To Create Drawing Views from Part Simplified Representations in an Active Drawing
When creating or editing drawing views of parts with part simplified representation, you can insert a drawing view for the part simplified representation within the same drawing sheet.
1. Open a drawing of a part with simplified representations.
2. Perform one of the following operations:
◦ Click
Layout >
Drawing Models.
◦ Right-click and click Drawing Models on the shortcut menu.
The DWG MODELS menu appears on the Menu Manager.
3. Click Set/Add Rep. The SELECT REP menu appears.
4. Select the required representation from the available list and click Done/Return.
5. On the
Layout tab, in the
Model Views group, click
General.
6. Click a location where you want to place the general view of the part simplified representation. The Drawing View dialog box opens.
7. Click View States. The View States category page is displayed in the Drawing View dialog box. The Simplified representation box displays the current representation. You cannot modify this representation.
8. The remaining options in the Drawing View dialog box are optional. If required, change these options and click Apply. The view of the part simplified representation is placed in the drawing.
9. Click OK. The Drawing View dialog box closes.
|  You can create drawing views only of part simplified representations that are created in Pro/ENGINEER Wildfire 3.0 or later, or updated to Pro/ENGINEER Wildfire 3.0 or later. |