NX X How to project the perimeter of a model onto a datum plane

NX for Design



How to project the perimeter of a model onto a datum plane.


This method will only include the perimeter or envelope of a part or an assembly. 
  1. In the Part Navigator, expand the Model Views node.
  2. Select the desired Model View, 'MouseButton3 (MB3)-->Make Work View'.
    This will be the view of the part or assembly used to create the perimeter. 
  3.  Add a datum plane at the desired location and orientation to project the perimeter onto.
  4. Select 'File-->Preferences-->Visualization Preferences'.
  5. Select the 'Visual' tab.
  6. In the Select Views group, select the view you want from step 2.
  7. In the General Display Setting group under Part Settings (Selected Views) subgroup, set the Redering Style to 'Wireframe'.
  8. In the Edge Display Settings group under Part Settings (Selected Views) subgroup, set Hidden Edges to 'Invisible' and OK the dialog.
  9. In the Menu, select 'Insert-->Derived Curve-->Extract'.
  10. Select 'Shadow Outline'. Select OK and then Cancel. 
  11. Hide any components or geometry, so that only the Shadow Outline curves are visible.
  12. In the Menu, select 'Insert-->Derived Curve-->Project Curve'.
  13. Select the Shadow Outline curves for Curves or Points to Project.
  14. Select the datum plane for Objects to Project To.
  15. Specify the vector for the Projection Direction.
  16. [optional] Uncheck 'Associative' in the Settings group.
  17. OK the dialog.
NOTE: If needed later, the Shadow Outline curves can be deleted and the components or geometry can be made visible again.

Notes and References

Hardware/Software Configuration

Platform: all
OS: n/a
OS Version: n/a
Product: NX
Application: DESIGN
Version: V11.0
Function: CURVE

Ref: 001-9220680

KB Article ID# PL8004759



Associated Components