Have inherited model PMI and PMI section view to drafting. All options for PMI have been turned on under Settings -> PMI for both the PMI section view and the PMI base view where the Cutting Plane Symbol show in modeling, but no section line, symbolizing the PMI cutting plane, is shown in drafting.
How to accomplish a section line related to the PMI cutting plane symbol?
Solution
PMI Cutting Plane Symbol is not inherited to a drawing view in drafting directly through the same function as other PMI objects. This is due to a section line for a section view being related to 2 views, the parent view where the section line is displayed and the section view itself.
To get your PMI Cutting Plane Symbol to show in drafting as a section line you need to use the Section Line command in drafting with Type: Derived. This can be done with the following procedure:
In NX drafting with a drawing file containing a PMI section view and a base view where you want to show the section line.
- Invoke Section Line command
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Please note: If you only have one view in addition to the PMI section view the command immediately launches the sketcher, (to draw a section line) and graphics window zoom in on base view (imported view). Press "Finish" on the sketch. You get a "Section Line Definition" message with the question, "Do you want to fix the section line definition?, press <No>
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- In the Section Line menu, set Type: Derived
- Select the PMI Section View as Source View either in graphics window or in Part Navigator
- Select the base view as Parent View, (the view where you want the section line to be displayed)
The PMI Cutting Plane Symbol will now display as a Section Line in your parent view
- OK on the Section Line menu.
Done!
Notes and References
Hardware/Software Configuration
Platform: INTL64
OS: window
OS Version: 10_1709
Product: NX
Application: PMI
Version: V12.0.2
Function: SECTION_VIEW
Ref: 001-9414842