NX X Flattening a Cylindrical Surface to see a Hole Pattern

NX for Design



In the case where a Cylindrical surface has a Pattern of Holes that you want to flatten and place on a Drawing Sheet, how can this be accomplished?


One solution would be to create a Tangent Datum Plane on the cylindrical surface and then use the Unwrap command to unwrap the face edges on to the Plane. 

You can then orient the Plane parallel to the screen, save a new view and add that view to the drawing sheet and use "Layer Visible in View" to turn off unwanted geometry.

  1. Menu --> Insert --> Datum/Point --> Datum Plane 
  2. Type: Tangent 
  3. Select the Cylindrical Surface --> OK

  4. Menu --> Insert --> Derived Curve --> Wrap/Unwrap Curve
  5. Choose Unwrap from the drop-down
  6. For Select Curve, select the Edges of the Cylindrical surface and the Holes 
  7. For Select Face, select the Cylindrical Surface 
  8. For Specify Plane, select the Tangent Plane created previously --> OK

  9. Menu --> View --> Operation --> Orient 
  10. Type: CSYS of Object --> Select the Tangent Plane --> OK

  11. Menu --> View --> Operation --> Save As --> Enter Name --> OK 
  12. Add the newly saved view to the drawing sheet.

Notes and References

Hardware/Software Configuration

Platform: INTL64
OS: window
OS Version: 1064
Product: NX
Application: DESIGN
Version: V1847
Function: CURVE

Ref: 002-7008378

KB Article ID# PL7008378



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