I need to clean the assembly for import to Teamcenter.
Where in native NX 11 is "clean" assembly function ?
This is a large 500-600 parts assembly.
Ok. It is Part Cleanup. Not Assembly Cleanup ( It does not exist.)
- How to use Part Cleanup for my purposes ?
What to press to remove those ghost parts in Import into TC ?
I think the one you are most interested in is "clean interpart links". For cleaning files before import to TC, I'd suggest using all the moderate cleanup/delete actions. In your screenshot, the "work part" is selected; meaning only the work part will be cleaned. There is another option for "entire assembly" (or "all components" or something like that) to clean the entire assembly. The components probably need to be fully loaded for this to work and you will need to save them after cleanup to make the changes stick.
I'd suggest turning on the "delete unused objects" option as well. It is a bit confusing because if you turn off timestamp mode in the part navigator you will see an "unused items" folder that lists objects that have no dependents. The cleanup option is NOT referring to these objects; it will not delete unused points or curves that are displayed onscreen. Rather it refers to internal objects (such as Xforms and scalars) that NX uses to maintain associativity between objects. Sometimes these internal objects hang around in the file after the geometric objects are deleted.
And if all else fails:
- look for inter-part expressions
- look for WAVE links (if you have an Advanced Assemblies??? license there is a link browser that can help)
- are there any other ways stuff can be refernced? (views on drawings? ???)
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
One common cause is files renamed on the OS.
For example, if you rename one of the components (or assembly) using the rename option in Windows Explorer from bracket.prt to bracket_lhs.prt, the Import Assembly into Teamcenter command will try to import both files, because renaming on the OS does not rename any internal references to the filename, it just renames the externally displayed name of the part file. Therefore, ALWAYS use the Save As command in NX to rename a part file!!
You have been warned