basic dictionary, or you can replace it entirely. You can also customize the icons that are associated with the element types. To customize the dictionary, you need to run the following scripts: PSLNomenAccessFeat.CATScript reads the existing dictionary and writes it to a preformatted Microsoft* Excel file. PSLNomenBuildFeat.CATScript takes a properly fomatted Excel file and generates a new dictionary.
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Project Standards To accomplish this procedure, you must have installed Microsoft Excel 97 or later version. You should be familiar with the basic editing features of Excel, as well as with the file navigation and file editing capabilities of your system. 1. Copy the following files from intel_a code command to a drive or directory for which you have read and write permissions: • • • PSLNomenAccessFeat.CATScript PSLNomenBuildFeat.CATScript PSLNomenAccessFeatTemplate.xls
2. Start CATIA. 3. From the menu bar, select Tools -> Macro -> Macros. 4. Select External File for the Macro In: field. 5. Click the Select button, and use the Windows dialog box to navigate to the appropriate file. 6. Select the file PSLNomenAccessFeat.CATScript and select OK. 7. Edit PSLNomenAccessFeat.CATScript as follows: Define the path strEXCELTemplateFileName to point to the directory to which you copied the files in Step 1.
8. Save and close the file. 9. Select Run. Microsoft Excel is launched, and a file is created. 10. Edit the Excel file to add or delete entries, as appropriate. 11. Save the Excel file with a unique name. 12. From the CATIA menu bar, select Tools -> Macro -> Macros again. 13. Select the Select button, and select the file PSLNomenBuildFeat.CATScript. 14. Edit PSLNomenBuildFeat.CATScript as follows: • • Define the input path strEXCELInputFileName to point to the Excel file you saved in Step 11. Define the output path strCATIAV5FeatOutputFileName to point to intel_a eat. If you do not have write permissions for this output path directory, you can define a temporary location. Contact your system administrator to move or copy the file to the correct location after it has been created. 15. Save and close the file. resources graphic CATArrNomenclature.f
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routingSystems 16. Select Run. The output file is created in the directory you specified. If you defined a temporary location for the file, it must be moved or copied to intel_a resources graphicCATArrNomenclature.feat before the modifications can take effect. The modifications will take effect when you restart CATIA.
Searching User-Created Dictionary Entries
This task shows you how to search documents for objects or elements that are user created. To learn more about the Search function see the Infrastructure user guide. To learn more about customizing see Customizing the Dictionary of Types. 1. Click Tools - Macro - Macros. This will display the Macro dialog box. In the drop down menu select External File and click Select.
2. The Select External File dialog box will display. Navigate to the directory where CATIA is installed and open the directory intel_a code command. Select the file CATArrExtractArrFeatAsCATNLS.CATScript and click Open. The Select External File dialog box will close and the Macro dialog box will display, with the file CATArrExtractArrFeatAsCATNLS.CATScript selected. Click Run. 3. 4. Close the CATIA session. Using Windows Explorer navigate to the directory C: file CATArrNomenclatureFeat.CATNls to the directory temp and copy the
intel_a resources msgcatalog. 5. Also copy the file CATArrNomenclatureFeat.CATNls to all language subdirectories (if any) of Intel_a resources msgcatalog.
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Saving a System Assembly or Logical Assembly as a Separate Document
This task shows you how to create and save a system assembly or logical assembly as a separate document.. This function is needed if you want to work separately on a component of a larger project. If you save the system assembly or logical assembly as a separate document you can open it without having to open the entire project. At the same time it remains part of the larger project. 1. When creating a new System Assembly or Logical Assembly check the Create new document option.
2. Enter a name in the File Name field and click OK. The new document appears in the specifications tree as a child of whichever element you created it under. In the specifications tree, the icon for a system or logical line created as a separate document is different from that which is not created in a separate document. In the illustration below WasteWater is created as a separate document, Piping System Assembly1 is not.
3. When you save the project a dialog box will ask if you want to proceed with other document save operations. Click OK.
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Creating a Catalog
Creating Parts
This task explains how to create parts for the Systems Routing Product. 1. Create the geometry for the part. Use the Version 5 Part Design product to create the geometry. See the Version 5 Part Design User's Guide for instructions about how to use this product. • • • If you want to be able to place the part parametrically, go on to Step 2. For fixed-sized parts, save the part as a CATPart document and skip to Step 5. If you want to use the same set of geometry for different sizes of the same type of part, go on to Step 2.
2. Define parameters for the geometry.
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Project Standards When you define parameters, you must adhere to the following naming conventions to ensure that the part can be sized correctly when it is placed. The values for these reserved parameters are derived from the run on which the part is placed. • • • • • • CATRouOutsideDiameter : outside diameter of the part if it is placed on a cylindrical run CATRouOutsideHeight : overall height of the part if it is placed on a rectangular run CATRouOutsideWidth : overall width of the part if it is placed on a rectangular run CATRouFaceToFaceLength : overall length of a stretchable part such as pipe or duct CATRouAngle : turn or branch angle of parts such as an elbow or tee CATRouTurnRadius : bend radius of a part such as an elbow or horizontal turn
You may also add two other reserved parameters to your part as User attributes. • • CATRouPartNumber : a string parameter. This parameter will contain the part's part number. CATRouSize : a string parameter. This parameter will contain a character string representing the nominal size of the part. It can be used instead of CATRouOutsideDiameter/Height/Width.
All of these parameters do not need to exist on every part. Define only those parameters that apply to the part you are creating. For example, to create a straight cylindrical part, you would define only the CATRouOutsideDiameter and CATRouFaceToFaceLength parameters. Optionally you can define CATRouSize instead ofCATRouOutsideDiameter. In addition to the reserved parameters, you may define other parameters on the part. These parameters must also be included in the design table if these parameters have different values for different sizes when the part is placed.. 3. Save the part as a CATPart document. 4. Create the design tables. See the Version 5 Infrastructure User's Guide for detailed instructions on how to create a design table and associate it to a part for which you must use external table files. Excel files are easy to edit, but using tab-delimited text files instead of Excel files makes parts placement more efficient. You can build and edit your tables in Excel, then convert the file to a tab-delimited text file, and attach the text file to your part document.
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routingSystems Design tables are used to manage the allowable combinations of values for the parameters of a part. You must create tables with the following reserved names in order for them to be recognized by the Systems Routing product. (Except external files, see below.) • CATRouFixedSize
This table must contain those reserved run parameters described after Step 2 which you want as fixed size parameters. Your table may contain one or more rows of values, each row generally represents a specific fixed size part. The first row contains the parameter names. They may be reserved parameters or other parameters. Those that are reserved run parameters are used as a key to select the appropriate row in the table. When the part is placed, the values for these parameters are derived from the run. If an exact matching of values on the run and values in the table is not found then the row with the closest match is used. This table must also contain parameters not associated with the run, if any, that are needed to complete the geometry definition. Generally, you may wish to include in your table CATRouPartNumber as the first parameter, CATRouSize as the second, then the other reserved run parameters, then the other part parameters. • CATRouParametricSize
This table is used to define parameters that can be dynamically defined by the run. All parameters in this table must be defined on the run. When a part is placed, the values for these parameters are retrieved from the run and used to size the geometry. If you use external files they can have any name. But when you create the design table in the part document it must have one of the reserved names. 5. Define connector data on the part by following the steps below.
Connector data is used to properly position, align, and orient parts when they are placed on a run. In addition, it is used to properly position, align, and orient a run that is started from a part. a. Start a new CATProduct document. b. Right-click the Product in the specification tree and select Existing Component. The Insert an Existing Component dialog box is displayed. c. Find and select the CATPart document you saved. d. Select the part in the specifications tree. e. Add a connector using the Build Connector command. h. Save the CATPart document.
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All About Connector Data
There are three types of connector data: Face data, Alignment data and Orientation data. Face data is generally defined using a face of the part, such as the circular face at the end of a pipe. Alignment data is generally defined using a line, such as a not shown line along the centerline of a pipe. The actual connection point location is the intersection between the face plane and the alignment line. They do not have to actually intersect: the system will find the intersection location between the infinite line and the infinite plane. The face does not have to be the actual diameter face or width-height face. Orientation data is generally defined using the xy plane, or another plane or face in the part, to define an "up" direction. Face Connector Data. To define the directional planar location for each connection face of the part. If the part is stretchable, two connection face definitions will be used to define the extremity locations of the part. For routing from the part, a connection face (along with the corresponding intersecting alignment line) will be used to define the start point of the run. You should select one of the faces in the part to define a face connection. Select a face that faces outward from the part, in the direction of routing or other attached parts. You must define a face for each connection end of your part. The pre-defined names for face connector data include the following. The names are defined by the connector function. Use the connector function to delete a connector. CATRouFace : for the first or only connection face of a part. CATRouFace1 (same as CATRouFace): for the first connection face of a part. CATRouFace2: for the second connection face of a part. CATRouFace3: for the third connection face of a part. CATRouFace4, 5, 6, etc. CATRouHole CATRouHole1 CATRouHole2, 3, 4, etc. Hole connections are a unique type of face connection. Whereas a pipe or tube may stretch to a face connection, a pipe or tube may pass through a hole connection. This is useful for placing such parts as tubing clamps along a run
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routingSystems without cutting a tube. Alignment Connector Data. To define the alignment at each of the face connections of this part. For placement of an attached part or routing from the end of a part, this data will define the alignment. You will generally select a line for the alignment connector data, which may likely be no-shown. But you may also select a cylinder, and its implied centerline will become your alignment data. Each part connection face does not necessarily need its own alignment line. A pipe and a valve might have one alignment definition, but an elbow would need two alignment definitions. A tee needs two alignment definitions, but could have three. A cross with four connection ends needs at least three alignment definitions. When the number of alignment definitions is less than the number of connection ends, it must be only one less, and alignment1 corresponds with face1 and face2, and alignment2 corresponds with face3. The pre-defined names for alignment include the following: CATRouAlignment: for the first or only alignment line of a part. CATRouAlignment1 (same as CATRouAlignment): for the first alignment line. CATRouAlignment2: for the second alignment line of a part. CATRouAlignment3, 4, etc. Other pre-defined names for alignment include the following: CATRouTop: for top-center CATRouCenter: for center (same as CATRouAlignment) (center is default alignment) CATRouBottom: for bottom-center CATRouLeft: for left-center CATRouRight: for right-center CATRouTopLeft CATRouTopRight CATRouBottomLeft CATRouBottomRight including 1, 2, 3, 4, etc
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Orientation Connector Data. To define the orientation/clocking of a part when placed on a run. Many parts direction, such as horizontal trays and power & free conveyors, require a well-defined "up". Round ducts and pipes do not require a well defined "up" direction, they can rotate. Rectangular ducts do not have a strict "up" direction, but do have four usual orientations corresponding to each of the four sides. Tubing elbows can flip upside down in order to swap end1 and end2, since they often have different end styles. Generally, parts are built in such a way that the Z direction is up. If this is the case, then generally the XY plane can be used to define the orientation. The orientation plane and the face plane should not be parallel. For a particular connection end, you should not define an alignment going up in the Z direction and an orientation plane pointing up in the Z direction. Rarely will an "Orientation2" be needed. Some tubing clamps use an orientation2 because they have one alignment along the tube alignment and another alignment going up through the bolt hole (for stacking). Tray vertical elbows and vertical tees also need an orientation2. The pre-defined names for orientation include the following: CATRouUpOnly: the part has a well-defined "up" direction. (Tray) CATRouUpOnly1: same as CATRouUpOnly CATRouUpOnly2, 3, etc. CATRouCircular: the part has no strict "up" direction. (Pipe) CATRouCircular1: same as CATRouCircular CATRouCircular2, 3, etc. CATRouRectangular: the part has four orientations that can be "up". (Rect duct) CATRouRectangular1: same as CATRouRectangular CATRouRectangular2, 3, etc. CATRouOrientation: same as CATRouUpOnly (up-only is default orientation) CATRouOrientation1: same as CATRouUpOnly1 CATRouOrientation2, 3, etc. same as CATRouUpOnly2, 3, etc. Sample Publication Management combinations for connector data: A pipe or piping valve: CATRouFace1
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CATRouFace2 CATRouAlignment CATRouCircular A piping cap: CATRouFace CATRouAlignment CATRouCircular A rectangular duct elbow: CATRouFace1 CATRouFace2 CATRouAlignment1 CATRouAlignment2 CATRouRectangular An OPF conveyor track: CATRouFace1 CATRouFace2 CATRouBottom CATRouOrientation A tray horizontal tee: CATRouFace1 OR CATRouFace1 CATRouFace2 CATRouBottom1 CATRouBottom1 CATRouFace2 CATRouFace3 CATRouBottom2 CATRouBottom2 CATRouFace3 CATRouOrientation CATRouBottom3 CATRouOrientation A round duct cross: CATRouFace1 OR CATRouFace1 CATRouFace2 CATRouAlignment1
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CATRouAlignment1 CATRouFace2 CATRouFace3 CATRouAlignment2 CATRouAlignment2 CATRouFace3 CATRouFace4 CATRouAlignment3 CATRouAlignment3 CATRouFace4 CATRouCircular CATRouAlignment4 CATRouCircular
A tubing clamp: CATRouHole1 OR CATRouHole1 CATRouHole2 CATRouAlignment1 CATRouAlignment1 CATRouOrientation1 CATRouOrientation1 CATRouHole2 CATRouFace3 CATRouAlignment2 CATRouAlignment2 CATRouOrientation2 CATRouOrientation2 CATRouFace3 CATRouFace4 CATRouAlignment3 CATRouAlignment3 CATRouOrientation3 CATRouOrientation3 CATRouFace4 CATRouAlignment4 CATRouOrientation4
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Creating a Catalog
This task explains how to create a catalog. The Catalog facility is a standard facility provided with the V5 Product line. For detailed information regarding Catalogs, please see the Infrastructure documentation - Advanced Tasks - Using Catalogs. Information that is particular to this product is given here. To properly learn to create a catalog you must read the document referenced above. 1. Open the Catalog Editor by clicking on Start-Infrastructure-Catalog Editor. The Catalog Window opens with a basic catalog structure in the left column. Catalogs are created analogous to books, with the book being at the top level, chapters under it, and, if necessary, sub-chapters under them, and with pages at the lowest level. Each family contains references to one or more parts. The illustration below shows the Catalog Editor. The column to the left is where your chapters and families are displayed. The column to the right will display parts when you click on a family.
If you click the Reference tab you will see the directory path to each part (the file). Clicking the Preview tab displays the part. Clicking the Keywords tab displays the keywords. To add a keyword double click on the family where you want to add it, , and add your information in the Keyword click on the Add Keywords button Definition dialog box that displays. See below on how to add values for keywords. Click here to see a list of keywords. 2. Rename the catalog and chapter and add as many chapters and families as you want to. You can add these later also. Save and close the window and reopen it to see your changes. To rename the chapter, right-click on it and bring up the Definition dialog box. To rename the book, save the catalog, at which time you can rename it.
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3. Add a component to the page. Make the page active and click the Add component button to bring up the Description Definition dialog box. Click the Select document button, navigate to the the component document and select it. Click OK to end. To add values for keywords click the Keywords values tab. A window will display all the keywords associated with that family. Select a keyword and enter the value in the Values field. Keywords and values are case sensitive and you must enter them accordingly.
