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How can I fill or delete voids in a part?

I've got a complicated part with some complex internal geometry.  I want to simplify it by deleting or filling in all the internal voids.  All I care about is the outer shape.  Does anyone have any ideas on how to do this?


Put another way, I only want the faces that I could paint or would be needed to render the part.  The internal geometry is just taking up space and is not needed. 





Re: How can I fill or delete voids in a part?

Hi Mark,


what version of NX are you using?  if you are using NX9/NX10 you could do the following:


1. copy / WAVE link you geometry so you can maintain the original design

2. new file -> copy solid geometry to another layer

2a. NX selection group, make sure the All But Selected is available

3. using Synchronous -> Delete Face -> Selection intent = Boss or Pocket Face -> select the internal faces (NX will highlight them) -> select All But Select button

4. if the cap faces are not fill, then using surface -> Fill Surface

5. Unite 2 solid bodies






Sam Kuan

Re: How can I fill or delete voids in a part?

You could use linked exterior.  If you can make a part that can cover over big openings.  (Die Castings for Example).  Then use Linked exterior this could possibly remove your internal surfaces.  Just depends on how accurate you are wanting it to be.  Does require advanced assembly license.

Re: How can I fill or delete voids in a part?

If you have Checkmate then there is a check that can remove voids.

SASIG-PDQ -> Solids -> Solid void


This check has a heal option.  If you use the heal option then it will create a Delete Face feature for the interior voids. 

Rick Hebert
NX Magician
Used NX (Unigraphics) since 1984
Houston, TX, USA