A drawing has been created inside the part file without using the Master Model
method. How to now export the drawing inside the part file into a new drawing
specification file.
Solution
1. In managed NX, open the part file containing the drawing.
2. Select 'File-->New'.
3. Select a drawing template to create a new specification.
This will add the part file as a component to the specification just
created.
4. Select 'File-->Save' to save the part and the new specification file.
5. Make the component part file the work part.
6. Select 'File-->Export-->Part'.
7. Part Specification = Existing.
8. Select the 'Specify Part' button.
9. Select the specification file created in Step3.
10. Select the appropriate sheets from 'Drawing Selection'
11. OK the dialog.
The drawing sheets will be imported to the specification file.
12. Make the specification file the work part.
13. Switch to the Drafting application.
14. Select the sheet from the Part Navigator, 'MouseButton3(MB3)-->Open'.
15. Select the drawing in the Part Navigator, 'MB3-->Update'.
NOTE: The dimensions might lose associativity, but the views will update.
Retained dimensions can be re-associated. Check to make sure changes to the
model will update in the drawing views.
16. After verifying the drawing sheets in the specification file are
up to date, make the component part file the displayed part.
17. Delete the drawing information out of the component part file.
18. Make the specification file the displayed part and save all parts.
Notes and References
Hardware/Software Configuration
Platform: all
OS: n/a
OS Version: n/a
Product: NX
Application: NXMANAGER
Version: V7.5
Function: FILE_NEW
Ref: 001-6872668