Making a Catalog Accessible
This task explains how to specify the location of a catalog so that it can be accessed in order to place parts from it. Some catalogs are provided with the application. These are located in the .. intel_a startup components subdirectory.
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routingSystems 1. Click Tools-Options, select General and then the Document tab. Select Other folders in the window and click Configure.
2. In the Other Folders dialog box, double-click on the drive where the catalogs you want are located. This will display all directories in the drive. Navigate to the directory that contains the catalog(s), select one or more, and click Add. All the catalogs you have selected will display in the lower window, as shown in the image below.
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3. Click OK. This will save the search order. Now when you click the Catalog Browser button you will be able to select parts from the catalogs you defined. To change the catalogs that are displayed when you click the Browser button (the search order), you can repeat the steps above and specify different catalogs. You can also use the Export function in the Other Folders box to save the location of other catalogs or groups of catalogs. This will enable you to open them by recalling the search order, rather than having to repeat the steps given above. To do this: 4. Bring up the Other Folders dialog box and navigate to the directory where the catalogs are located. Select the catalogs so that they appear in the lower window. Click Export. The Export Search Order dialog box will display.
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5. Enter a file name and specify a location for the file. Click Save. 6. To recall a saved search order, click Import in the Other Folders dialog box and select the file that specifies the catalogs you want to open. Click OK. This will create a new search order and these catalogs will display when you click the Browser button. 7. Use the Import Add button to add a search order to an existing search order. For instance, if you have a search order open but you want to add to it catalogs defined in another search order, click Import Add, navigate to the directory where the saved file is, and select it. The catalogs in that file will be added to the search order that was open.
Catalog Keywords and Values
You need to add keywords and values for some parts to the catalog to enable certain behavior. The process for adding keywords and values is explained in Creating a Catalog. A list of keywords and values is given below. They should be entered exactly as they are shown in their mixed case (upper and lower case).. The keyword PlaceAndStretch allows parts to bridge the gap between two dissimilar ends, such as a round and square run, or different sized pathways. It has no values. The keyword LoadType affects how a part should be loaded into memory from the catalog. If the keyword is not added then its values is assumed to be NewReference, which is explained below. LoadType has two values. • SameReference -- the part is always an exact copy of the catalog part. Never changes
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•
the parameters of the placed part. NewReference -- the part has parameters that can be changed. New copies of the part will made as needed.
The PlacementType keyword restricts the placement of the part, and can have one of the following values: FreeSpaceOnly -- part can only be placed in free space. Equipment -- same as FreeSpaceOnly, part can only be placed in free space. Inline -- Can be placed at the ends of parts and runs. Reducer -- part is used to change size or shape. Usually placed on the node between two connected, collinear or parallel runs of different sizes or shapes. Reducers can be placed at the ends of runs and parts. Turn -- part is placed on a turn or at the ends of runs and parts. Branch -- part is usually placed at the intersection of two straight segments, where the end of one segment intersects the middle of the other. Branches can also be placed at the ends of runs or parts • • • on straight segments at corners at intersections of the ends of no more than three segments.
When using the multi-place (shift) option, branches will be placed on all intersections on a run that have exactly three pathways. Cross -- part is usually placed at any intersection containing four pathways (e.g. four end segments, or two end segments meeting in the middle of another segment). Can also be placed • • • on the ends of runs on straight segments at corners.
When using the multi-place (shift) option, crosses can be placed on all intersections on a run that have exactly four pathways. Complex branch -- part can be placed at an intersection with more than four connections and anywhere a cross can be placed. Offset -- can be placed at the ends of parts or runs. The part connects runs that are offset from one another. Terminus -- part placed at the end of a run or part (e.g. a cap).
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Coupler -- can be placed on part ends. It is small connecting part, such as a gasket or flange. Support -- placed in the middle of segments, or on the ends of parts and runs. The part is used to support other parts, such as hangers. . Strengthener -- placed in the middle of segments. The part is used to strengthen or stiffen. It can be Nozzle -- can be placed on the ends of parts. Part is used to connect equipment to a part transporting fluid (e.g. pipe).
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Routing MEP Systems
Table Of Contents
Preface ......................................................................................................... 1 What's New? ................................................................................................. 3 New Functionality ........................................................................................ 3 Enhanced Functionality ................................................................................ 3 Using This Guide ............................................................................................ 5 Getting Started.............................................................................................. 7 Setting up the Environment .......................................................................... 7 Routing a Run............................................................................................. 9 Routing Runs in a controlled environment ......................................................14 Placing Parts on a Run ................................................................................18 Saving Documents .....................................................................................18 Basic Tasks ..................................................................................................21 Managing Systems .....................................................................................21 Creating a System Assembly .....................................................................21 Creating a Logical Assembly ......................................................................22 Creating a Logical Set ..............................................................................23 Creating a Path Reservation ......................................................................24 Routing Runs .............................................................................................29 Routing Runs ..........................................................................................29 Routing from the End of a Routable............................................................35 Routing from an Item Reservation..............................................................36 Auto-route Between Equipment .................................................................37 Routing a Run Within a Pathway ................................................................38
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routingSystems Branching a Run ......................................................................................38 Modifying Runs ..........................................................................................39 Using the Definition Dialog Box..................................................................39 Moving or Deleting a Node ........................................................................41 Fixing Broken Routables ...........................................................................44 Connecting Routables...............................................................................46 Disconnecting Routables ...........................................................................48 Break a Run at a Branch ...........................................................................49 Placing Parts..............................................................................................52 Placing Parts in a CATProduct Drawing........................................................52 Detecting Clash in Parts Placement ............................................................56 Creating a Parent-Child Relationship...........................................................57 Using Quick Translate to Move Objects .......................................................59 Layout Tools ..............................................................................................60 Making an Element Active .........................................................................60 Using the Step Input Box and Construction Elements ....................................61 Using Offset Planes and Advanced Offset Planes...........................................63 Flipping Elements ....................................................................................65 Advanced Tasks ............................................................................................67 Advanced Routing Tasks..............................................................................67 Routing a Run at a Slope ..........................................................................67 Routing in 3D with the Compass ................................................................67 Edgeline: Routing Parallel to a Run.............................................................68 Aligning a Run to an Existing Surface .........................................................70 Routing at an Offset of a Routable..............................................................71
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Table Of Contents Routing Along a Spline .............................................................................72 Routing with Defined Nodes ......................................................................73 Advanced Layout Tasks ...............................................................................74 Snapping Elements ..................................................................................74 Mirroring Elements ..................................................................................83 Aligning Elements ....................................................................................85 Distributing Elements ...............................................................................87 Rearranging the Specifications Tree ...........................................................89 Changing the Current Axis ........................................................................91 Disabling/Enabling Manipulation Handles.....................................................92 Generating Detail Information ...................................................................93 Editing Parts ..............................................................................................94 Changing the Reference File for a Part ........................................................94 Change the Parameters of a Part ...............................................................95 Creating and Modifying Connectors ...............................................................97 Create Connectors ...................................................................................97 Using the Compass to Manipulate Connectors ............................................103 Modifying or Deleting Connectors .............................................................103 Creating Duplicate Connectors.................................................................104 Using the Plane Manipulator ....................................................................106 Working with Bendables ............................................................................107 Extracting Bending Data from Bendable Pipes and Tubes.............................107 Design Checks for Bendable Pipes and Tubes .............................................109 Transfer Elements to New Document...........................................................111 Workbench Description ................................................................................115
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routingSystems Workbench Description .............................................................................115 Toolbars .................................................................................................116 Systems Routing Toolbar ........................................................................116 General Design Toolbar ..........................................................................117 Product Placement Toolbar......................................................................117 General Environment Toolbar ..................................................................118 Project Standards .......................................................................................121 Systems Routing Settings..........................................................................121 General Settings....................................................................................121 Display Settings ....................................................................................123 Design Criteria Settings ..........................................................................124 Working in Cache Mode ..........................................................................125 Customizing the Dictionary of User Types..................................................126 Saving a System Assembly or Logical Assembly as a Separate Document .........129 Creating a Catalog....................................................................................130 Creating Parts .......................................................................................130 Creating a Catalog .................................................................................138 Making a Catalog Accessible ....................................................................139 Catalog Keywords and Values..................................................................142
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Preface
The Systems Routing product enables you to create physical designs of HVAC systems, piping systems and other production systems. The main focus of the product is to provide capabilities for preliminary routing of these systems, but capabilities are also provided to evolve the preliminary routing to the detailed production routing. All of this is accomplished through a very simple and highly intuitive interface which combines traditional 2D layout paradigms with the 3D capabilities to allow you to build a full 3D digital representation of the production routing that capture the design intent within the project. The Systems Routing User's Guide has been designed to show you how to create production routing systems within the project. This book provides an overview of the product and illustrates specific design procedures to aid your system routing efforts. Using This Guide
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What's New?
New Functionality
You can transfer elements in a document to a new document or work package. The import node points command allows you to predefine the node points of a run in a document and route using that document.
Enhanced Functionality
Modifying or deleting connectors on the instance of a part is no longer allowed. You can only perform these tasks on a reference or unique part.
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Using This Guide
This book describes how to use the Systems Routing product. Before you read it, you should be familiar with basic concepts such as document windows, standard tool bars, and view tool bars. To get the most out of this guide, you should start with the tutorial in the Getting Started section. It demonstrates how to create some basic elements of a routing system in a hierarchical structure. The remaining sections of the book describe in detail the procedures for using all of the features of the Systems Routing.
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Getting Started
Setting up the Environment
This task explains the setup tasks involved to use the System Routing workbench. You will be perf following tasks: 1. Cache Mode settings 2. Making Catalogs accessible 3. Setting working units and Grid
1. Cache Mode: Deactivate the option 'Work with cache system'. To do this click Tools in the menu bar and In the dialog box that appears, select Project Center - Project - Cache Management. Uncheck the option Work with cache system. Restart the application for the change to take For more information, refer Working in Cache Mode.
2. Making catalogs accessible: Click Tools-Options, select General and then the Document tab. Select Other folders in the w click Configure.
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routingSystems In the Other Folders dialog box, double-click on the drive where the catalogs you want are located. This will display all directories in the drive. Navigate to the directory that contains the catalog(s), and click Add Tree.
Click OK to save the search order. For more information, refer to Catalog's User Guide.
3. Set Working Units and Grid: Select Tools - Options and expand the General node. Select Parameters and Measure then click the Units tab. Under Magnitudes, select Length and click the drop down arrow to set the unit of measure you will be using; Foot, Meter, etc.
8
Getting Started
Now, scroll down the list in Magnitudes and select Area. Select the unit of measure you will be using for area. Note: This is normally consistent with the Length standard.
To set the Grid Step, under Tools - Options, select Engineering - System Routing and click on the General tab. Enter a value for the Grid Step field; for example, 1 ft. The grid step is the increment used for snapping (to grid). Imagine a grid placed over your workspace, consisting of squares. The value you enter in this field becomes the distance between the lines of each square. If you enter 1 ft, then, when routing, the run will extend by 1 ft at a time. Runs begin, end and turn at grid intersections (there are ways of overriding this). Similarly, when placing parts in free space (as opposed to on a run), they will place at grid intersections. Click the OK button to complete the customization of the working units.
The grid step setting will display in the General Environment toolbar at the bottom of the 3-D view change it in the toolbar during your session but the new value will only apply to your current sessi close the application and reopen it, the toolbar will again display the value in the General tab page These will be your default settings and will remain in effect until you change them.
Routing a Run
This tutorial will show you how to use space reservations and route simple runs. The tutorial is div parts. • Creating a network
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routingSystems • Using Space Reservation • Routing a Run
This task assumes the user has setup the environment as described in Setting up the Environmen Creating a network:
1. Start Digital Project and enter "System Routing" workbench. An empty CATProduct docume 2. Click on the Logical Assembly icon on the System Routing toolbar. 3. From the Logical Assembly window, select HVAC Assembly from the dropdown menu. The Assembly system is added to the specification tree.
The Systems and Logical assemblies allow the user in organizing and grouping logical lines. For m information refer Managing Systems. Using Space Reservation: 4. Activate the HVAC Assembly just created by double clicking it in the specification tree.
and browse to the MechanicalSystems.Catalog located 5. Click the Catalog Browser icon $(PrjStdsInsDir)/startup/Catalogs/Systems Routing/, where $(PrjStdsInsDir) = Installation directory of the Project Standards. 6. Select the SpaceReservation object from the Spatial Objects chapter.
10
Getting Started
The SpaceReservation object allows you to place a representative model for various equipments a in routing systems. You can place multiple copies of this object to represent the mechanical equip 7. Place one object in space as seen in the image below. You can change the parameters of th SpaceReservation object to customize it to represent different units in the system. (Use the Edit part parameters command to modify the parameters - Refer Edit Part Parame
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routingSystems Routing a Run:
8. Click the Run button The Run dialog box is displayed.
9. From the Type dropdown, select a Hydraulic run. Click on the Section to modify the section Select a Rectangular section and 'Center Center' as the Set Point. Modify the Envelope dim want to. Click OK on the Section dialog box to return to the graphic window. Do not click OK on the box yet. For detailed information, refer Routing Runs.
12
Getting Started
10. Move the pointer over the face of the SpaceReservation from which you want to route. Wh arrow appears, click and begin to route.
11. Click in free space to continue creating the run. Click once to define the ending point of a s can change the direction of the run after you click in free space. Click twice to end the run.
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12. Click OK in the Run dialog box to create the run.
The green arrows are the Connectors, used to create logical connections between various objects SpaceReservation object and other parts) used in system routing. For more information, refer Man Connectors.
You have created a HVAC network with one run. You can now create additional runs using the same steps described above (Steps 8-12), or you can go on to the task of placing parts on the run.
Routing Runs in a controlled environment
14
Getting Started
This tutorial will show you how to use VirtualSupports and route runs constrained to the environme controlled environment - floor of a house, for instance. In such a practical project you will have to the run will have to be of certain size and shape. In the example below we will use a sample mode environment. The steps involved in this task are: • Placing a VirtualSupport • Constraining the VirtualSupport • Routing a Run
This task assumes the user has setup the environment as described in Setting up the Environment Routing Runs tutorial in the getting started guide. Placing VirtualSupport:
1. Open the sample model file MEPProduct.CATProduct 2. Two SpaceReservations have been placed in the basement of the model. The goal is to rout basement.
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routingSystems
3. Click the Catalog Browser icon and browse to the MechanicalSystems.Catalog located i Routing/, where $(PrjStdsInsDir) = Installation directory of the Project Standards. 4. Select the VirtualSupport object from the Spatial Objects chapter.
The VirtualSupport object allows you to place constraint points for routing ducts and pipes. The me VirtualSupports to the given environment and route runs through them. These VirtualSupports hav runs through them.
5. Place a VirtualSupport approximately in between the two columns as seen in the image belo
16
Getting Started
Constraining the VirtualSupport: 6. Switch to Project workbench. Activate the Constraints toolbar if it is not visible by right clic Constraints toolbar from the contextual menu.
icon on the constraints toolbar. 7. Apply Offset constraint by clicking the 8. Select the vertical plane of the VirtualSupport and the face of the column marked with num 9. Again use the Offset constraint command and select the horizontal plane of the VirtualSupp distance to -1000mm. Change the sign if the support moves below the floor.
