Cancel
Showing results for 
Search instead for 
Did you mean: 

How to fix geometry created in Solid Works and opened in NX?

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Hello guys,

 

Our customer sent us a file which was (probably) originally created in Solid Works, then translated into Solid Edge, and finally opened in NX.

 

The problem is corrupted geometry, which I am trying to modify with Synchronous Modeling commands: Move Face, Delete Face, Move Edge etc. See pic1.

 

In addition, the body reports a problem when I am trying to use Measure Body. (pic2)

 

I used Heal Geometry and Optimize Face, but it didn't succeed.

 

How should I fix the geometry? Please help! 

5 REPLIES 5

Re: How to fix geometry created in Solid Works and opened in NX?

Siemens Esteemed Contributor Siemens Esteemed Contributor
Siemens Esteemed Contributor

Hi @Lidia,

 

You might find that you have to remove more than you expected to cleanup those faces.  For example, try removing the entire blends colored grey using Delete Face.  Unfortunately the Synchronous Modeling commands are not quite as straight forward as one would hope in these cases - you may have to get inventive.

 

Regards, Ben

Ben Broad | PLM Enthusiast | Siemens GCSS

NX (v17 - 1876) | Teamcenter (9 - 12)
Value Based Licensing | Adaptive UI | BETA Registration

Re: How to fix geometry created in Solid Works and opened in NX?

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Start with the 'examine geometry' command. Turn on all the body and face checks, rectangle select around the entire model, and press OK; this should highlight the problem areas that need attention.

Re: How to fix geometry created in Solid Works and opened in NX?

Phenom
Phenom

You will probably have to sew, unsew faces, delete face command with heal turned off, then finaly use fill surface command to fill in the open surfaces.  You will then need to sew everything back together into a solid body

Re: How to fix geometry created in Solid Works and opened in NX?

Gears Phenom Gears Phenom
Gears Phenom
@Lidia,

There isn't a really straight forward answer to what might be the root of the issues - I see some really bad faces - look at that X shape in the background in the lower left area.

Some things that might help:

Make sure you're expanding all the options on your Delete Face dialog - some of the choices in there will directly impact your success or failure on deleting blend faces (or what should be blend faces), such as Delete Partial Blend.

Sometimes it might help to first try to see if NX is recognizing a blend face by first seeing if Resize Blend will work - if it does, don't resize it, just exit the command and then try delete face - make sure you try to select in reverse order of blending as that can sometimes impact success or failure on a non-optimized model. Also, keep selecting blend faces - don't stop with just a couple if it comes back with "I can't do this" types of errors - maybe start on another set of blend faces on top or bottom and make sure to try the whole chain (which equates to possible 1 blend feature in NX).

Lastly, and I would use this sparingly, is the use of Optimize Face - sometimes it's really helped me, when other times it just makes a mess of things.
Tim
NX 11.0.2.7 MP11 Rev. A
GM TcE v11.2.3.1
GM GPDL v11-A.3.7
Highlighted

Re: How to fix geometry created in Solid Works and opened in NX?

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Thank you guys!!! You helped me so much!!!

 

I made several steps to fix it:

1. I deleted all the blends that didn't cause problems.

2. I copied arc of the problem corner using Composite Curve.

3. Then I unsewed the model using Delete Face with the Heal checkbox off and got a sheet body.

4. In the problem corner I created a surface using Through Curves Mesh on the copied arces, then I sewed the model with this surface. The new solid body became more NX-friendly and I was able to use Delete Face on the problem blend!