NX 'Feature Parameter' annotation not created on an assembly drawing in NX 11

The NX Drafting 'Feature Parameters' command does not create any thread dimensions on an assembly drawing in NX 11.


The 'Feature Parameters' command is 'legacy' functionality, but it can be used 
in NX 11, if required, when working with 'Exact (Pre-NX8.5)' views.


When a view of an assembly model is created in NX 11 the default behavior is for the view to reference the default arrangement of the assembly. (In previous versions of NX, no specific assembly arrangement was referenced by the drawing view unless it was specifically selected during the view created process.) The use of assembly arrangements in a drafting view is not supported by the 'Feature Parameters' command, in any version of NX, however now that an assembly arrangement is used by default in NX 11 it gives the impression that the 'Feature Parameters' command no longer works for assembly views.

Solution

In order to create a view in Drafting that does not reference a specific assembly arrangement, the user should select the 'No Arrangement' option in the 'Arrangement to Use' list, in the 'Base View' command dialog.

The 'No Arrangement' option is not enabled by default and is controlled by the customer default 'Always Show 'No Arrangement' Option', under 'File - Utilities - Customer Defaults - Drafting - General/Setup - Standard - Customize Standard - View Workflow':

After turning ON the 'Always Show 'No Arrangement' Option', 'Save' the changes to the Drafting Standard, exit and restart NX. 

Notes and References

Hardware/Software Configuration

Platform: INTL64
OS: window
OS Version: 764SP1
Product: NX
Application: DRAFTING
Version: V11.0
Function: ANNOTATION

Ref: 001-8346427