Side View Routing Run:
10. Click the Run button . The Run dialog box is displayed. 11. Move the pointer over the face of the AHU_Center unit in the model and select the connecto VirtualSupport. The routing begins. Click on the green arrow of the VirtualSupport pointing to end on the front face of the other AHU by clicking on the green arrow as seen in the ima 12. Click OK to create the duct.
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Thus you have created a duct in a controlled environment. You can later modify the location of the environment, and the duct routing will be updated. More Control can be obtained by placing number of VirtualSupports and constraining them with the
The next task explains you how to place the various mechanical parts and equipments for draw finalized.
Placing Parts on a Run
Now that you have a conveyor run in your network, you can add conveyor parts to the run. 1. Click the Catalog Browser button . 2. Navigate to the Systems Routing/Conveyor directory. 3. Place your parts. See Placing Parts in a CATProduct Drawing for more information on using the Catalog Browser.
Saving Documents
This task contains recommendations on saving your documents.
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Getting Started Ways in which documents are saved are explained in the Infrastructure User's Guide - Creating, Opening and Saving Documents. You must read that documentation because the various methods are not explained here. This task simply suggests the methodology you should follow in specific circumstances. 1. If you are saving a document to a local machine or network drive it is recommended that you use the "Save Management" command initially. The Propagate Directory command (which is in the Save Management dialog box) should not be used routinely. It is meant to be used in specific circumstances, such as when you want to place all the contents of a document in one directory before sending it to another location. 2. If you are saving a document to another site or network you should use the "Send To" command. In this case, you should be careful about the links for documents such as resolved parts folder or line ID. These links could change to reflect the local network drive to which the documents have been sent. You should make sure they point to the original location - using the Reset button in the Save Management dialog box is one way of doing this. 3. You should check the active document before you execute the Save command . The root product must be the active document if you want to save everything under it.
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Basic Tasks
Managing Systems
Creating a System Assembly
This task describes how to create a distribution system. A system assembly is a mechanism for organizing and grouping logical lines. You can create logical lines (such as a Piping Line or HVAC Network) under a system assembly, a logical set under a logical line, and then create runs under them. A system assembly, logical line and logical set will only display in the specifications tree because they are organizational elements. A run will also display in your viewer. In the illustration below, the specifications tree shows a piping system assembly under an area, a logical line (Piping Assembly1) under the piping system assembly, and a run (Pipe Run1) under the logical line. The run can be seen in the area.
1. Click on the System Assembly button. The System Assembly Creation dialog box is displayed. If you want to create the system in a new document see Saving a system assembly or Logical Line as a Separate Document. 2. Click on the down arrow and make a selection in the pull-down menu if you want to designate your system assembly as being of a certain type, i.e. conveyor, piping, power, etc.
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3.
Click OK. If the assembly is not visible in the specification tree, refer Display Settings.
Creating a Logical Assembly
This task describes how to create a logical assembly. A logical assembly is a mechanism used to group runs together. For instance, if you want to organize six runs together you can create a logical assembly and then create the runs under the logical assembly. A logical assembly has a function similar to other lines such as piping and ducts (available under the same menu). A logical assembly is normally created under a system assembly. It can be created under an area if there is no system. 1. Make the appropriate element active in the specifications tree. 2. Select the Logical Assembly icon .
The Logical Assembly Creation dialog box is displayed.
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Basic Tasks
. 3. Select the type of logical assembly you want to create.
4. Click OK.
Creating a Logical Set
This task shows you how to create a logical set. A logical set is a mechanism for organizing and grouping. You can create logical sets under a logical assembly (such as a Raceway Assembly) and then create runs under them. See Creating a System Assembly for more information. 1. Click on the Logical Set button. The Logical Set Creation dialog box is displayed.
2. Click on the down arrow to designate your network as being of a certain
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routingSystems type, i.e. work set. 3. Click OK.
Creating a Path Reservation
This task shows you how to create a path reservation on an area. 1. Make the appropriate area active. See Making an Element Active. 2. Click the Path Reservation button .
The Path Reservation dialog box displays.
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Basic Tasks 3. Define the type of path reservation you want to create.
4. Define the routing mode for the path reservation:
Point-to-point
Orthogonal
Slope
Directional Edgeline Branch at Center: see Branching a Path Reservation In addition, if you place the compass on an object the Use Compass Origin will display. If you click the button and start to route the route button will start from the compass origin. If you are in the middle of routing, the compass origin will serve as a routing point. Click one of the Select Mode buttons - the default is No Filter. The Select Mode buttons allow you to define where you can start routing from. No Filter: No filters are applied and you can route from any routable object or in space.
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In Space: Routing will be in space. This is useful when you have a large object in the background, such as a ship structure, and you want to be able to route in space. Only Part Connectors: Select this to be able to route from part or equipment connectors only. Import Node Points: This allows you to route using predefined node points. See Routing with Defined Nodes for more information.
5. To define Section parameters, do the following: a. Click the Section type button .
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Basic Tasks
The Section dialog box is displayed.
b. Define the section type and the corresponding parameters for each of them:
No Section Rectangular • • • • • Set Point Envelope height Envelope width Display Nominal size
Circular • • • • Set Point Envelope diameter Nominal size Display
Flat Oval. • • • • Set Point Envelope height Envelope width Display
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Radius Corner: Enter or select the: • • • • • Set Point Envelope Height Envelope Width Radius Corner Display
c. The Display buttons allow you to select a display mode of Line/Curve, Solid or Flat.
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Basic Tasks
d. Click the Display Centerline button to show the centerline of the run. This will appear as a dashed yellow line. In addition a dashed blue line will appear to display the Set Point setting. This feature works in all display modes, Line/Curve, Solid and Flat. e. Select OK on the Section dialog box. Instead of entering the type of path reservation, the set point and the height, width or diameter in the Section dialog box, you can select an existing path reservation in your document. Once you select the path reservation the Section dialog box will display the same values as the one you selected. To select, click on the Path Reservation button and then click the left mouse button once on the path reservation whose values you want as the default. Make sure the entire path reservation is selected, and not just one segment or node. It will be easier to select the path reservation in the specifications tree. 6. Optional. Key in a value for the turn radius. 7. Click in the drawing to define the routing points. 8. Double-click the last point to stop routing.
that shows at the beginning of the 9. Click on the Close Loop symbol routable if you want to create a closed loop routable. In a closed loop routable the ends of the routable are joined.
Routing Runs
Routing Runs
This task shows you how to create a run. You can begin routing a run from: • • • • • • Space. An object, such as a tube. The end of a run or middle of a run. A point. Connectors. SpaceReservation face.
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routingSystems 1. Click the Route a Run button The Run dialog box is displayed. .
Click on the down arrow and select the Type of the run. 2. Define the routing mode for the run:
Point-to-point: routing will be directly between two points indicated by clicking.
Orthogonal: routing between two points will proceed first in the X direction, then in the Y direction.
Slope routing: see Slope Routing.
Directional routing: see Routing with a Compass. Edgeline: see Edgeline Routing. Branch at Center: see Branching a Run.
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Basic Tasks
In addition, if you place the compass on an object the Use Compass Origin button will display. If you click the button and start to route the route will start from the compass origin. If you are in the middle of routing, the compass origin will serve as a routing point. Click one of the Select Mode buttons - the default is No Filter. No Filter: No filters are applied and you can route from any routable object or in space. In Space: Routing will be in space. This is useful when you have a large object in the background, such as a building structure, and you want to be able to route in space. Only Part Connectors: Select this to be able to route from part or equipment connectors only. 3. Define the Section parameters: a. Select the Section Type button. The Section dialog box is displayed.
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b. Define the section type and corresponding parameters for each of them:
No Section Rectangular. Enter or select the: • • • • • Set Point Envelope Height Envelope Width Nominal Size Display
Circular. Enter or select the: • • • • Set Point Envelope Diameter Nominal Size Display
Flat Oval: Enter or select the: • • • • • Set Point Envelope Height Envelope Width Nominal Size Display
Radius Corner: Enter or select the: • • • • • • Set Point Envelope Height Envelope Width Radius Corner Nominal Size Display
Double Ridge: Enter or select the: • • • • • Set Point Envelope Height Envelope Width Nominal Size Display
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Basic Tasks The Envelope field refers to the total work area needed.
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routingSystems
c. Select OK on the Section dialog box. The Display buttons allow you to select a display mode of Single, Double or Flat. Click the Display Centerline button to show the centerline of the run. This will appear as a dashed yellow line. In addition, a blue line will appear to display the Set Point setting. This feature works in the Single, Double and Flat display modes. Instead of entering the type of run, the set point and the height, width or diameter in the Section dialog box, you can select an existing run in your document. Once selected, the Section dialog box will display the values for that run. To select, click on the Run button and then click on the run whose values you want as the default. Make sure the entire run is selected - not just a segment or a node. It will be easier to select the run in the specifications tree. If you enter a minimum length or turn radius you will not be able to route correctly unless these values are satisfied. For instance, if you enter a minimum length of 10 feet, you will not be able to complete a segment that is 5 feet. In the illustration below, the green line shows the minimum segment length that will be created, even if you try to make a shorter segment, because the minimum length you entered is longer than the segment you are now trying to create. Similarly, if you enter a value for the turn radius, your run will automatically be adjusted to satisfy the defined turn radius.
6. Click in the drawing to define the routing points. 7 Double-click on the last point to stop routing. You can also click OK in the Run dialog box to stop routing. Click Cancel to abort your routing. 8. Click on the Close Loop symbol that shows at the beginning of the run if you want to create a closed loop run. In a closed loop run the ends of the run are joined.
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Basic Tasks
Routing from the End of a Routable
This task explains how to route from the end of a routable. If you route an element with the same type and parameter values as the "source" element (i.e., the element from which the routable is routed), you can specify whether the new element is a continuation of the source element or a separate element. If you want to use the "Continue" option, be sure that the parent for the source element is active before you begin. 1. Select the Route a Run button . The Routing dialog box is displayed.
2. Define the routing parameters. See Routing a Run for instructions.
3. Move the pointer to the end from which you want to route. When a green arrow appears, click and begin to route. Double click to end routing.
4. Once you begin routing the following buttons are added to the Routing dialog box:
Continue Routing: If you select this the run you create will be part of the run from which you are routing.
Create New Route: If you select this the run you create will be a new run. 5. When starting a run that is a continuation of an existing run, a branch from an existing run, or routing from an object or equipment (nozzle) use either or both of the following buttons as applicable: Get Size/Spec from Selection: If you select this button the run you create will be a new run but will assume the size and specification attributes
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routingSystems of the run or object you are routing from. Get Line ID from Selection: If you select this button the run you create will assume the same line ID as the run or object from which you are routing. If you de-select it, the new run will belong to the line ID displayed in the menu bar.
Routing from an Item Reservation
This task shows you how to route from an item reservation. Click the Route a Run button. 1. 2. Click on the face of the item reservation from which you want to route. 3. Begin routing.
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Basic Tasks The point on the item reservation face from which the run will start depends on the set point of the run. In the illustration above the set point is set at Center Center. If the set point was set at Bottom Center the run would have started at the bottom center edge of the item reservation. To change the set point, click button in the Run dialog box and select the Set Point on the Section Type from the drop down list in the Section dialog box that
displays.
Auto-route Between Equipment
This task shows you how to auto-route a run between two pieces of equipment or two connectors. 1. Make the appropriate element (area, system or line) active by doubleclicking in the specifications tree. 2. Place the two pieces of equipment you want to connect on your area. 3. Click on the Route a Run button and enter parameters in the dialog box that displays. 4. Move the cursor to the first equipment - an arrow displays at the connector point. If the equipment has more than one connector point the arrow will display at different points as you move your cursor.
5. Click to select the starting point of the run. 6. Move the cursor to the second equipment, where the arrow will also display, and click to select the ending point of the run. The run is created over the 37
routingSystems shortest possible path. 7. Press the shift key to see other possible routes for the run between the two objects.
Routing a Run Within a Pathway
This task shows you how to route a run within a pathway.
. The Run dialog bo 1. With your pathway model open, click the Route Thru a Pathway button 2. Click the Section button to open the Section dialog box. Select the type of run, the set point an
3. Click on the pathway in which you want to route your run. This displays set points on the pathw clicking on one of the points. For example, if you select Top Center the run will align to the top Apply in the Run dialog box to see how the run looks and to try different positions. Click OK wh
Branching a Run
This task explains how to branch a run from any of these elements: • • • Another run Boundary Contour
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Basic Tasks • Pathway
If the "source" element (i.e., the element from which the run branches) is moved or resized, the run is adjusted accordingly. 1.With your document open, select the Route a Run button. The Routing dialog box is displayed. 2.Define the parameters for the run. See Routing a Run for instructions. 3. Select the element from which you want to route the run and begin routing. 4. If you want to branch from the center of the segment, click the Branch at Center button in the Run dialog box. The branch will begin from the center of the segment, irrespective of the point in the segment that you route from. If you want to create a run that "branches" from the end of a run, see Routing from the End of a Routable.
Modifying Runs
Using the Definition Dialog Box
This task gives you an overview of the definition dialog box. You can make modifications to a routable using the functions contained in this box. Specific task-oriented modifications are explained elsewhere in this section. You should be familiar with the concepts explained in Routing a Run to be able to take full advantage of these functions. 1. Right click on a routable and, in the drop down menus that display, select the routable and then Definition.
2. This brings up the Definition dialog box.
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3. The Name field allows you to change the routable's instance name. 4. The Section button lets you change section parameters, as explained in Routing a Run. 5. Click one of the Turn Type buttons if you want to change the turn type. • • • 6. No Turn: The turn radius for all turns is changed to 0. The Turn Radius field is not displayed. Uniform Turn: All turns in the run have the same turn radius. Mixed Turn: Turns in the run can have different turn radius.
The Display Error Report button is green
when there is no error in the
run. It turns red when you insert a value or make some other change to cause an error. Click the button to display a report. This error function checks to make sure that the turn radius and minimum length conform to the design rule. 8. The Turn Radius field displays the turn radius. To change it you need to display the Node Definition dialog box (see Moving Nodes) and enter a value. If you introduce an invalid turn radius, by entering a value in the Node Definition dialog box, then the Display Error Report button will turn red. (You can also introduce a turn radius error by shortening the length of one or both segments.) A red arc will also display on your run. The ends of the arc are the minimum point to which each segment should be routed for a valid turn. In the example below, the segment is not long enough to support the turn radius value entered by the user.
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Basic Tasks
9. The Node Edit Table button displays a table containing node values - see Moving Nodes. 10. The Minimum Length field displays the minimum length of each segment. You cannot change the value in this field if you are using design rules. 11. The Total Length field displays the total length of the run. You cannot change the value in this field.
Moving or Deleting a Node
This task shows you how to move the nodes on a path reservation, boundary, or run. In the example below a node will be moved in a pipe run. 1. Place your mouse pointer over the element and click the right mouse button.
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routingSystems 2. From the menu that displays, select the Definition option. This will bring up the Definition dialog box. Symbols are displayed on the pipe run to show the location of nodes: asterisks represent non-connected nodes, and Os (circles) represent connected nodes.
3. To move a node by entering coordinates, do one of the following: • Right-click the node symbol and select Definition from the pop-up menu. The Node Definition dialog box displays.
