Exporting Step file of assembly does not retain the assembly structure 1

[CAD Application Support]

Hi All,

NX1892. I have been trying to export a step file of an assembly and import it and retain the assembly structure. But everytime I export the file and using Open >> Part type Step >> choose the file i exported, NX opens the assembly into a single part without retaining the assembly structure. I use Menu >>File>> Import >> Step 214 and import the file by making sure I uncheck flatten assembly, still NX does not retain the assembly structure.

How can I fix this issue? I want to see the assembly structure of the file I exported when I import it back into NX.

 

[cowski]

[ul]
[li]Make sure that your current load options can find all the components of your assembly.[/li]
[li]Use the "entire part" export option in the STEP export dialog.[/li]
[/ul]

www.nxjournaling.com

 

[CAD Application Support]

Hi Cowski,

Using Entire part would export datums, sketches etc if they are in the reference sets of the component , isnt it? We dont want that.

We are trying to export the assembly as step from Teamcenter, so that person can open that step file in native session and work on the assembly.

 

[cowski]

In the export dialog, turn off the object types that you don't want to export and give it a try.

www.nxjournaling.com

 

[Toost]

When you export, IF you do a "manual selection" , i.e pick the objects to export, the export will NEVER be an assembly, always a single part.
Is this the case ?
You can do a "displayed part export" but be aware that you need to either suppress components that should not be exported or set these components to reference set=empty, else they will be exported.

Regards,
Tomas

 

[cowski]

We are trying to export the assembly as step from Teamcenter, so that person can open that step file in native session and work on the assembly.

Are you planning on bringing the changed files back into TC? If so, I'd suggest using the "export assembly outside of TC" command so the user gets the fully parametric files to work with. Once they are done with the files, you can re-import them to TC, overwriting the existing files or creating new revisions as necessary.

www.nxjournaling.com

 

[lklo]

Hi - If you are dealing with a Managemode Session, then simply:
1.Export entire assembly out of teamcenter, as an NX assembly.
2.Fire this Native assembly up in a NX native session.
3.In > File > Save As dialog, change the format from .prt to .stp ( see inside the dropdown )

lklo

 

[CAD Application Support]

Hi All,

Got it .. Thanks so much for the response..