How to Create a Reference Set for Different Features.
SolutionSee the above video showing the procedure for creating a reference set for different features.
This can be used when adding the part as a component and using reference sets to show two versions of the same component.
How to Create a Reference Set for Different Features
Creating the Demonstration Model & Extracting Geometry
1. Open a part file.
2. In the Top Border Bar, select Menu -> Insert -> Design Feature -> Cylinder.
3. Choose the Home tab -> Synchronous Modeling group -> More -> Extract Geometry.
4. In the Extract Geometry window, change the drop-down to Body.
5. In the Settings group, check Fix at Current Timestamp.
6. Select the desired body.
7. Click OK.
8. In the Part Navigator, right click on the Extracted Body and select Hide.
9. Choose the Home tab -> Construction group -> Sketch.
10. Select the desired plane.
11. Click OK.
12. Using the Curve commands, create a sketch to be revolved.
13. Click Finish.
14. Choose the Home tab -> Base group -> Revolve.
15. Select the sketch and set the revolve details as desired.
16. Click OK.
Creating the Reference Set
1. Choose the Assemblies tab -> Context group -> Reference Sets.
2. Click Add New Reference Set.
3. In the Reference Sets dialog, change the Reference Set Name as desired.
4. In the Part Navigator, select the feature that will be made into a Reference Set.
5. Click Add New Reference Set.
6. Change the Reference Set Name as desired.
7. In the Part Navigator, select the Extracted Body.
8. Click Close.
Using Reference Sets
1. In the Part Navigator, Show the Extracted Body.
2. Choose the Assemblies tab -> Base group -> New Parent Assembly.
3. In the Resource Bar, choose the Assembly Navigator.
4. In the Assembly Navigator, right click on the body.
5. Choose Replace Reference Set and select the desired Reference Set.
- Note: From here, the Reference Sets can be toggled.