OR Bring up the (run) Definition dialog box and click the Node Edit Table button to display the Node Edit Table and make changes to values in the table.
• •
Key in new values for X, Y, or Z. Click OK in the Node Definition dialog box.
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Basic Tasks 4.
To move the node using the cursor, place the cursor over the node symbol and drag it to a new location. A line is displayed to show the new location for the segment.
5. Click OK in the Definition dialog box to complete the change. A node will move parallel to the compass base plane, which is normally XY. To move a node vertical to the base, change the compass base to the XZ plane. 6. To move a node parallel to the compass Z axis. • • • Bring up the Definition box for the routable. Place the compass on a 3-D object where it can be manipulated. Change the Z axis to the desired direction. Click on the square around the node and move it with the mouse button depressed. It will only move parallel to the compass Z axis. If you click on the node itself you will be able to move it in any direction.
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routingSystems 7. To move a node of a routable to the origin of the compass. This allows you to move the compass to a specific point on a routable or resource, and then move the node to it. To do this: • • • • Bring up the Definition box for the routable which has the node you want to move. Move the compass to the point where you want the node to move. Bring up the Definition box for the node that will be moved. . The node will move to the Click the Compass Origin button compass base, as shown in the image.
8. To delete a node right-click on the node and select Delete Node from the pop-up menu that displays.
Fixing Broken Routables
This task shows you how to fix - or rejoin - routables in which segments have become separated. In the illustration below, the dotted line - the broken routable indicator - shows that a run has become separated at that point.
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Basic Tasks
You can re-join the run in one of several ways, depending on the nature of the break and your requirements. The methods are as follows: 1.Bring up the Definition dialog box for the run, then place the mouse pointer over the broken routable indicator and click the right mouse button. This will display a pop-up menu. Click Create Segment. 2.Bring up the Definition dialog box, then drag one of the segment handles to re-join the run. 3.Bring up the Definition dialog box. An arrow will display at each end of the broken routable indicator. Drag one of the arrows (depending on circumstances) to re-join the run. In the illustration below, one segment of the run has been moved to connect to the portion of the run still connected to the pump.
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4.In certain cases you will see the Auto Route option beneath the Create Segment option in the pop-up menu (See Step 1). This can happen when a segment connecting two parallel routables (on different X-Y planes) is broken. • Select Auto Route. The Auto Route dialog box will display.
• •
Click on the Toggle button. Options for re-joining the run will be shown as a dotted line. Click OK to make your selection.
Connecting Routables
This task shows you how to connect a routable to another routable. Routables are path reservations, space reservation, boundaries, or runs.
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Basic Tasks
There are two kinds of connections: branch and end-to-end. In a branch connection the end of one element connects to the middle of another. In an end-to-end connection two ends are connected together. In the examples below the two runs will be connected to each other, first as a branch and then as an end-to-end connection.
When you connect two elements one becomes the Employee and the other becomes the Manager. In the example above, if you make the run on the right the Employee and the one on the left the Manager, after you connect them, the Slave will follow the Manager to maintain the connection. The direct method to connect the routable is as follows: Click the Connect button and select one of the elements you want to connect. The element selected first will be the employee and will move to join the manager element. You must click on one of the connector indicators on the employee run. Select the manager element. The first run will move to connect to the manager and the connection symbol will display. Alternatively, you can follow these steps in particular scenarios. 1. Place the mouse pointer over the element you want to designate the Slave and click the right mouse button. 2. From the pull-down menu that displays, select the element you want to modify, in this case Run, and select the Connect Routes option.
3. Select the Master Connector. To select, move your mouse pointer over the run you wish to designate the Master and click on either the support or center line connector. See Information below.
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When you move the mouse pointer over the routable you will see two lines alternatively, as you move the pointer from bottom to top. The solid line is the support line connector, and the dashed line is the center line connector (illustrated below). The second routable will connect to whichever line you select. Select the line by clicking.
4. Select which end of the Slave you want to connect to the Master. The Slave will connect with the Master after you click.
The two elements will connect at the point where the two support or center lines would intersect. If you want to change the position, see Moving Nodes. 5. To make an end-to-end connection replace Step 3 above with the following: Select the Master Connector. To select, move your mouse pointer over the run you wish to designate the Master and click on the arrow that displays at whichever end you want to connect.
Disconnecting Routables
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Basic Tasks This task shows you how to disconnect a routable that is connected to another routable. Routables are path reservations, space reservations, boundaries or runs. 1. If it is a branch connection select the Slave element. If it is an end-to-end connection you can select either Master or Slave. 2. Right click on the element you selected. From the pull-down menu, select the element (XXX.object) you want to modify, in this case Raceway Run, and select the Definition option. The Definition dialog box is displayed, and a small, circular node symbol is displayed at the point where the two runs are connected.
3. Right-click the node symbol. A pop-up menu shows. Select Disconnect.
4. Click OK on the Definition dialog box. The two elements are disconnected. As an alternative, click the Disconnect button where the two runs are connected. , then click the connection symbol
Break a Run at a Branch
This task shows you how to break a run at a branch.
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routingSystems There may be times when you want to move all the segments of a connection at the same time. Breaking runs at branch intersections is one way. When you break runs at branch intersections you create what is called a star connection. In this type of connection (recognizable by a square or diamond-shaped symbol), all the segments joined at a connection will move if you move the connection. In a master-slave connection, the slave will maintain a connection with the master if you move the master. The illustrations below show 1) a run with a star connection; 2) the star connection is moved by dragging with the mouse; and 3) all nodes connected to the star connection move to the new star connection location in order to maintain that connection.
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Basic Tasks
1. Click on the Star Connection button. 2. Click on the routable, system or network you want to convert to star connection. A branch connection symbol connections in the selected element. will display at all branch
A pop-up panel will ask: OK to continue? Click Yes. The connection will be converted. The illustrations below show a branch connection converted to a star connection, with the diamond-shaped star connection showing.
The illustration on the left shows that the main section consists of one segment. But after conversion to a star connection it is broken at the
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routingSystems connection into two segments.
Placing Parts
Placing Parts in a CATProduct Drawing
1. Click on the Browser button. 2. Navigate to the catalog from which you want to select a part.
This task shows you how to place a part from a catalog into a CATProduct drawing. See also Detec
If you want to define a new search path then click Tools-Options, select General and then the Doc search order by clicking on Export, in which case they will stored in a file in a directory you spec
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Basic Tasks
3.
Double-click on directories , to navigate to the page containing the parts. Then double-click on a
4. Click at one or more locations to place the part. NOTE: To place a part, you can also select an e selected. 5.
The different scenarios are discussed: Placing Reducers (straight and branched): You can place reducers (straight and branched) dimension run to get correct orientation of the reducer.
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Placing Reducing Turns: Turns can be placed on runs oriented at 90 degrees. After the turn has connector of the smaller run to get correct orientation of the reducer.
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Basic Tasks
Placing Transitional Reducers: For the transitional reducers provided (round to Rectangular), pla Placing Valves: The same rules as those for straight reducers apply for valves.
Placing Equipments: Equipments will be placed at the end of runs. Some may replace the space
Sometimes the following message will display:
This means that there is more than one type of the selected part in the catalog. The difference ma wanted to place a tee that was 9.6 inches in diameter. If there are two tees in the catalog, one 9 i Part Parameters function. You may also use Flip Part Position if the orientation of the part is reversed.
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Some parts have restrictions attached to them that will not allow you to place them in certain loca
You can choose to display or hide a "preview" of the part you are placing. To do this select Tools obtain the effect you want.
By default, when you click (in free space) to place a part the center of that part will be placed at th to place the origin of the part at the point where you click. To do this click on Tools - Options, sele
No parts can be placed on the run itself. They must be placed either at the ends or at connections. • • To place a part inside an item reservation, press the shift key and click the mouse button. To place a part on a face of an item reservation, click the mouse button.
Detecting Clash in Parts Placement
This task shows how you can detect clashes between parts when you are moving parts in a document. This function only works when you are placing/moving parts in free space. It will not work if the parts have been placed on a run, for instance. Three modes are available: Clash Detection Off; Clash Detection On, and Clash Detection Stop. 1. To turn clash detection off click the Clash Detection (off) button . This is the default mode. 2. . To turn clash detection on click the Clash Detection (On) button When you move a part in such a way that it interferes with another part, a red outline will display, as in the images below. (If your part displays red highlights and you want to change the color you can do so by clicking Tools-Options-Display and selecting another color.)
3.
To change to the stop mode click the Clash Detection (Stop) button . When this mode is on you will not be able to move a part to a position in which it interferes with another part. In the first image below the pump
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Basic Tasks has been stopped because it interferes with the heat exchanger. However, when the user moves his pointer to the other side, and there is enough room for the pump, the pump will appear on the other side of the exchanger.
Creating a Parent-Child Relationship
This task shows you how to create a parent-child relationship between two elements. This function can be used to create a relationship between resources, between a resource and an element like an area; or between products in a process. The example below uses electrical parts and robots. The procedure is the same for all types of objects and elements. 1. Click the Attach button 2. Select the parent (or master) element. 3. Select the child (or slave) element. The attachment is created. If you move the child, the connection between the two will remain; however, unlike a master-slave relationship, the child element will not snap back to its original position. If you move the parent the child will follow.
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4. To hide all the Parent/Child symbols and text (attachments) in a product, click the Hide Attachment button, then click the Product in the specifications tree. All attachments in the product will disappear.
To hide individual attachments, click the Hide Attachment button, then click the object. The attachment will be hidden. If a local Attachment is selected, e.g., an attachment between two elements in a product, only that attachment is hidden or shown. If a Product is selected you not only Hide/Show all attachments of the selected product but also all attachments to the children of the selected product. If you open a product and don't know if there are existing attachments, click the Swap Visible Space button been hidden. to reveal any attachments that may have
5. To show all previously hidden attachments, click the Show Attachment button, then click the Product in the specifications tree. All attachments will be shown. To show a previously hidden "local" attachment, click the Show Attachment button, then click the object or select it in the specification tree. The attachment will be shown. 6. To delete an attachment select it and use the delete key.
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Basic Tasks
Using Quick Translate to Move Objects
This task shows you how to use the Quick Translate command to move elements. This function allows the user to transfer an element relative to a location on another element by any of the following alignment methods: • • • • • • Point-to-Point Point-to-Line Point-to-Plane Plane-to-Plane Plane-to-Point Line-to-Point
An object or element moved using this command does not rotate. 1. With your document open, click on the Quick Translate button . The Translate dialog box opens. Depending upon which From element you select the available To elements will either be grayed out or become active.
2. Select the type of transfer, Point-to-Point, Point-to-Plane, etc. Using the Point-to-Plane method as an example, select a point on the From element in your document and select a plane on the To element.
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3. The transfer occurs when you click on the To element. Click the Update button, if necessary. In this case, the object or element has moved, aligning the selected point with the selected plane.
4. The function works similarly with the other From/To selection methods and may be applied as the design dictates.
Layout Tools
Making an Element Active
This task shows you how to make an element in a drawing active. An element is active when it is highlighted in blue in the specification tree, as shown below.
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Basic Tasks
1.
You can make an element active by following any of these steps: • Double-click the element in the drawing or in the specification tree.
• • •
Select Activate Parent button parent active.
to make the active element's
and then To activate an area, select the Activate Area button select any element under the area. To activate a network, distribution system or logical set, select the Activate Network button the network. and then select any element under
2.
Optional. You can change the display of elements that arenot active using the Toggle Dimming Mode button on the General Environment Toolbar: When Dimming Mode is on, elements that are not active are dimmed. When Dimming Mode is off, inactive elements are not dimmed.
Using the Step Input Box and Construction Elements
This task shows you how to use the step input box and construction elements for more control over routing and placing of resources and item reservations. The value entered in the step input box is used for accurate routing and resource placement. You can only route in multiples of the value in the step input box. If the value is 0.25 meters you cannot create a run that is 0.33 meters in length, but you can create runs that are 0.50, 0.75 meters and so on. The value in the step input box works with some of the construction elements to further refine your routing and resource placement, as explained below.
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routingSystems 1. To enter a value in the step input box, select the increment field and key in a value. You can also click on the down arrow and select a value, if it is appropriate for your task. The following sections explain how the step input box is used together with some of the construction elements. 2. Click on the down arrow and select Snap to steps off current axis button. This allows you to snap to points that are multiples of the value entered in the step input box measured from the current axis (also called origin). As you move your mouse pointer a label will show the distances (coordinates) from the current axis in multiples of the value entered in the step input box. In the illustration below, the label is showing that the distance is 500 mm from the axis along the X axis, and 500 mm from the axis along the Y axis. When routing you will only be able to create segments whose length is in multiples of 500 mm. Similarly, you will only be able to place (or move) a resource at points that are measured in multiples of 500 mm from the axis. You can change the value in the step input box at any time.
3. Snap to steps off last position . This will allow you to snap to points that are multiples of the value in the step input box measured from the last point at which you clicked. When you select this option the label will first show the distances from the current axis. After you click, it will show the distances from the last point where you clicked. You can change the value in the step input box after a click if you want to route a segment of a certain length, or place a resource an exact distance away from where you last clicked. 4. . This option allows you to snap to the Snap to XY construction planes XY grids on a construction plane. You first create a grid using the Construction Planes command. If you have an XY grid you will only be able to place resources at, or route to, the intersections of X and Y grids. If you have only X or Y grids you will only be able to place resources at, or route to, the grid lines. 5. Snap to all construction planes snap to the X, Y or Z grids. 6. Snap to elevation planes . Selecting this option allows you to snap to the elevation planes of a Z grid. In the illustration below the user is routing on the Z axis and snapping to the elevation planes of the Z grid. . Choosing this option allows you to
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7. Snap to Drafting elements . This option is used when attaching the drafting view of a 2D drawing to an area. By using this option you will be able to snap to the elements of the 2D drawing. For instance, if you are attaching the 2D drawing of a conveyor belt to an area, by choosing this option you will be able to use the Conveyor Reservation function to select the drawing (you select by clicking on different elements of the drawing). This will allow creation of an identical conveyor layout in 3D.
Using Offset Planes and Advanced Offset Planes
This task shows you how to define a plane to use as a temporary reference for positioning other elements. The second part of the document explains the use of an advanced offset plane, which allows you to define origin, orientation and other parameters. 1. Select the Offset Plane icon . 2. Define the reference plane by doing the following: a. Place your cursor over a geometric element that defines the plane (e.g., a construction plane, boundary, area contour, item reservation). As you move the cursor, a small white rectangle is displayed to show the selectable planes, as shown below.
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If you do not see the white rectangle, zoom out from the drawing. The white rectangle cannot be displayed if the element under your cursor is displayed too small. b. Click to select the plane. The white rectangle changes to a blue rectangle, and remains displayed on the reference element, as shown below.
The reference plane can now be used as a reference to position other elements. 3. Use the advanced offset plane feature to set your plane reference, origin and orientation settings as follows: a. Click the Advanced Offset Plane button. The Define Plane dialog box will display.
b. The Define Plane button is selected by default. However, you can select any button in the
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Define Plane box. Click when you have found a location. The plane manipulator displays.
Click on the buttons in the Define Plane dialog box to make your selections. See Creating Connectors on using the buttons. c. Click OK when done. The reference plane will be created.
