NX X Convert to PMI creates PMI in specification part instead of UGMaster

NX for Design



Have a master model drawing, (specification, (UGPART)). Perform Convert to PMI
selecting a drawing view in drafting. The PMI objects are created in the
modeling workspace of the drawing part file.
I expect the PMIs to occur in the model workspace of the model part,
(UGMASTER). How to accomplish this?


To get the converted drawing objects, dimensions, annotations etc. to occur as
PMIs in the modeling workspace of the model in a master model relationship you
need to enable the "Create in Master Model Part" option.
This is found in the Convert to PMI Settings menu (Convert to PMI menu,
Settings icon bottom right in Settings group), under Conversion Process in
Conversion group.
Please note: In order to store a change done in the Convert to PMI Settings
menu you need to store a new conversion option file, (also in the Convert to
PMI Settings menu). In the Conversion Option File group under Conversion
Process, there is a Save Settings to File field you need to browse/enter a new
name in and finally press the "Save" icon. (Which will make the "Load From"
field display the same path/name).

If you still after this adjustment experience that the PMI data still only
occur in the modeling workspace of the drawing, there might be an issue with
NX not recognizing the drawing being a master model drawing.
When NX drafting performs Convert to PMI with "Create in Master Model Part"
enabled NX verifies that the drawing actually is a drawing in a master model
relationship, (specification). This is done by looking at the NX_NON_MASTER
attribute in the drawing part file, it should be NX_NON_MASTER=drawing.
If the attribute does not exist, please add it.

Notes and References

Hardware/Software Configuration

Platform: INTL64
OS: window
OS Version: 764SP1
Product: NX
Application: DRAFTING
Version: V12.0.1

Ref: 001-9131159

KB Article ID# PL8004230



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