NX Parts list callouts unexpectedly change when (native) partslist is added.

The callout column shows the correct callout numbers as they have been assigned through the TC-Structure manager (BVR). 
In Native NX, the moment you click the parts list command the callout values (see in the callout column in assembly navigator) is instantly changed and re-numbered with incremental numbers.


The callout numbers should not change and remain the same as assigned in the TC BOM (BVR). 

Solution

The behavior you see is default for NX-native. This is because the partslist definition has by default, for a native partslist, following setting for the callout:
 
  Default Text :  $~C

This makes the partslist "the engine" (number generator) to generate the callout-values. It will generate and populate (also update) the callout attributes. If the parts list should not generate callout-numbers, than the parts list column for the Callout has to be set to load the value from attribute Callout:

   Default Text :  <W$=@CALLOUT>

If you change the default partslist in Drafting Standard to e.g. ...\NX1980\UGII\table_files\generic_parts_list_pdm_metric.prt, then the Callout column is <W$=@CALLOUT>, and the callout is not renumbered.

Usually company would have another layout, and you can set that as default parts list, as long as the Callout columns is set correctly. Add this partslist in NX then uses that partslist as template:

Tip: You also can setup a (table-)Palette which contains this (and other) partslist-definition, then you can Drag&Drop any variant you define onto a drawing. 

Notes and References

Hardware/Software Configuration

Platform: INTL64
OS: windows
OS Version: 1064
Product: NX
Application: DRAFTING
Version: V1980
Function: TABLES

Ref: 001-10159223