Flipping Elements
This task shows you how to flip a part that has been placed in a document. 1. 2. Click the Flip Part Position button. Select the part you want to flip. The part is flipped.
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Advanced Tasks
Advanced Routing Tasks
Routing a Run at a Slope
This task shows you how to route a run at a slope. 1. At the point in your run at which you want to slope it click the Slope button in the Run dialog box. 2. Enter the degrees of slope you want.
Click the Section button and enter data about the type and size of run. 4. Continue creating your run. Click once to define the ending point of a segment. Click twice to end the run.
3.
Routing in 3D with the Compass
This task shows you how to use the compass to route in any direction. Click the Route a Run button. 1. The Routing dialog box is displayed.
2. Click the Directional Routing button. Select the type of run and enter other values. See Routing a Run for more 3. details.
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routingSystems 4. Click at the point where you want to start your run from. This places the compass at that point.
To begin routing click and drag the compass so that its Z axis (it may read W) is pointing in the direction in which you want to route. To change direction, drag the Z (or W) axis of the compass, or press the Shift key repeatedly until the desired axis is highlighted.
5. Double click, or click OK to end your routing. You can also double click on the compass to bring up the Compass Manipulation dialog box, which allows you to enter values to modify compass direction and/or location.
Edgeline: Routing Parallel to a Run
This task shows you how to route parallel to, or at an offset of, a routable. See also Routing at an Offset of a Routable and Position Segment Relative to Plane. This function is used when you have an existing run and want to route parallel to it, or at a certain clearance from it. It is sometimes known as edgeline routing. You can also place an offset plane on a surface and use it as a reference point. 1. Display the run you want to route parallel to and click the Run button . The Run dialog box displays. 2. Click the Edgeline button . The Distance field will display and the Offset and Clearance buttons will appear in the Run dialog box.
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If you click the Offset button the distance between the two runs will be measured from centerline to centerline. If you click the Clearance button the distance between the two nearest edges will be measured. If there is a part on a piping or tubing line the distance will be measured from the part. If there is no part the distance will be measured from the line. 3. Enter the distance between the two runs. If you enter 0 and click the clearance button, the two runs will touch at the edges. 4. Click at the starting point. The compass will display at that point. 5. Move the compass so that the Z axis points in the direction that you want to route, which should be in the direction of the run that you want to parallel. You can do this by moving it manually, or by clicking the second mouse button once and then toggling the shift key. 6. Once the direction is selected, route toward the run you want to parallel. When the centerline of the target run is highlighted, press the Shift key to toggle between various "solutions," or various sides. In the images below there are only two solutions and you can route on two sides of the target run.
7. Select the target run after you have decided which side you are routing on.
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routingSystems 8. Begin routing and double click to end. The finished run is shown below.
You can place an offset plane on a surface and use it as a reference to route parallel to, or to keep a certain clearance from. After placing the offset plane use the procedure described above.
Aligning a Run to an Existing Surface
This task shows how to align a run to an existing surface or edge while in directional routing mode. This function uses the compass to align a run to the surface or edge. It is assumed that you have taken the steps necessary to start a run. See Routing a Run on an Area. 1. In the directional routing mode move the compass that shows at the end of the run to the edge whose angle you want to emulate.
2. 3.
The Z axis of the compass (it may read W) assumes the angle of the edge against which it is held. At the same time the last segment of your run assumes the angle of the
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Advanced Tasks compass' Z axis. Click once at the end of the segment to move the compass back to it. You can repeat the action to make the run align with any other edge or surface in the area. Double click to end the run.
4.
5.
Routing at an Offset of a Routable
This task shows you how to route a run at an offset of a routable. This function allows you to create a run paralleling an existing run, a defined distance apart. 1. Click the Create an Offset Route button. The Run dialog box displays.
2. Select a segment of the run to which you want an offset. The compass is placed on the segment. 3. The direction in which the Z axis of the compass is pointed determines where the new run will be placed: you can place the new run or runs to the inside, to the outside or stacked on top of the existing run by adjusting the compass. 4. Enter your options in the Run dialog box. or Constant Clearance button. If Click either the Constant Radius you click the Constant Radius button the radius of the turns will be maintained but the offset may vary. If you click the Constant Clearance button the offset will be maintained but the radius of the turns may change. Select one of the Offset Between buttons to indicate whether you want the offset measured from outside edge to outside edge, center line to center line or center line to outside edge.
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A negative offset may be entered to offset in the opposite direction to the compass Z direction. 5. Click OK. The offset run(s) will be created. In the illustration below the run has been created with the Constant Clearance option.
Routing Along a Spline
This task shows you how to route along a spline. This process applies to all routables, such as runs, pathways, and functional path reservations. 1. Import the model which contains the spline into the Piping Design workbench.
2. Click on the Route from Spline button. 3. Select type of run and enter other options. Note: The SAG option is used to define the maximum distance a segment can be from the spline. The run that is created consists of straight segments, as you can see in the illustration below. The smaller the SAG number entered, the closer the run will resemble the spline. But this will also cause more segments to be created. 4. Select Create connection to curve if you want a connection between the run and the spline. If this option is checked the run will move if the spline is moved. 5. Click on the spline. The run is created.
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Advanced Tasks
Routing with Defined Nodes
This task shows you how to route a run with predefined node points. You can create a run by predefining the node points. This means you do not need to route the run by clicking the mouse pointer in the 3D window, as explained below. See Routing a Run for basic information. 1. Create a text file, using a text editor like Wordpad, with column headings as shown below, and define the node sequence, X/Y/Z coordinates and bend radius of the node points. A sample file is provided with this application to help you define the text file. The file name is RunInputNodeData.txt and the location is: ...intel_a\startup\EquipmentandSystems\MultiDiscipline\SampleData. The file is reproduced below to show you the column headings and layout. (It has been opened in Excel to make it easier to distinguish columns.
You can see that there are two sets of node numbers, ranging from 1 to 4. Whenever the application reads the node number 1 it will start a new run. So, based on the file above, two runs will be created.
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. The Open the Run dialog box and click the Import Node Points button File Selection dialog box displays. Navigate to the location of your file and select it. The runs will be created.
Advanced Layout Tasks
Snapping Elements
Snap Resources Together
This task shows you how to snap two resources together. Resources can be joined at existing connectors, you can create new connectors to join them, or you can snap them together without using connectors. All procedures are described below, beginning with the procedure for snapping resources in which you create connectors. To snap resources together by creating new connectors, click the Snap . 1. button 2. Click one of the resources you want to snap together. The resource changes
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Advanced Tasks color and the Define Reference Plane (From) dialog box displays.
By default the Define Plane button is selected, allowing you to select a plane for the connector you will create. See Creating Connectors for information about using the Define Plane functions. The two resources will have a Master-Slave relationship to each other - but only if you choose to add a constraint (see below). If you add a constraint the first object you select becomes the slave, and the second object becomes the master. Also note that the first resource you select will move to snap - the second resource you select remains stationary. 3. Select the second resource. The Define Reference Plane (To) box will display - make your selections as explained above. You can also select an existing connector. Click OK when done. The two resources will snap together and 75
routingSystems the Constraint Options dialog box will display. 4. You can clear the Align, Face and Orientation check boxes and click OK if you want the two resources to remain snapped together without any new connectors being created. To add one or more constraints - which will also result in creating connectors - follow the steps given below. 5. Make your selections in the Snap Options box.
Align: You can increase distance between the two resources, but if you change the alignment the slave will snap back to the original alignment. In the image below the distance is increased but the alignment remains the same.
Face: The two resources will maintain the face if you move one of them. In the image below the two maintain the same face, though the alignment has changed.
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Orientation: The two connectors will maintain the same orientation if you move them, i.e. the red arrows visible in the connectors will align. It is therefore important to make sure that the red arrows in the connectors are pointed correctly and oriented correctly with reference to the part. The red arrow is usually set to the "Up" position of the resource, which means that on both resources they should point in the Up direction. If the red arrow points "down" in one resource and "up" in the other, then the resources will snap together incorrectly. You can toggle the position of the red arrow by clicking on the green arrow that is parallel to the plane. Fix in space: If you select this option the position of the master resource is fixed - if it is moved it will snap back to its original position. Attach: Checking this option allows you to attach the two objects. Place manipulator at snapped location: Check this if you want to rotate the snapped object after placing it. The manipulator is placed on the object if you check this. You can then click on the bottom curve of the manipulator (see image below) and rotate the object. It will rotate in increments, based on the value entered in the Snap Angle field. In the image above it is 45 degrees.
To remove a constraint select it in the specifications tree and delete it. To remove the 'Fix in space' option right click on the Fix line in the specifications tree, click Properties, go to the Constraints tab, and uncheck the Fix in space box. 6. Click OK when done. 7. To snap resources together using preexisting connectors: a. Click the Snap button. b. Move the pointer over the first resource - the connectors will display.
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routingSystems Select the connector. c. Move the pointer over the second resource - the connectors will display. Select the connector and the two resources will snap together. d. The Snap Options box will display. Make your selections and click OK.
Quick Snap Resources
This task shows you how to Quick Snap two resources together. The Quick Snap procedure allows you to snap two resources together using one of three selection methods. You can select the snapping point on one of the resources using one of these methods. On the other resource the snapping point will either be its origin, or at a connector, as described in Step 2. The three selection methods are: • • • Center of three points (on a circle): the snapping will be the center of three points indicated by you. Center of polygon: the snapping point will be the center of any surface indicated by you. Surface: the snapping point is at any point indicated by you.
The three methods are described below. To snap resources together using the center of three points on a circle 1. method, click the Snap Three Points button .
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Advanced Tasks 2. Click the resource that you want to move. Note: • • • If you click the resource at a connector it will snap to the other resource at that connector. You can create a connector if you want to. If you click the resource at a point other than a connector it will join to the other resource at its origin. If the resource was preselected when you clicked the snap command you will not be able to select a connector.
These points apply to all three methods of Quick Snap. In the image below the user wants the paint gun to snap to the robot arm. After he clicks the paint gun the compass displays at the origin of the paint gun to show that the part will snap at that location. You can choose not to display the compass at the snap location by unchecking the option Place compass at snapping point in the Snap Options dialog box. The box displays when you click on any of the Quick Snap buttons. Placing the compass at the snapping location allows you to rotate the resource after it has snapped.
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routingSystems 3. Define the point on the robot where you want the paint gun to snap, in this case the end of the robot arm, by clicking on three points. You can only select your defining points on the edges of a circle. Only points on the ends of edges are selectable. Note: If you click the three points clockwise the paint gun will attach "inward" as shown in the image below:
If you click counter clockwise then the paint gun will attach "outward", which is the correct position in this example.
4. To Quick Snap using the center of polygon method, click the Snap Center of Polygon button and perform the action detailed in Step 2.
5. Select the snapping point on the second resource by clicking on a surface. The resource will be placed in the center of the polygon.
6.
To Quick Snap using the surface method, click the Snap Surface and perform the action detailed in Step 2.
button
7. Select the snapping point on the second resource by clicking on any surface. The resource will be placed at the point you click. If you double click a command you will be in repeat mode. This allows you to snap a resource to a different location, using a different selection method if you want.
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Advanced Tasks
Snap and Rotate a Resource
This task shows you how to rotate a resource after snapping it to another resource. 1. With both resources on the screen, click on the Snap resource. The orientation symbol will appear. button and then on a
2. Click on the second resource. A white square will appear. Move the pointer over the resource and click when the white square is at the location where you want to snap the two resources. The orientation symbol will appear at the location and the Define Reference Plane dialog box will display.
3.
Click on the Define plane using compass button . The compass will be placed at the location where you want to snap the two resources.
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4. Click OK on the Define Reference Plane box. The two resources will snap together.
5. Click on the Select button to exit the Snap command. Click on the resource you want to rotate, then grab one of the handles on the compass with your pointer and move it. Different handles will move/rotate the resource in different directions.
You can also double click on the compass to bring up the Compass Manipulation dialog box and enter the required figure in the Angle field. Click on the + or - sign next to the Z axis to rotate it.
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Advanced Tasks
Mirroring Elements
This task shows you how to move one or more elements to the opposite side of a selected plane, as a mirror image. It also shows how to copy one or more elements to the opposite side. 1. Select the element(s) you want to move. (You can also select after Step 2.) 2. Click on the Mirror button . 3. The Reference panel will display if you already have a reference plane defined (by having used the offset plane command).
Click the New Reference Plane button and follow Step 4 if you want to define a new reference plane. Follow Step 4b if you want to use the existing reference plane. The Reference panel will not display if you do not have a reference plane already defined. 4. Define a reference plane across which to mirror the element by doing the following:
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routingSystems 1. Place your cursor over a geometric element that defines the plane (e.g., a construction plane, boundary, area contour, item reservation). As you move the cursor, a small white rectangle is displayed to show the selectable planes, as shown below. If you do not see the white rectangle, zoom out from the drawing. The white rectangle cannot be displayed if the element under your cursor is displayed too small.
b. Click to select the plane. The selected elements are mirrored to the other side of the plane, as shown below.
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5. To Mirror and Copy the elements, follow the steps outlined above and then click the Mirror and Copy icon . The selected elements will be copied to the other side of the plane. In the illustration above, the selected elements will stay where they are and two similar elements will be added to the other side of the plane.
Aligning Elements
This task shows you how to align elements in your layout. You can align the center or the sides of an element to a user defined reference plane that you define. You can also rotate an element to align it with a reference plane. 1. Select the element(s) that you want to align. 2. Select the icon for the type of alignment you want to perform:
Align Sides: aligns the sides of two or more elements
Align Center: aligns along the centerlines of two or more elements
Rotate to Align: rotates elements on the axis to align them
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Align Planes: aligns selected planes
Distribute: See Distributing elements 3. Define the plane to use as a reference for the alignment. If you have an offset plane already defined it will be used as the reference plane. If you do not already have the offset plane defined do the following: a. Place your cursor over a geometric element that defines the plane (e.g., a construction plane, boundary, area contour, item reservation). As you move the cursor, a small white rectangle is displayed to show the selectable planes, as shown below. A line normal to the rectangle shows the direction in which the alignment will be performed.
If you do not see the white rectangle, zoom out from the drawing. The white rectangle cannot be displayed if the element under your cursor is displayed too small. b. Click to select the plane. The selected elements are aligned along the plane.
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Advanced Tasks
4. Using the Align Planes command allows you to select any plane on an item reservation or part. After you select the first plane to which to align to, you can only select a plane that is parallel to it. For instance, if you select the the top of an item reservation you need to select the top or bottom of the second item reservation - you cannot select the sides. Click any button in one of the tool bars to exit the alignment command. If you want to continue with the alignment command using the same reference plane then select another element in the model.
Distributing Elements
This task shows you how to distribute elements within parameters that you define. 1. Select the elements you want to move. 2. Click the Distribute button . 3. Define a reference plane for the distribution by doing the following: a. Place your cursor over a geometric element that defines the plane (e.g., a construction plane, boundary, area contour, item reservation). As you move the cursor, a small white rectangle is displayed to show the selectable planes, as shown below. A line perpendicular to the rectangle shows the direction in which the distribution will be performed.
