Creating Rule-Based Simplified Reps in Pro/ENGINEER Wildfire 2.0

Pro/ENGINEER Wildfire 2.0 gives you the ability to create rule-based simplified reps - similar to creating rule-based layers. You can define a simplified rep - based upon your own criteria - that will automatically update when new parts are added to the assembly.

As an example of this, we will look at a steering column assembly. We want to create a simplified rep that excludes all the hardware so we get better performance when working on the design. And, we want to be sure that any hardware added in the future will automatically become a part of this simplified rep.

1. Let's create a simplified rep called No_Hardware.
2. With the rep selected in the View Manager dialog box, select Edit, Redefine. (Figure 1)
3. In the EDIT: NO_HARDWARE dialog box, make sure the Exclude tab is selected and press the Setup Rule Actions icon. (Figure 2)
4. At this point, the NO_HARDWARE dialog box will come up. (Figure 3)
5. Press the + button to add a new condition to the definition of the simplified rep. A new line will appear in the box, defaulting to exclude parts that match the rule criteria, and with an undefined condition.
6. Simply right-click the undefined condition and select New to create a new condition.
7. Press enter inside the condition box to bring up the Rule Editor dialog box (Figure 4). If the Query Builder is not shown in the Rule Editor dialog box, click on the Options button at the bottom of the dialog box, and select Build Query. (Figure 5)
8. The next step is to create the actual criteria we will use to find all the hardware in our assembly. Unfortunately, we do not have a PART_TYPE parameter that has a unique entry for hardware components, so we will have to create our rule based upon the PART_DESCRIPTION parameter.
9. We will accomplish this by searching for all solid models that have the words "nut", "bolt" and "washer" in their description. To find all parts with the word nut in their description, set up the Rule Editor dialog box as shown in the Figure 6, and press the Add New button. Repeat this procedure, changing the Value field to "*Bolt*" and "*Washer*" to complete our rule definition for this simplified representation. (Figure 7)
10. After the Query Builder information is complete, select Preview Results to verify that we correctly defined our rule. Notice that in the preview box we see several parts in this assembly that are nuts, bolts and washers. This means we have correctly defined this rep, and we can press OK in the Rule Editor dialog box to complete our rule.
11. Finally, after pressing OK on all subsequent dialog boxes, we have successfully created our rule-based simplified representation.

An alternate way to do this exercise is to create a PART_TYPE parameter in each part (you can include this parameter in your start parts) and classify them as hardware, electrical, sheetmetal, etc. Then creating rules becomes easier and more accurate, as you do not rely on any consistency in part names or descriptions.

As one last note, if any parts are subsequently added to our assembly that have the words nut, bolt or washer in their description, they will automatically be excluded from this simplified rep.