PTC Express: Creating Part Level Simplified Representations in Pro/ENGINEER

December 2005

Creating Part Level Simplified Representations in Pro/ENGINEER

As a Pro/ENGINEER user you may regularly create simplified versions of complex assemblies using simplified representations. But did you know that similar functionality exists to simplify parts as well? Not only is this capability useful when designing a complex part, but these simplified parts can also be used as a substitute for the fully detailed part in an assembly simplified representation. These substitutions are an effective way to represent cutouts, create zones, and show only portions of models needed for a particular design task. This tip will show a variety of part level simplified reps on the model shown in Figure 1.

Part level simplified reps are created by using the view manager just as assembly simplified reps are created. This tip focuses on creating three different types of reps.

To get started,

Pull up an individual part and select the view manager icon. This will bring up the View Manager dialog box (Figure 2). This dialog box is similar to the view manager dialog box in assembly mode. The only difference is that the Style and Explode tabs are missing since these do not apply to individual parts.
Select the Simplified Rep tab near the top of the dialog box. By default, there will be four reps that already exist in the model as shown in Figure 2. These reps are the master, symbolic, geometry, and graphics rep. These are simplified representations that are created automatically when saving a part file.
Select the New button from the View Manager dialog box and give the rep a name. Either select Edit, Redefine from the buttons or use the right mouse button (RMB) pop up menu to select redefine. This will bring up the Edit Method menu. (Figure 3)

The Edit Method menu allows you to set the attributes about the part level simplified reps as well as create three different types of simplified reps. The three types of part level simplified reps are features, work regions, and surfaces. We will look at each one of these types of reps.

1. Features. This type of rep allows you to exclude features from the model. This functionality is different from simply suppressing features because due parents of features can be excluded without requiring you to suppress the children. Here are the steps:

Select Features from the Edit Method menu. The Feat Inc/Exc menu will appear. By default the menu will be set to allow you to select the features to exclude. To change the default, use the Attributes menu pick from the Edit Method menu. For this example, the default of including the features and selecting the features to be excluded will be used.
Select a few features to exclude.
Select the Update Screen pick to update the part with the selected features excluded.

Another way to select a set of features is to use the search tool. This tool can be used to select all features of a certain type. This is a great way to create a simplified rep that excludes all the rounds from a model. Here are the steps:

With the Exclude menu pick selected, select the binoculars icon to launch the search tool. The Search Tool dialog box will appear.
Select the Type radio button and use the criteria options to set the type equal to round. (Figure 4)
Select the Find Now button to find all the rounds in the model. The rounds will be listed in the left hand column under a title of items found. You can select individual rounds from this list or multiple items by using the ctrl or shift key. All the items in the list can be selected by selecting ctrl A. Once the desired rounds are selected, use the arrows button to move the items from the found list to the selected column on the right hand side of the dialog box.

Close the search tool and notice that the rounds are shown as excluded in the model tree. This search tool can be used in a number of ways to select a variety of features.

Once the features are selected to be excluded from the rep, select Done from the Feat Inc/Exc menu. This will bring you back to the Edit Method menu.
To finish off the rep, select Done/Return from this menu. The view manager dialog box will appear.
To switch between the new rep and the master rep simply double click on the rep name from within the dialog box. The red arrow will indicate which rep is active. Figure 5 shows a simplified rep of the example model with no rounds.

2. Work regions. A work region allows you to create a cut or series of cuts to remove material from the model leaving only a section of the model to work on. This is a great technique to eliminate a portion of volume from large part models or to create cutouts to use in an assembly. Here are the steps:

Reset the Master rep to active from the View Manager dialog box by double clicking on the Master Rep.
Select to create a new rep as done before by hitting the new button in the dialog box and giving the rep a name.
Use the right mouse button pop up to select redefine on the new rep name. This will bring up the Edit Method menu again. This time, select Work Region from the menu. This will bring up the Solid Opts menu.
Choose an option to Extrude, Revolve, Sweep, or any other desired creation method.
Select Done from the menu and the dashboard will appear.
Use the right mouse button popup menu to define an internal sketch.
Select a sketching plane and enter into the sketcher.
Create a sketch to define the area to remove. This sketch will be extruded to create a work region of half the model. (Figure 6
Once the sketch is created, use the dashboard to choose the extrusion options. For this example, the sketch was created on a center datum and extruded “Through All” in both directions. The options tab in the dashboard can be used to set the extrusion depths quickly and easily.
Choose the green check mark from the dashboard to finish the cut.
Then select Done/Return from the Edit Method menu to finish the new simplified rep. The view manager dialog box should now appear. Figure 7 shows finished work region simplified rep.

3. Surfaces. Surfaces allow you to select a set of surfaces to be displayed for the part instead of the entire volume. These types of reps are great to use as substitutions in an assembly level simplified rep. You can create a surfaces part level simplified rep that only contains the mating or critical surfaces of the model and substitute that rep to simplify a higher level assembly. Here are the steps:

Open the View Manager and ensure that the Master Rep is set to active in the View Manager by double clicking on it (the red arrow should be pointing to Master Rep).
Select the New button from the dialog box to create another new part level simplified rep. Now give the new rep a name.
Again, use either the right mouse button popup or the Edit pull down button to select redefine on the simplified rep. The Edit Method menu will again pop up.
This time, select Surfaces from the menu. The dashboard will appear allowing you to copy surfaces. All surface selection methods are now available.
Use the ctrl key and individually select a few surfaces. The shift key can also be used to select surfaces by either the surface and boundaries or loop methods.
Once the surfaces are selected, select the green check from the dashboard to finish the surface copy. The model should appear as only the selected surfaces.
Select Done/Return from the Edit Method menu to finish the rep. (Figure 8)

Use the view manager to switch between these simplified reps. These reps can be valuable for working on or analyzing the individual part (they can be used in Pro/ENGINEER Structural and Thermal, for example).

As mentioned before, another use for these part level simplified reps is in assembly level simplified reps. Here are the steps:

Pull up an assembly that contains a part with part level simplified reps.
Once the assembly is up, select the icon to launch the view manager. Create a new simplified rep and again use the right mouse button popup menu or the edit pull down to choose to redefine the rep. This will bring up the Edit rep dialog box with three tabs across the top.
Select the Substitute tab. The By Rep method will be selected by default.
Select the part that contains part level simplified reps. A list of the part level simplified reps should appear. (Figure 9)
Choose the desired simplified rep and select the Accept button. The rep name should show up in the model tree next to the part name.
Select the green check mark to create the rep. Multiple assembly level simplified reps can be created that reference different part level simplified reps through this substitution technique. (Figure 10 and Figure 11)