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Derive .prt file

Valued Contributor
Valued Contributor

Hello to all,

I am searching for the best way to derive or import .prt inside .prt. What do you suggest?

I am using CRTL+C / CTRL+V. Durring that I have to redefine some references such as planes..etc.. so I would like to import part inside a part without any additional settings and redefinition except where to place.

Exporting to .iges and import is a fine method but it explodes my model on thousands of bodies.

 

Best,

Danijel

9 REPLIES

Re: Derive .prt file

Siemens Phenom Siemens Phenom
Siemens Phenom
File > Export > Part.
Can be exported to the existing or new part file. There are many other options that can be used as per your requirement.

Re: Derive .prt file

Legend
Legend

All depends on what your intent is or why you are importing a .prt into another .prt.

If you just want a non parametric Solid then exprt Parasolid.

If you want it to be Parametric then yes you have to copy Feature and attach.

Are creating some sort of dumb assembly (why would you? I would always use add Component)

Re: Derive .prt file

Siemens Phenom Siemens Phenom
Siemens Phenom

There's also "File > Import > Part", which imports the entire part, including attributes. "File > Export > Part" allows you to select geometry from multiple parts in an assembly.

 

As @joewhite stated, it all depends on your intent.

 

Importing Parts

Exporting Part Data

 

Regards, Ben

Re: Derive .prt file

Valued Contributor
Valued Contributor

Hello,

The reason is an .iges file (solid body) exported from other CAD system. I only need some surfaces (so I have extraced them from model) and planes. Now I need to import them to another part to use as input for further modeling.

I have done that by exporting to .iges (I don't like to do that) and to import as iges in another part. After process of import, there are thousand of "bodies" (each body is an surface) in modeling three that I don't like also.

I would like to export the surface in one piece and to import the surface in one piece also.

Capture.PNG

 

 

 

 

Re: Derive .prt file

Valued Contributor
Valued Contributor
BTW, Is there any specific reason to export a solid as Parasolid? Is it better that other export formats?

Re: Derive .prt file

Siemens Phenom Siemens Phenom
Siemens Phenom

Export Parasolid will remove all parameters from your geometry, but it will allow you to select the extracted surfaces to be exported into a single *.x_t file which you can then import into your destination file using "File > Import > Parasolid".  Alternatively, use @GaneshKadole's solution, to use "File > Export > Part".  You can specify the destination part and use Class Selection to select the extracted surfaces.  These will arrive in the destination part as "Extracted Face" features.  If you unchecked the Associative option when extracting the surfaces then they will arrive as "broken" (unlinked) Extracted Face features (meaning their associativity to their parent part has been broken), otherwise the parent geometry will also be imported.

 

Regards, Ben

Re: Derive .prt file

Siemens Phenom Siemens Phenom
Siemens Phenom
Since Parasolid is the modeling kernel for NX, the exported data is identical to the original. IGES, STEP or other translators do not guarantee the exported geometry to be identical to the original.
Regards,
Abe

Re: Derive .prt file

Valued Contributor
Valued Contributor

@Abeinjapan wrote:
Since Parasolid is the modeling kernel for NX, the exported data is identical to the original. IGES, STEP or other translators do not guarantee the exported geometry to be identical to the original.

Thank you for the clear answer!

Re: Derive .prt file

Siemens Creator Siemens Creator
Siemens Creator

I'm perhaps missing the point, but wouldn't wave linking (un-associative) be another approach to solve this task?