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routingSystems If you do not see the white rectangle, zoom out from the drawing. The white rectangle cannot be displayed if the element under your cursor is displayed too small.
b. Click to select the plane. The selected elements are distributed along a line perpendicular to the plane, as shown below.
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Advanced Tasks
Rearranging the Specifications Tree
This task shows you how to transfer elements in your layout from one level of the specifications tree to another. 1. Make the appropriate element active.
You must make active an element that is at least one level higher than both the source element (i.e., the one that is being transferred) and the target element. For example, in order to transfer ArrBox5, ArrBox6, ArrBox7, ArrBox 8, and ArrBox9 to ArrArea3, shown below, ArrArea1 or Product1 must be active.
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2. Select the elements you want to transfer.
Select the Transfer Elements in Tree button . 4. Select the element to which you want the elements transferred. The target element must also be a child of the active element.
3.
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The elements you select in Step 2 become children of (i.e., subordinate to) the element you select in Step 4.
Changing the Current Axis
This task shows you how to change the current axis. When you activate an object, the current axis is reset to the axis of that object. Changing the current axis changes the reference point by which elements are 91
routingSystems routed and placed. . 1. Click the Change Current Axis icon 2. Select the object you want to use as a reference. The axis for the selected object is displayed. 3. You can also change the current axis and place the compass on the object. The compass allows you to manipulate that object. To do this click the Change Current Axis and Snap Compass button The axis and compass are both placed. and select the object.
Disabling/Enabling Manipulation Handles
This task shows you how to disable or enable manipulator handles using the Toggle Manipulator Handle Mode command. The default is for the manipulation handles to be enabled. If you are working on a large document, however, displaying the handles on each part can take up time. If you do not need the handles then you can use this feature to disable the display. It is a toggle button, so clicking it again will enable the handles. This feature can be used with parts placed in-line or in free space. To disable display of the manipulation 'handles' click the Toggle Manipulation 1. Handle Mode button . To enable them again click the button once more. The handles look like a green box on parts placed in free space. On parts placed in line they look like the image below.
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Advanced Tasks
Generating Detail Information
This task shows you how to display detailed information about objects as you move the pointer over them. The Analyze Item command displays information about an object when the pointer passes over it. This information can include line IDs, nominal size of runs and parts, XYZ coordinates of connectors, etc. The type of information shown will depend on the object and the product you are using. See also Display Information About Routables. From Release 13 the angle of routables from the x,y,z axis will also display, as in the image below.
1.
With your document open, click the Analyze Item button . 2. Move the pointer in the document highlighting various objects. Attributes and their values are displayed, depending on the type of object highlighted. In the illustration below the pointer is on a tubing tee.
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3. When you click again the feature will be disabled.
Editing Parts
Changing the Reference File for a Part
This task shows you how to change the reference file for a part. When you place a part in a document, each part has a reference file associated with it. This file contains data about that part. To save disk space, the application normally uses one reference file for all similar parts - an elbow that has been placed nine times in a document will have one reference file for it. It also means that you cannot change the dimensions of one or more of those elbows. This function allows you to create a unique reference file for one or more parts, allowing you to assign unique parameters to them. Using this function you can: • • 1. With your document open, click the Change Part Reference button Change Reference dialog box will display. . The Assign a unique reference file to a part. Assign a part the unique reference file (and parameters) of another part.
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2. If you have already selected a part a file name will display in the file name field; if not it will display when you select a part. If you want to change the file name make sure you have not already assigned it. 3. Click OK. 4. To assign an existing unique reference file to a part: If one of the parts in your document already has a unique reference file you can assign it to other parts. Select the part or parts to which you want to assign a reference file; click the Select New Reference button in the Change Reference box; then select the part that has the unique reference file. You will see the file name change to the unique reference file name in the specifications tree.
Change the Parameters of a Part
This task shows you how to change the parameters of a part.
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routingSystems 1. Select the part, in this case an elbow, at the end of a run and click the Edit Part Parameters button . This will display the Parameter Explorer dialog box.
2. The box will display a list of parameters that can be edited for the part you selected. Select one of the parameters. 3. If it is possible to change this parameter by entering a value in the Parameter Value field then do so. If the Value field is grayed out then click the button to the right of it
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4. A dialog box will display, displaying the values that can be selected. Select one of the values.
5. Click OK to exit the dialog boxes. These are the only commands relevant to the change part parameter procedure. Other buttons and fields on the Parameter Explorer dialog box are meant for other functions and should not be used.
Creating and Modifying Connectors
Create Connectors
This task shows you how to create a connector. Connectors can only be created on objects that have existing geometry that satisfies the rules of connector creation. If existing geometry is not present, you will have to create the geometry. 1. If the resource is not active, make it active by double-clicking in the specifications tree. Click the Build Connector button. This will bring up the Manage Connectors 2. dialog box. You will not be able to add a connector on the instance of a part using the Add command in the Manage Connectors dialog box. You can only add connectors on the reference of a part (the part in the master catalog), using the Create Part command. However, you can add a connector to a unique part using the Manage Connectors dialog box. The Manage Connectors dialog box will list all connectors on the selected part. To see a connector and its associated geometry on the part, select a connector from the list. Adding a connector is explained below; Delete, Modify and Duplicate are explained elsewhere in this section. To Publish a connector means you are
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routingSystems allowing people who do not have write access to your document to establish a connection. This is explained further in Using Work Packages. You can Publish or Unpublish connectors using the two buttons.
3. Click the Add button. The Add Connectors box displays.
Select the type of connector - piping, HVAC, etc. In some applications the flow direction field will be available. The piping (or tubing) part connector has flow direction built in and you must select a flow direction also from the drop down menu. The mechanical part connector has no flow direction. 98
Advanced Tasks
Another type of connector - the nozzle connector - will be available if you are placing a connector on a nozzle. A nozzle connector must be placed on the end of the nozzle that connects to equipment. A part connector is placed on the end that connects to the pipe or duct. An electrical part connector should only be placed on a socket. The electrical part connector should be placed on the end of the socket that connects to equipment. A cableway part connector should be placed on the free end of the socket that does not connect to equipment. When you are placing a connector on a Bendable, such as a bendable pipe, you must use the Define New Geometry option. You must not use existing geometry to place the connector. You can name each connector by selecting in the Name field. This is useful for some functions, such as designing using a schematic. The concept of Publishing or Unpublishing a connector is explained above. Check the checkbox as necessary. Face, orientation and alignment are explained below. The orientation, alignment and face must be defined correctly before a connector can be created. To explain what these are, the face is the surface to which you attach a connector. As an example, if you want to attach a clock to your office wall, the wall is the face. You want the numeral "12" to be up, so you orient the clock accordingly. This is the orientation. The alignment is the direction in which the clock face is pointed - normally it would be perpendicular to the wall. When creating a connector, the alignment always has to be perpendicular to the face. The face is generally defined using a face of the part, such as the end of a pipe. Alignment is usually defined using a line, such as the not-shown line along the centerline of a pipe. Orientation is defined using the xy plane, or another plane or face to define an "up" direction. In the illustration below the Z axis indicates the alignment of the connector. It also indicates the direction in which routing will occur. The X and Y axis together define the orientation. They are useful when attaching two resources.
It is necessary to select geometry in the part to which you want to attach a connector so that these three characteristics are correctly defined. If the part does not have the necessary geometry then you must create it.
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routingSystems 4. If you want to create a connector using the part's existing geometry click the Use existing geometry option. Click the Select Face button to select a face. Selectable faces will highlight as you move your pointer over the part.
Click this button to select the alignment. You will only be able to indicate the alignment by selecting a line - from the construction geometry, or elsewhere in the part if there is one. You can only select a line that is perpendicular to the face plane. Click this button to select the orientation. You will only be able to select a plane that is perpendicular to the face you selected. If you cannot find a plane to select, click the Swap Visible Space button (see below) to make the construction geometry visible, and select a plane.
Some connector types require you to place a datum point. The datum point is placed by clicking this button and then clicking a 3-D point on the part. The datum point is used as follows: • • • Lofted reservation section: Datum is used to define where the spline will start and end when creating lofted reservations. Tubing & waveguide parts: Datum is used to define where the spline will start and end when creating flexible tubes. Hangers: See Hanger Design documentation.
You can display the part construction geometry, if there is any, to make it easier to select existing geometry. Do this by: • • • Right click on the part entry in the specifications tree. Click Hide/Show. The part will disappear from the screen. . The part will reappear on Click the Swap Visible Space button your screen with the construction geometry visible. Clicking the button again will toggle you back.
5. The fields under Classify Connector will become available after you have successfully selected the geometry explained in Step 4. Click on the down arrows to make your selection. Select a type.
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For Flow direction, select In, Out, InOut or None. Select the Face type. A Hole connection allows a routable to pass through it it is useful for placing parts like clamps along a run without cutting a tube. A Face connection will stop a routable and not allow it to pass through. Select an alignment. Choose an orientation: Circular will allow the connector to attach to another connector at any orientation; round ducts and pipes, for instance, do not need a well-defined "up" direction because they can rotate. A Rectangular orientation is used for parts like rectangular ducts; they do not have a strict ''up" direction. Up allows the connector to attach to another connector or part in the up position: horizontal trays, for instance, require a well-defined "up" position. You can also use the "up" orientation for a hole connector. In the image below, the connector on the right has the up orientation, the connector on the left does not.
The number in the Number field is assigned by the application. This can be significant because when you are creating a new connector, you have the option of using the alignment and orientation used in the previous connector after you select the face. You can choose to do this, or select a new alignment and/or orientation. 6. Click OK. The new connector will be listed in the Manage Connectors box. 7. To define new geometry for placing a connector, select the option Define new geometry, then click on the Select plane button will display. . The Define Plane box
8. Use the functions provided by the Define Plane box to reposition the connector, if necessary, as explained below. (The colors of the buttons may be slightly different in some applications.)
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Click the Define Plane button to redefine the plane as well as the origin by clicking once on the face. Click the Define Plane using Compass button to redefine the plane using the compass. Click the Define 3-point Plane button to define the plane by clicking on any three points with your pointer. The connector will be placed on the first point you click. Click the Define Line-Point Plane button to select the plane by clicking on a point and a line, like an edge. The connector will be placed on the first point you click. Click the Define Line-Line button to select the plane by clicking on two lines. The plane will be defined by the first line selected. But if the two lines are parallel the plane will be defined as the plane in which both lines exist. Click the Define plane at center of circle button to select the plane by clicking three points on the edge of a circle. This method is used for multiCAD documents, usually for CGR circles. You can click at points where two lines meet or in the center of a face. The Z axis of the plane manipulator will be placed according to the right hand rule. If you click clockwise the Z axis will point into the object. If you click counter clockwise the Z axis will point out from the object. Click the Define plane at product origin button and then the object to place the plane manipulator on the origin of the object. The plane manipulator axis will match that of the product. Click the Define Orientation button to change the orientation. Click the button and then click a point or a line. If you click a point the X axis will point to it. If you click a line the X axis will become parallel to the line.
Define Origin at Plane Use the Move Origin buttons to define the plane. or Compass allows you to define the origin using the compass or plane command. You use the compass or plane as the base plane along which the
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origin can be selected.
Define Origin at Point or Center of Face lets you
Define Origin at Center of select the origin by clicking on a point or face. Circle allows to select the origin by clicking at three points - the origin will be placed in the center of an imaginary circle drawn using those three points. The plane and orientation will not change when using this command. 9. Click OK. The connector will be placed and the Add Connector dialog box will display again.< 10.Make your selections in the fields under Classify Connector as described in Step 5. Click OK.
Using the Compass to Manipulate Connectors
This task shows you how to use the compass to manipulate connectors placed on resolved parts. You can use the compass to manipulate connectors placed on resolved parts only. Use this method when adding a new connector, or by using the Modify command. Both are explained below. 1. To manipulate while adding a connector, drag the compass and place it over the connector while the Define Plane box is displayed. 2. To manipulate using the Modify command, select the resource, click the Manage Connectors button and, in the Manage Connectors dialog box, select the connector in the connectors list. Click the Modify button. 3. The Modify Connectors box will display. You can now drag the compass and place it over the connector. 4. Click on one of the handles on the compass and manipulate the connector to the desired position. You can change alignment, orientation and origin using the compass.
5. Click OK on the Modify Connector or the Define Plane dialog box when done. Remove the compass from the connector by dragging it to the axis.
Modifying or Deleting Connectors
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routingSystems This task shows you how to modify or delete connectors. You will not be able to modify or delete a connector that has constraints or connections. You will not be able to modify or delete a connector on the instance of a part using the Modify or Delete commands in the Manage Connectors dialog box. You can only modify or delete connectors on the reference of a part (the part in the master catalog). You need to use the Create Part command to modify a reference part. However, you can modify or delete a unique part using the Manage Connectors dialog box. 1. To delete a connector select the resource by double clicking in the specifications tree and click the Build Connectors button. This will display the Manage Connectors dialog box. 2. Select the connector in the connectors list and click the Delete button. The connector will be deleted. 3. To modify a connector click the Modify button in the Manage Connectors box. The Modify Connectors dialog box displays.
4. Follow the procedures described in Step 4 and subsequent of Creating Connectors.
Creating Duplicate Connectors
This task shows you how to create one or more duplicate connectors.
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Advanced Tasks You can only make duplicate connectors on a resolved part. Connectors can only be duplicated on the same part. With your resolved part displayed, click the Build Connectors button. This will open 1. the Manage Connectors dialog box. 2. Select the part. This will display all connectors on it and also display a list in the dialog box.
3. Select the connector you want to duplicate and click Duplicate in the Manage Connectors dialog box. The Duplicate Connectors dialog box displays.
4. Enter the spacing between the connectors and the number of connectors you want.
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routingSystems 5. Drag the compass and place it on a surface with the Z axis pointing toward the direction in which you want the new connectors located. The two illustrations below show how you can change the location of the new connectors by changing the direction of the Z axis.
6. Click OK.
Using the Plane Manipulator
This task shows you how to use the plane manipulator. You can use the plane manipulator to change the orientation, alignment, plane and location of the plane you propose to create. The X and Y axis indicate the orientation and the Z axis indicates the alignment. For example, if you create a connector and route from it, routing will occur in the direction indicated by the Z axis.
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1. To change the orientation of an axis, click on the dot at the end of it. It will flip 180 degrees.
2. To move the manipulator along any axis, click and drag on that axis. The manipulator will move and the distance will display. 3. Click on the origin (red square) and drag to move the manipulator to a new plane. 4. To change the orientation you can also click and drag any of the arcs in the manipulator to rotate it. It will rotate in increments, which is 15 degrees in the image below.
To change the degree of rotation click Tools-Options, select Equipments & Systems and select the General tab. Enter the degree of rotation in the Snap Angle field. For instance, if you enter 45, the manipulator will snap in increments of 45 degrees, counting its starting position as 0. It will snap to the nearest 45 degree step - if you move it to 88 degrees from its starting position it will snap to 90 degrees.
Working with Bendables
Extracting Bending Data from Bendable Pipes and Tubes
This task shows you how to extract bending data from Bendable Pipes and Tubes and transfer it into a Microsoft Excel worksheet. Bending data can be fed into Bending machines to precisely create bends in bendable tubes and pipes. • The standard macro supplied with this product displays bending data in a sample format. However, a user with some Microsoft VBScript experience can change the script supplied to change the format.
