Figure 1. Casting model.

Figure 2. Machining model.

1. Create a casting model and a machining model using either the inheritance feature (new in Pro/ENGINEER 2001) or assembly merge technique. This approach closely represents actual casting and machining processes, allowing one model to contain only the casting features and the other to contain the machining features. The casting model can then be sent to foundries and the machining models to machine shops, so that each receive only the information they need to perform their work.

A. Using the inheritance feature.

• Create the casting model (e.g., FILENAME_CST.PRT) and add features necessary to create the casting. Note that using the default datums and coordinate system for both models makes this much easier
• Now create a machining model (e.g., FILENAME_MCH.PRT). The first feature you create after the default datums and coordinate system should be the inheritance feature. To do this, select Insert, Shared, Data, Inheritance. The command prompts you for a model that you wish to use (remember to change your reference control settings if necessary), and then a location.
• Continue on to Step 2.

B. Using the assembly merge technique.

This technique works with older versions of Pro/ENGINEER as well as 2001, but is more involved. Properly performed, it leaves you with two linked files without an external reference to an assembly—just like an inheritance feature.

• Create your casting model (for example FILENAME_CST.PRT) adding only features necessary to create the casting.
• Create a temporary assembly, and create the machining model (e.g., FILENAME_MCH.PRT) in it using Component, Create. Use the default placement.
• Assemble the casting model into the assembly. Use the default placement.
• Using Component, Adv Utils, Merge, follow the prompts and pick the machining model and then the casting model. Accept the defaults for the options that appear (Reference and No Datums).
• Answer No to the question “Support associative placement for the feature?”
• Answer Yes to the question “Detach reference part FILENAME from the assembly?”
• Close the assembly and using In Session, open and Save the machining model.
• Close all files, and Erase Not Displayed.
• Continue on to Step 2.

2. In the casting model, choose View, Model Setup, Color and Appearance.

Fig. 3. Color and appearances menu.		Fig. 4. Selection menu.

3. Change the selection box to Surfaces, and then select the Solid Surfs option (Fig. 4).

4. Pick anywhere on the model to select all of the solid surfaces, and choose the color to which you want to change it.

5. Open (if needed) and regenerate the machining model. All of the inherited surfaces appear in the new color. Note: You may have to force the regeneration by using the model player.

Only the surfaces of the cast/mold model inherit the new color. All existing and new “machining” features show the original color. This technique also provides a quick way to visually check on spotfaces and machining cleanup.

Other Pro/ENGINEER models that might benefit from this treatment are weldments, molded parts, and other parts that have secondary operations performed on them, such as a model of a purchased component that is then modified. In addition, you can use this technique on a single file model. Just color it using the above technique after the appropriate feature.

Marc DeBower is an engineering information systems analyst at Schneider Electric–Square D in Cedar Rapids, Iowa, USA. He can be reached by e-mail at debowerm@squared.com.