How to Place a Drawing View of a Part Simplified Rep

Simplified representations of parts can be very useful when designs become complex. Regeneration time can be greatly improved and model display simplified by excluding unnecessary features. One of the few drawbacks of part simplified reps, however, has always been the inability to place views in a drawing mode. This technique shows how to get around this limitation easily.

1. Create a part simplified rep to exclude complex features.

Figure 1. Master Rep of Gear		Figure 2. Simplified Rep (NO_TEETH)

2. Create an assembly and assemble just the gear part.

3. Now create an assembly simplified rep by selecting Simplfd Rep, Create, and enter a name. Select Master Rep as the default rule, select Substitute, and select the gear part from the model tree.

4. Select the NO_TEETH part simplified rep to substitute into the assembly simplified rep.

Figure 3. Creating the Simplified Rep

5. Now you can place a drawing view of the assembly simplified rep, which contains only the part simplified rep.

Figure 4. Drawing View of Rep

Florin Neamtu is a senior technical support engineer at PTC. He can be reached by email at fneamtu@ptc.com.