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routingSystems • • The sample script assumes that the bendable objects are placed on a run under a distribution system or a logical line. For more information on placing parts, see Placing Parts in a CATProduct Drawing. command subdirectory.
1.
Using Windows Explorer, locate the intel_a
code
2. Copy the files PslTubingExtract.CATScript and PslTubingExtractTemplate.xls
to C: temp (with read-write access). Select the two files and click the right mouse button. Click Properties in the drop-down menu that displays. The
Properties dialog box will display. Uncheck the Read-Only option.
3. In the specifications tree, select the logical line or distribution system under which the run containing the bendable objects has been placed.
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4. Click Tools - Macro - Macros. The Macro dialog box will display. Select External File from the drop down list, select PslTubingExtract.CATScript and click Select. The Select External File dialog box will display. Select PslTubingExtract.CATScript and click Open. This will again display the Macro dialog box. Select PslTubingExtract.CATScript and click Run. Data will be extracted from the bendable objects and displayed in an Excel worksheet, part of which is displayed below. (CATIA will create the table, but you must have Excel installed!)
Design Checks for Bendable Pipes and Tubes
This task shows you how to perform design checks on bendable pipes and tubes. The design checks will tell you whether the radius of a bend, the total length of the run and the rest length are within prescribed limits. The rest length is the straight segment between two nodes (with bend radius). Click the Update button whenever you see it active (not greyed out) during this process. Also, don't forget that you need to have the Knowledge Expert product installed for this process. In the following example the maximum bend radius will be checked.
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routingSystems 1. Click Start - Infrastructure - Knowledge Expert to enter the Knowledge Expert workbench. 2. Set up your options correctly or you will not be able to do the following steps correctly. • • • • • Click Tools - Options and select General from the left column of the window. Click the General tab. Select Automatic for the Update function. Click Product in the left column of the window and scroll to the Product Structure tab. Under the Specification Tree function make sure the Relations and Automatic Expand options are selected.
3. Make the run active. 4.
Click the Insert Rules button directory.
and navigate to the KnowledgeRules
5. Select Bendable_CheckMaxBendRadius.CATProduct and click Open. 6. If the desired bend radius violates the bend radius rules, a red light will show against the relevant CATProduct line icon in the specifications tree, in this case CATKWEBendRadiusCheck.1. If there is no violation then a green light will show next to it. In the illustration below the red button is showing (with the mouse pointer pointed at it).
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Advanced Tasks 7. To change the maximum bend radius do the following: Each check has a parameter element beneath it in the specifications tree - in this case it is MaxBendRadius. Double-click on the element to display the Edit Parameter dialog box. Enter your maximum bend radius in this box. To check for rest length and total run length select the appropriate CATProduct in the Load Report dialog box. Make sure it has the word "check" in it.
Transfer Elements to New Document
This task shows you how to transfer elements to a new document. You can use this function to transfer elements to documents or work packages that are under the same Product. See also Transfer Run to Another Document. This function removes selected elements from a document and moves them to a new document. You cannot move them to an existing document. 1. With your document open, click the Transfer Elements button . The Transfer Elements dialog box displays. In the image below it displays equipment that has been selected.
2. You can select elements to transfer in various ways: • • Click the element you want to transfer. Click the Select Elements in Range button and make your selection in the Analyze Networks dialog box that displays.
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• •
Click the Select Spools Selection List. Click the Select Line IDs Selection List.
button and make your selection in the button and make your selection in the
3. If you do not want to transfer some elements in the Selection List, select the element(s) and click Remove. Remove All removes all elements. 4. Make your selections. Spools and Lines will display the existing name in the File Name field. You can edit this name, or add a Prefix or Suffix (or both) to distinguish it from the original name. Elements do not display any name you need to enter a name. In this example it is TestTransfer. The image below shows the entries in the specifications tree, with the Equipments node expanded, before the transfer.
5. The vessel has been selected for transfer (the associated nozzle will automatically be selected). Click Apply or OK. Apply allows you to transfer more elements. OK exits you from the command. The image below shows the transferred equipment.
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Workbench Description
Workbench Description
The Systems Routing workbench includes the following toolbars:
Systems Routing Toolbar
General Design Toolbar
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General Environment Toolbar
Product Placement Toolbar
Update the System
Toolbars
Systems Routing Toolbar
The Systems Routing Toolbar contains the following tools:
See Creating a Logical Assembly.
See Creating a System Assembly See Creating a Logical Set See Routing Runs and Modifying Runs. See Route a Run Along a Spline See Route a Run at an Offset of a Routable See Route a Run within a Pathway See Create an Offset Connection between Segments See Disconnecting a Run See Connecting a Run See Breaking Run at a Branch
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Workbench Description
See Creating a Pathway
General Design Toolbar
The General Design Toolbar contains the following tools:
Align Toolbar See Aligning Elements See Aligning elements See Aligning elements See Distributing Elements See Aligning elements Snap Toolbar See Snap Resources Together Snap Three Points: See Quick Snap Resources Snap Center of Polygon: See Quick Snap Resources Snap Surface: See Quick Snap Resources See Create Parent-Child Relationship See Mirroring Elements. See Mirroring Elements See Rearranging Elements in the Specification Tree. See Connectors
Product Placement Toolbar
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routingSystems The Product Placement Toolbar contains the following tools:
See Catalog Browser See Placing Multiple Parts in a Run See Flipping Elements See Change the Reference File for a Part See Change the Parameters of a Part
General Environment Toolbar
The General Environment Toolbar contains the following tools:
See Changing the Current Axis.
See Generating Detail Information See Using Offset Planes
Advanced Offset Plane See Using a Step Grid for these icons: Snap to steps off current axis Snap to steps off last position Snap to XY construction plane Snap to all construction planes Snap to elevation (Z) construction plane
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Workbench Description
Snap to Drafting elements See Making an Element Active.
See Manipulation Handle Mode See Making an Element Active for these icons: Activate Parent Activate Area Activate Network/Logical Line
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Project Standards
Systems Routing Settings
General Settings
This task is to inform you about the settings in the General tab. The General tab provides settings for General Environment, Resolved Part Storage path, Resource Attributes and Catalog Placement Options. 1. Click Tools - Options - Equipment & Systems and select the General tab.
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routingSystems 2. General Environment: • Grid Step. This is the default grid step setting that displays in the General Environment toolbar at the bottom of the 3-D viewer. Even if you change the value in the toolbar during your session, the value entered in the Grid Step field will re-appear when you open a new session. Enter your preference for the Grid Step. Note: The Units (unit of measure) is set in the Units tab under Tools - Options - General - Parameters and Measure. See also Set Correct Working Units and Grid. The Snap Angle sets the degree of rotation of the plane manipulator. See Using the Plane Manipulator for more information.
•
3. Resolved Part Storage for Spatial Objects: • Directory. This is the location where resolved Spatial objects unique to the Plant Layout, Systems Routing and Systems Space Reservations products are stored. Click the Open file button and navigate in the Resolved Part Storage Directory Browser window to set or change the location for the directory.
4. Resource Attributes: • Automatic creation of resource attributes. Certain attributes accompany Spatial objects (those created in Plant Layout, Systems Routing and Systems Space Reservations); objects such as item reservations, areas, runs, etc. These attributes, or properties, are generated specifically for the Delmia product line and cannot be assigned or changed in other product lines.
Although you will not be making use of these resource properties, their creation will have no affect on the product you are working in. If you do not want these properties to be created, uncheck the box Automatic creation of resource attributes and click OK. 5. Catalog Placement Options: • Display image while placing catalog object in 3-D viewer. You can choose to hide or display a "preview" of the part you are placing. Check or uncheck the box Display image while placing catalog object in 3D viewer to obtain the effect you want. Place at component's origin when placing in free space. By default, when you click (in free space) to place a part, the center of the part will be placed at that location. The application determines the center of the part by creating a box around it and selecting the center of the base of the box. You can also choose to place the origin of the part at the point where you click. To do this check the box Place at component's origin when placing in free space.
•
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Project Standards
Display Settings
This task is to inform you about the options available in the Display tab. The Display tab provides display options for Analysis Mode, Specifications Tree, 3-D Viewer Display and Routable Display options. 1.Go to Tools - Options - Equipment & Systems and click the Display tab.
• •
Analysis Mode: Check the box in Analysis Mode to display information about routables. It works only when you are performing an action with a routable, such as placing a part, branching a run or creating an offset route. Specification Tree: In Application objects check the box Show application grouping to organize the objects in the tree by application, e.g. Piping objects, Equipment, etc. Under Spatial objects check the boxes of the items you want to appear in the specifications tree. Spatial objects may only be placed using the Systems Routing, Systems Space Reservation and Plant Layout workbenches.
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• •
3-D Viewer Display Options: Check or uncheck the boxes to set the connection and connector display options as desired. Set the color of the connection and connector symbols using the drop down color palette. Routable Display Options: Increase the Twist Smoothness Factor to increase the smoothness of a run at a twisting turn.
Design Criteria Settings
This task is to inform you about the settings in the Design Criteria tab. The Design Criteria tab allows you to toggle settings for ID Management, 3D Design, and 3D Placement. 1. Click Tools - Options - Equipment & Systems and select the Design Criteria tab.
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Project Standards
•
• •
ID Management: Update ID on property change. When the object naming convention (ID schema) includes an attribute, e.g. nominal size, and you change its value using the Properties dialog box, the name of the object will change to reflect the new value of the attribute. 3D Design: Check Schematic Driven if you are placing parts from a schematic into a 3D design document. Used with Piping Design, Tubing Design, HVAC Design and Waveguide Design applications. 3D Placement Options: When the Place automatic parts box is checked you can place an object such as a valve (e.g., in Piping Design); the flanges, gaskets and welds will be placed automatically when you place the pipe.
Working in Cache Mode
This task discusses steps you should take to design efficiently in cache mode. Cache mode refers to designing without loading all the technological data of objects in your document. It is recommended because it allows quicker loading of documents and execution of commands. However, you may need to take certain steps to design efficiently in this mode, which are discussed here. This task also explains ways of executing certain commands while in cache mode.
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routingSystems 1. When you are using the command Place Object from Catalog while you are in cache mode you will not be able to place a part on a connector because connectors are not loaded. To change that part to design mode click the button and then click the part. That part will be Analyze Item converted to design mode and connectors will be visible. 2. It is recommended that you redefine the location of the CATCache directory. This directory is used to store certain design elements (cgr files) that are used when visualizing a document in cache mode. If the file name of an element is too long then the visualization will not be correct - this is a Windows limitation. Because the full path name is used in the file name, you should redefine the location so that the path name is short - as short as you can make it. To redefine the path name click Tools - Options Infrastructure - Product Structure and select the Cache Management tab. Enter the new path in the Path to the Local Cache field.
3. Wireframe geometry, such as the sections on trapeze hangers, are not visible in cache mode, which also means they cannot be selected. If you want to be able to see them in cache mode then check the option Save Lineic Elements in CGR. You can find it in Tools - Options - Infrastructure Product Structure and the CGR Management tab.
Customizing the Dictionary of User Types
Customizing the Dictionary of User Types
This task explains how to customize the list of types that are displayed when you create any of these elements:
• • •
System assembly Logical assembly Runs
A basic dictionary of these element types is provided with the product. You can add entries to or delete entries from the basic dictionary, or you can replace it entirely. You can also customize the icons that are associated with the element types. To customize the dictionary, you need to run the following scripts: PSLNomenAccessFeat.CATScript reads the existing dictionary and writes it to a preformatted Microsoft* Excel file. PSLNomenBuildFeat.CATScript takes a properly fomatted Excel file and generates a new dictionary.
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Project Standards To accomplish this procedure, you must have installed Microsoft Excel 97 or later version. You should be familiar with the basic editing features of Excel, as well as with the file navigation and file editing capabilities of your system. 1. Copy the following files from intel_a code command to a drive or directory for which you have read and write permissions: • • • PSLNomenAccessFeat.CATScript PSLNomenBuildFeat.CATScript PSLNomenAccessFeatTemplate.xls
2. Start CATIA. 3. From the menu bar, select Tools -> Macro -> Macros. 4. Select External File for the Macro In: field. 5. Click the Select button, and use the Windows dialog box to navigate to the appropriate file. 6. Select the file PSLNomenAccessFeat.CATScript and select OK. 7. Edit PSLNomenAccessFeat.CATScript as follows: Define the path strEXCELTemplateFileName to point to the directory to which you copied the files in Step 1.
8. Save and close the file. 9. Select Run. Microsoft Excel is launched, and a file is created. 10. Edit the Excel file to add or delete entries, as appropriate. 11. Save the Excel file with a unique name. 12. From the CATIA menu bar, select Tools -> Macro -> Macros again. 13. Select the Select button, and select the file PSLNomenBuildFeat.CATScript. 14. Edit PSLNomenBuildFeat.CATScript as follows: • • Define the input path strEXCELInputFileName to point to the Excel file you saved in Step 11. Define the output path strCATIAV5FeatOutputFileName to point to intel_a eat. If you do not have write permissions for this output path directory, you can define a temporary location. Contact your system administrator to move or copy the file to the correct location after it has been created. 15. Save and close the file. resources graphic CATArrNomenclature.f
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routingSystems 16. Select Run. The output file is created in the directory you specified. If you defined a temporary location for the file, it must be moved or copied to intel_a resources graphicCATArrNomenclature.feat before the modifications can take effect. The modifications will take effect when you restart CATIA.
Searching User-Created Dictionary Entries
This task shows you how to search documents for objects or elements that are user created. To learn more about the Search function see the Infrastructure user guide. To learn more about customizing see Customizing the Dictionary of Types. 1. Click Tools - Macro - Macros. This will display the Macro dialog box. In the drop down menu select External File and click Select.
2. The Select External File dialog box will display. Navigate to the directory where CATIA is installed and open the directory intel_a code command. Select the file CATArrExtractArrFeatAsCATNLS.CATScript and click Open. The Select External File dialog box will close and the Macro dialog box will display, with the file CATArrExtractArrFeatAsCATNLS.CATScript selected. Click Run. 3. 4. Close the CATIA session. Using Windows Explorer navigate to the directory C: file CATArrNomenclatureFeat.CATNls to the directory temp and copy the
intel_a resources msgcatalog. 5. Also copy the file CATArrNomenclatureFeat.CATNls to all language subdirectories (if any) of Intel_a resources msgcatalog.
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Saving a System Assembly or Logical Assembly as a Separate Document
This task shows you how to create and save a system assembly or logical assembly as a separate document.. This function is needed if you want to work separately on a component of a larger project. If you save the system assembly or logical assembly as a separate document you can open it without having to open the entire project. At the same time it remains part of the larger project. 1. When creating a new System Assembly or Logical Assembly check the Create new document option.
2. Enter a name in the File Name field and click OK. The new document appears in the specifications tree as a child of whichever element you created it under. In the specifications tree, the icon for a system or logical line created as a separate document is different from that which is not created in a separate document. In the illustration below WasteWater is created as a separate document, Piping System Assembly1 is not.
