When redefining the 'X-direction' of a Projected View, the selection scope
only has 'Within Work Part Only' as an option. If the drawing uses the master
model concept, the geometry of the part is not within the work part. How can
geometry from the part, such as edges, be selected to define the 'X-direction'
of the projected view?
Solution
Use the option 'Extracted Edges'. The edges will be extracted into the
drawing and can be selected.
1. Hover the cursor over the projected view border,
'MouseButton3-->Settings'.
2. Expand 'Common' and highlight 'Configuration'.
3a. Toggle 'Representation' to 'Exact'.
3b. Or toggle 'Representation' to 'Exact (Pre-NX8.5)'.
And also toggle on 'Extracted Edges'.
4. Select 'Apply' on the Settings dialog.
5. Expand 'Projected' and highlight 'Settings'.
6. Under the Orientation group, select 'Specify X-direction'.
The Selection Scope will still only have the option 'Within Work Part Only';
however, now there are extracted edges from the part that reside in the
drawing (work part) that can be selected to define the X direction.
Notes and References
Hardware/Software Configuration
Platform: all
OS: n/a
OS Version: n/a
Product: NX
Application: DRAFTING
Version: V9.0
Function: DRAWING/VIEW
Ref: 001-7188520