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NX 11 make solid Feature

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor

Hello Guys,,

 

   There is a new option in NX 11 called Make Solid that is in 
Menu--insert--combine--make solid

What is the use of this becoz i tried creating set of closed sheets for making this into a solid.But whenever i select this feature nothing is working..i'm unable to select the sheets i created..

 

 

any Solutions???

11 REPLIES

Re: NX 11 make solid Feature

Siemens Phenom Siemens Phenom
Siemens Phenom

From Documentation

 

"Use the Make Solid command to convert any facet or analytic closed sheet bodies to solid bodies."

 

"Use the Sew command to join two or more sheet bodies into a new single sheet body. If the collection of sheet bodies encloses a volume, a solid body is created. The selected sheet bodies must not have any gaps larger than the specified tolerance, or the resulting body will be a sheet body."

 

If the sheet bodies are created within NX, use 'Sew' and check the result.

 

Re: NX 11 make solid Feature

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor

Thanks Ganesh Smiley Happy

Re: NX 11 make solid Feature

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi,

The Make Solid command  takes a fully enclosed sheet body (or facet body) and makes it solid. At times when you import a body and even though it’s closed, it is still a sheet body then you can use MAKE SOLID to get a solid out of it. It supports b-rep or facet but must be fully enclosed.  

If it does not work for you please check the SHEET BOUNDARIES(examine geometry) once you sew all the sheet bodies and try to get rid of any boundaries. It sshould work then.

Best Regards

Kapil

Re: NX 11 make solid Feature

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor

Hello @kapilsharma,,

 

  Thanks for responding.Yeah i've tried the methods you suggested but, nothing is working it is not selecting the sheet bodies and i've tried with the facet bodies also.

Re: NX 11 make solid Feature

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi Karthik,

Not sure...but can you share the model if possible?

Best Regards

Kapil

Re: NX 11 make solid Feature

Siemens Phenom Siemens Phenom
Siemens Phenom

Karthik:

 

I did not see you confirm Kapil's question about if you have any free boundry edges or not.

You should NOT have any for this command to work (when you use Examine Geometry, you will not find any Free Boundry edges).

So the geometry will look like a Solid, completely sewn up and appearing "water tight", but will not be Solid. It's like a balloon with just the outer shell but hollow inside. The command will convert it go Solid, but nothing with change with geometry or topology.

If you do have any free edges, you need to Sew them closed first. This command does not do that for you.

I have seen this myself when wokring with certain geometry imported from other CAD systems.

Just recently I was also taught a method to create a fake case inside NX to test is:

   Set Preferences -> Modeling -> General -> Body Type to Sheet

   Sew sheets to "solid" (e.g. 6 faces into a cube)

   The result is a Sheet that looks Solid.

One more thing, in my tests I found that unless I had the Associative toggle ON, I could not select the Sheet. I'm still not sure why and in my real cases always wanted it ON anyway, so did not bother investigating further.

Hope this helps!

 

Re: NX 11 make solid Feature

Siemens Phenom Siemens Phenom
Siemens Phenom

@PatMcManus,

I found the same thing - Associative must be checked to select the body, but it can be unchecked once the body has been selected.  In the process of testing I also found that importing STL data into NX needs to be imported as Convergent.

 

I used the same fake case starting off with a block, unsewed one face, changed the 'Body Type' Modeling preference to Sheet and sewed everything back together again.  I originally couldn't select this sheet body (as Associative was unchecked) so I exported it as STL to import it back into NX as faceted and ultimately convergent.  Associative still had to be checked to select this convergent body.

 

Regards, Ben

Re: NX 11 make solid Feature

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor
Thanks mate.. It's working Smiley Happy

Re: NX 11 make solid Feature

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor
Thanks mate Smiley Happy Now i am able to select the sheet body and make it to solid