3. When you save the project a dialog box will ask if you want to proceed with other document save operations. Click OK.
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Creating a Catalog
Creating Parts
This task explains how to create parts for the Systems Routing Product. 1. Create the geometry for the part. Use the Version 5 Part Design product to create the geometry. See the Version 5 Part Design User's Guide for instructions about how to use this product. • • • If you want to be able to place the part parametrically, go on to Step 2. For fixed-sized parts, save the part as a CATPart document and skip to Step 5. If you want to use the same set of geometry for different sizes of the same type of part, go on to Step 2.
2. Define parameters for the geometry.
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Project Standards When you define parameters, you must adhere to the following naming conventions to ensure that the part can be sized correctly when it is placed. The values for these reserved parameters are derived from the run on which the part is placed. • • • • • • CATRouOutsideDiameter : outside diameter of the part if it is placed on a cylindrical run CATRouOutsideHeight : overall height of the part if it is placed on a rectangular run CATRouOutsideWidth : overall width of the part if it is placed on a rectangular run CATRouFaceToFaceLength : overall length of a stretchable part such as pipe or duct CATRouAngle : turn or branch angle of parts such as an elbow or tee CATRouTurnRadius : bend radius of a part such as an elbow or horizontal turn
You may also add two other reserved parameters to your part as User attributes. • • CATRouPartNumber : a string parameter. This parameter will contain the part's part number. CATRouSize : a string parameter. This parameter will contain a character string representing the nominal size of the part. It can be used instead of CATRouOutsideDiameter/Height/Width.
All of these parameters do not need to exist on every part. Define only those parameters that apply to the part you are creating. For example, to create a straight cylindrical part, you would define only the CATRouOutsideDiameter and CATRouFaceToFaceLength parameters. Optionally you can define CATRouSize instead ofCATRouOutsideDiameter. In addition to the reserved parameters, you may define other parameters on the part. These parameters must also be included in the design table if these parameters have different values for different sizes when the part is placed.. 3. Save the part as a CATPart document. 4. Create the design tables. See the Version 5 Infrastructure User's Guide for detailed instructions on how to create a design table and associate it to a part for which you must use external table files. Excel files are easy to edit, but using tab-delimited text files instead of Excel files makes parts placement more efficient. You can build and edit your tables in Excel, then convert the file to a tab-delimited text file, and attach the text file to your part document.
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routingSystems Design tables are used to manage the allowable combinations of values for the parameters of a part. You must create tables with the following reserved names in order for them to be recognized by the Systems Routing product. (Except external files, see below.) • CATRouFixedSize
This table must contain those reserved run parameters described after Step 2 which you want as fixed size parameters. Your table may contain one or more rows of values, each row generally represents a specific fixed size part. The first row contains the parameter names. They may be reserved parameters or other parameters. Those that are reserved run parameters are used as a key to select the appropriate row in the table. When the part is placed, the values for these parameters are derived from the run. If an exact matching of values on the run and values in the table is not found then the row with the closest match is used. This table must also contain parameters not associated with the run, if any, that are needed to complete the geometry definition. Generally, you may wish to include in your table CATRouPartNumber as the first parameter, CATRouSize as the second, then the other reserved run parameters, then the other part parameters. • CATRouParametricSize
This table is used to define parameters that can be dynamically defined by the run. All parameters in this table must be defined on the run. When a part is placed, the values for these parameters are retrieved from the run and used to size the geometry. If you use external files they can have any name. But when you create the design table in the part document it must have one of the reserved names. 5. Define connector data on the part by following the steps below.
Connector data is used to properly position, align, and orient parts when they are placed on a run. In addition, it is used to properly position, align, and orient a run that is started from a part. a. Start a new CATProduct document. b. Right-click the Product in the specification tree and select Existing Component. The Insert an Existing Component dialog box is displayed. c. Find and select the CATPart document you saved. d. Select the part in the specifications tree. e. Add a connector using the Build Connector command. h. Save the CATPart document.
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All About Connector Data
There are three types of connector data: Face data, Alignment data and Orientation data. Face data is generally defined using a face of the part, such as the circular face at the end of a pipe. Alignment data is generally defined using a line, such as a not shown line along the centerline of a pipe. The actual connection point location is the intersection between the face plane and the alignment line. They do not have to actually intersect: the system will find the intersection location between the infinite line and the infinite plane. The face does not have to be the actual diameter face or width-height face. Orientation data is generally defined using the xy plane, or another plane or face in the part, to define an "up" direction. Face Connector Data. To define the directional planar location for each connection face of the part. If the part is stretchable, two connection face definitions will be used to define the extremity locations of the part. For routing from the part, a connection face (along with the corresponding intersecting alignment line) will be used to define the start point of the run. You should select one of the faces in the part to define a face connection. Select a face that faces outward from the part, in the direction of routing or other attached parts. You must define a face for each connection end of your part. The pre-defined names for face connector data include the following. The names are defined by the connector function. Use the connector function to delete a connector. CATRouFace : for the first or only connection face of a part. CATRouFace1 (same as CATRouFace): for the first connection face of a part. CATRouFace2: for the second connection face of a part. CATRouFace3: for the third connection face of a part. CATRouFace4, 5, 6, etc. CATRouHole CATRouHole1 CATRouHole2, 3, 4, etc. Hole connections are a unique type of face connection. Whereas a pipe or tube may stretch to a face connection, a pipe or tube may pass through a hole connection. This is useful for placing such parts as tubing clamps along a run
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routingSystems without cutting a tube. Alignment Connector Data. To define the alignment at each of the face connections of this part. For placement of an attached part or routing from the end of a part, this data will define the alignment. You will generally select a line for the alignment connector data, which may likely be no-shown. But you may also select a cylinder, and its implied centerline will become your alignment data. Each part connection face does not necessarily need its own alignment line. A pipe and a valve might have one alignment definition, but an elbow would need two alignment definitions. A tee needs two alignment definitions, but could have three. A cross with four connection ends needs at least three alignment definitions. When the number of alignment definitions is less than the number of connection ends, it must be only one less, and alignment1 corresponds with face1 and face2, and alignment2 corresponds with face3. The pre-defined names for alignment include the following: CATRouAlignment: for the first or only alignment line of a part. CATRouAlignment1 (same as CATRouAlignment): for the first alignment line. CATRouAlignment2: for the second alignment line of a part. CATRouAlignment3, 4, etc. Other pre-defined names for alignment include the following: CATRouTop: for top-center CATRouCenter: for center (same as CATRouAlignment) (center is default alignment) CATRouBottom: for bottom-center CATRouLeft: for left-center CATRouRight: for right-center CATRouTopLeft CATRouTopRight CATRouBottomLeft CATRouBottomRight including 1, 2, 3, 4, etc
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Orientation Connector Data. To define the orientation/clocking of a part when placed on a run. Many parts direction, such as horizontal trays and power & free conveyors, require a well-defined "up". Round ducts and pipes do not require a well defined "up" direction, they can rotate. Rectangular ducts do not have a strict "up" direction, but do have four usual orientations corresponding to each of the four sides. Tubing elbows can flip upside down in order to swap end1 and end2, since they often have different end styles. Generally, parts are built in such a way that the Z direction is up. If this is the case, then generally the XY plane can be used to define the orientation. The orientation plane and the face plane should not be parallel. For a particular connection end, you should not define an alignment going up in the Z direction and an orientation plane pointing up in the Z direction. Rarely will an "Orientation2" be needed. Some tubing clamps use an orientation2 because they have one alignment along the tube alignment and another alignment going up through the bolt hole (for stacking). Tray vertical elbows and vertical tees also need an orientation2. The pre-defined names for orientation include the following: CATRouUpOnly: the part has a well-defined "up" direction. (Tray) CATRouUpOnly1: same as CATRouUpOnly CATRouUpOnly2, 3, etc. CATRouCircular: the part has no strict "up" direction. (Pipe) CATRouCircular1: same as CATRouCircular CATRouCircular2, 3, etc. CATRouRectangular: the part has four orientations that can be "up". (Rect duct) CATRouRectangular1: same as CATRouRectangular CATRouRectangular2, 3, etc. CATRouOrientation: same as CATRouUpOnly (up-only is default orientation) CATRouOrientation1: same as CATRouUpOnly1 CATRouOrientation2, 3, etc. same as CATRouUpOnly2, 3, etc. Sample Publication Management combinations for connector data: A pipe or piping valve: CATRouFace1
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CATRouFace2 CATRouAlignment CATRouCircular A piping cap: CATRouFace CATRouAlignment CATRouCircular A rectangular duct elbow: CATRouFace1 CATRouFace2 CATRouAlignment1 CATRouAlignment2 CATRouRectangular An OPF conveyor track: CATRouFace1 CATRouFace2 CATRouBottom CATRouOrientation A tray horizontal tee: CATRouFace1 OR CATRouFace1 CATRouFace2 CATRouBottom1 CATRouBottom1 CATRouFace2 CATRouFace3 CATRouBottom2 CATRouBottom2 CATRouFace3 CATRouOrientation CATRouBottom3 CATRouOrientation A round duct cross: CATRouFace1 OR CATRouFace1 CATRouFace2 CATRouAlignment1
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CATRouAlignment1 CATRouFace2 CATRouFace3 CATRouAlignment2 CATRouAlignment2 CATRouFace3 CATRouFace4 CATRouAlignment3 CATRouAlignment3 CATRouFace4 CATRouCircular CATRouAlignment4 CATRouCircular
A tubing clamp: CATRouHole1 OR CATRouHole1 CATRouHole2 CATRouAlignment1 CATRouAlignment1 CATRouOrientation1 CATRouOrientation1 CATRouHole2 CATRouFace3 CATRouAlignment2 CATRouAlignment2 CATRouOrientation2 CATRouOrientation2 CATRouFace3 CATRouFace4 CATRouAlignment3 CATRouAlignment3 CATRouOrientation3 CATRouOrientation3 CATRouFace4 CATRouAlignment4 CATRouOrientation4
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Creating a Catalog
This task explains how to create a catalog. The Catalog facility is a standard facility provided with the V5 Product line. For detailed information regarding Catalogs, please see the Infrastructure documentation - Advanced Tasks - Using Catalogs. Information that is particular to this product is given here. To properly learn to create a catalog you must read the document referenced above. 1. Open the Catalog Editor by clicking on Start-Infrastructure-Catalog Editor. The Catalog Window opens with a basic catalog structure in the left column. Catalogs are created analogous to books, with the book being at the top level, chapters under it, and, if necessary, sub-chapters under them, and with pages at the lowest level. Each family contains references to one or more parts. The illustration below shows the Catalog Editor. The column to the left is where your chapters and families are displayed. The column to the right will display parts when you click on a family.
If you click the Reference tab you will see the directory path to each part (the file). Clicking the Preview tab displays the part. Clicking the Keywords tab displays the keywords. To add a keyword double click on the family where you want to add it, , and add your information in the Keyword click on the Add Keywords button Definition dialog box that displays. See below on how to add values for keywords. Click here to see a list of keywords. 2. Rename the catalog and chapter and add as many chapters and families as you want to. You can add these later also. Save and close the window and reopen it to see your changes. To rename the chapter, right-click on it and bring up the Definition dialog box. To rename the book, save the catalog, at which time you can rename it.
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3. Add a component to the page. Make the page active and click the Add component button to bring up the Description Definition dialog box. Click the Select document button, navigate to the the component document and select it. Click OK to end. To add values for keywords click the Keywords values tab. A window will display all the keywords associated with that family. Select a keyword and enter the value in the Values field. Keywords and values are case sensitive and you must enter them accordingly.
Making a Catalog Accessible
This task explains how to specify the location of a catalog so that it can be accessed in order to place parts from it. Some catalogs are provided with the application. These are located in the .. intel_a startup components subdirectory.
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routingSystems 1. Click Tools-Options, select General and then the Document tab. Select Other folders in the window and click Configure.
2. In the Other Folders dialog box, double-click on the drive where the catalogs you want are located. This will display all directories in the drive. Navigate to the directory that contains the catalog(s), select one or more, and click Add. All the catalogs you have selected will display in the lower window, as shown in the image below.
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3. Click OK. This will save the search order. Now when you click the Catalog Browser button you will be able to select parts from the catalogs you defined. To change the catalogs that are displayed when you click the Browser button (the search order), you can repeat the steps above and specify different catalogs. You can also use the Export function in the Other Folders box to save the location of other catalogs or groups of catalogs. This will enable you to open them by recalling the search order, rather than having to repeat the steps given above. To do this: 4. Bring up the Other Folders dialog box and navigate to the directory where the catalogs are located. Select the catalogs so that they appear in the lower window. Click Export. The Export Search Order dialog box will display.
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5. Enter a file name and specify a location for the file. Click Save. 6. To recall a saved search order, click Import in the Other Folders dialog box and select the file that specifies the catalogs you want to open. Click OK. This will create a new search order and these catalogs will display when you click the Browser button. 7. Use the Import Add button to add a search order to an existing search order. For instance, if you have a search order open but you want to add to it catalogs defined in another search order, click Import Add, navigate to the directory where the saved file is, and select it. The catalogs in that file will be added to the search order that was open.
Catalog Keywords and Values
You need to add keywords and values for some parts to the catalog to enable certain behavior. The process for adding keywords and values is explained in Creating a Catalog. A list of keywords and values is given below. They should be entered exactly as they are shown in their mixed case (upper and lower case).. The keyword PlaceAndStretch allows parts to bridge the gap between two dissimilar ends, such as a round and square run, or different sized pathways. It has no values. The keyword LoadType affects how a part should be loaded into memory from the catalog. If the keyword is not added then its values is assumed to be NewReference, which is explained below. LoadType has two values. • SameReference -- the part is always an exact copy of the catalog part. Never changes
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•
the parameters of the placed part. NewReference -- the part has parameters that can be changed. New copies of the part will made as needed.
The PlacementType keyword restricts the placement of the part, and can have one of the following values: FreeSpaceOnly -- part can only be placed in free space. Equipment -- same as FreeSpaceOnly, part can only be placed in free space. Inline -- Can be placed at the ends of parts and runs. Reducer -- part is used to change size or shape. Usually placed on the node between two connected, collinear or parallel runs of different sizes or shapes. Reducers can be placed at the ends of runs and parts. Turn -- part is placed on a turn or at the ends of runs and parts. Branch -- part is usually placed at the intersection of two straight segments, where the end of one segment intersects the middle of the other. Branches can also be placed at the ends of runs or parts • • • on straight segments at corners at intersections of the ends of no more than three segments.
When using the multi-place (shift) option, branches will be placed on all intersections on a run that have exactly three pathways. Cross -- part is usually placed at any intersection containing four pathways (e.g. four end segments, or two end segments meeting in the middle of another segment). Can also be placed • • • on the ends of runs on straight segments at corners.
When using the multi-place (shift) option, crosses can be placed on all intersections on a run that have exactly four pathways. Complex branch -- part can be placed at an intersection with more than four connections and anywhere a cross can be placed. Offset -- can be placed at the ends of parts or runs. The part connects runs that are offset from one another. Terminus -- part placed at the end of a run or part (e.g. a cap).
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Coupler -- can be placed on part ends. It is small connecting part, such as a gasket or flange. Support -- placed in the middle of segments, or on the ends of parts and runs. The part is used to support other parts, such as hangers. . Strengthener -- placed in the middle of segments. The part is used to strengthen or stiffen. It can be Nozzle -- can be placed on the ends of parts. Part is used to connect equipment to a part transporting fluid (e.g. pipe).
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