Creating Intent Surfaces from Patterned Geometry
You can create a datum reference feature pattern of intent surfaces or intent chains from patterned geometry created in Creo Parametric. You can then apply simulation entities to this datum reference feature in Creo Simulate with a single mouse click. This procedure assumes you are working in Creo Parametric.
1. First create a Creo Parametric feature, for example a hole. Create a pattern of the feature. Refer to the Online Help for part modeling for instructions on how to create a pattern.
2. Click > > 
Reference. The Datum Reference dialog box opens.
Reference. The Datum Reference dialog box opens.3. Select Intent Surface from the Type list.
4. Select Intent Name and type a name for Intent:
5. On the model, select surfaces on the pattern leader for which you want to create an intent surface.
 | The selected surface must be from the pattern leader only. |
6. Click OK. Creo Simulate creates a datum reference which is visible on the model tree.
7. Select the datum reference on the Model tree and click the right mouse button. Select Pattern. The pattern dashboard is displayed but no options can be selected. This is a pattern of intent surfaces for which you created a datum reference feature.
8. Click 
to create the datum reference pattern.
to create the datum reference pattern.9. Click to create a second intent surface datum reference feature. Select Intent Surface from the Type list.
to create a second intent surface datum reference feature. Select Intent Surface from the Type list.10. Click the Creo Parametric search tool 
to open the Search Tool dialog box.
to open the Search Tool dialog box.11. Select Intent Surface under Look for:. For Criteria select Comparison: is equal to. Type the name of the first datum reference feature you created.
12. Click Options and select Save Query To Feature on the drop down list. Click OK.
13. Click OK on the Datum Reference dialog box. This completes creation of a datum reference feature for intent surfaces of the pattern in Creo Parametric.
While working in Creo Simulate you can apply simulation entities such as loads and constraints to a pattern of surfaces using this datum reference feature. If the pattern geometry is updated in the Standard application the simulation entities applied to the pattern datum reference feature are also updated.
| | You can also create a datum reference feature for intent chains using the same procedure as above but select Intent Chain instead of Intent Surface. |
Return to Intent Objects.