NX X How to merge a separate drawing file into its related part file in Teamcenter

NX for Design



How to merge the non-master drawing file into the related part or assembly 


 1. Start NX & Teamcenter. 
2. In NX, open the drawing in the Drafting application. 
3. Select 'File-->Export-->Part'. 
4. Set 'Part Specification = Existing'. 
5. Select the 'Specify Part' button. 
6. Browse to the related part or assembly dataset you wish to 
 merge the drawing into. OK the dialog. 
7. Set the following: 
 Specify Exported Position = OFF 
 Object Select Scope = Work Part Only 
8. Select the 'Class Selection' button. 
9. Select the 'Select All' icon. OK the dialog. 
10. Select the 'Drawing Selection' button. 
11. Highlight all sheets. OK the dialog. 
12. Set the following: 
 Feature Parameters = Retain All Parameters 
 Expression Transfer Mode = Copy if Referenced 
13. OK the Export Part dialog. 
14. NOTE: A message may appear reporting that not all objects can be exported. 
 If so, select the 'Details' button to see the list of 
 objects that cannot be exported. OK the details dialog. OK the message. 
15. The export will complete. Select 'File-->Save All'. 
16. Close the drawing. 
17. Open the related part or assembly file. 
18. Switch to the Drafting application. 
19. In the Part Navigator, double-click on a sheet to make it active. 
The drawing should be available. 
Be sure to test to make sure dimensions and other associated entities will 

Notes and References

Hardware/Software Configuration

Platform: all
OS: n/a
OS Version: n/a
Product: NX
Application: TRANSLATOR
Version: V8.0
Function: DXF_DWG

Ref: 002-7005675

KB Article ID# PL7005675



Associated Components

CAD Translators