NX X Are not able to add dimensions in sketch to external objects

NX for Design



You have a NX part with a solid model which contains several sketches. You now want to edit one of the existing sketches and add some dimensions with external reference, i.e. put a dimension between one of the sketch curves and a solid edge or a datum etc.
Using Rapid Dimension it is not possible to select any datum plane or axis. If an edge of the solid body is selected as first object it is not possible to select a sketch curve or vise verse. Selection scope is set to "Within Work Part Only", so it should be possible to select external objects.
Please note the pointer is hovering over a sketch curve, but the curve is not highlighted for selection. Sketch is indicated to need 2 additional constraints, i.e. position the sketch on the face.


One possible explanation to the above described behavior is that the sketch is positioned with Positioning Dimensions so called RPO dimensions, (Relative Positioning and Orientation). 
This type of positioning dimension where commonly used in older versions of NX (Unigraphics). RPOs are not allowed to be used on sketches which have associative sketch origin, which is the default in in later version of NX.

To be able to add sketch dimensions referring to external objects like solid body edges or datum planes/axis, you need to remove any existing RPO positioning dimension. This is done when you are in edit mode of the sketch through the command:
(Menu) --> Tools --> Positioning Dimensions --> Delete
When the positioning dimension Delete command is invoked, the positioning dimensions occur and you can select them, to be deleted.

Notes and References

Hardware/Software Configuration

Platform: INTL64
OS: windows
OS Version: 1064
Product: NX
Application: DESIGN
Version: V1899
Function: SKETCHER

Ref: 002-7007679

KB Article ID# PL7007679



Associated Components