NX What's the process to convert drawing from UGMASTER to specification?

Is there a Workflow or utilities to help users to convert a UGMASTER to a specification drawing?

Currently there is no such utility. But there is the workflow below to accomplish this.

1. Load the UGMaster data (can be a single part or an assembly) into NX.

2. Find out the unit of this NX data (metric or inch unit).

3. Go to File > New command, using Drawing template to create a new empty drawing dataset (specification dataset). Be sure to use template from correct units.

4. Do not put any Base View in this newly created specification drawing. Save the drawing.

5. Close All Parts in NX.

6. Open the UGMaster data into NX again (don't open its specification drawing).

7. Execute File > Export > Part command. Use following options:

  a. Part Specification: Existing

  b. Click on Specify Part button and choose the UGPart dataset (the specification dataset that was created from step 3). OK.

  c. Click on Drawing Selection button and highlight the sheet(s) to export. OK.

8. OK the Export Part dialog.

9. Close All Parts in NX.

10. Now load the specification drawing dataset created in step 3 into NX.

11. Go to PNT and delete Sheet 1.

12. Activate Sheet 2 (and all other sheets of there is more sheets). Confirm all views contain geometry and annotation are there. Update sheet if needed.