Showing results for 
Search instead for 
Do you mean 
Reply
Solved! Go to solution

Assembly FEM. Partially meshed problem

Hello!
When I mesh geometry by making 2d mesh and then extruding elements to chexa8 and then trying to solve I have warning on my face to face gluing constraints


"WARNING
SSSO "Face Gluing(1)" is applied to geometry that is partially meshed or not meshed at
all.
This may be due to the presence of a tiny edge in the geometry."

What I'm doing wrong?

 

I have made little assembly exactly the way as the "real" one just to illustrate the problem.

6 REPLIES
Solution
Solution
Accepted by topic author guga50
‎11-30-2015 10:48 AM

Re: Assembly FEM. Partially meshed problem

Your glue simulation object is defined with regions containing polygon faces. Your solid meshes aren't associated to the geometry since you extruded them manually from 2D elements. Since there's no association between the polygon faces and the solid mesh, geometry based boundary conditions won't find the "related" meshes. There are 2 ways to solve this.

 

1. Define/edit regions using the solid element faces

2. Use 3D Swept Mesh to generate associated solid meshes

 

For the first option you just need to edit the existing regions to use element faces. The 2nd option would let you use the glue regions as is, but requires that you delete the existing 3D meshes and generate new ones using the geometry.

 

Regards,

Mark

 

Mark Lamping

Simulation Product Management

Simulation and Test Solutions

 

Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.

 

mark.lamping@siemens.com

www.siemens.com/plm

Re: Assembly FEM. Partially meshed problem

I've already chosen the second one. Thank you.

Re: Assembly FEM. Partially meshed problem

Hi what do you mean by edit regions?

Could you please explain more  about this?

I have a problem .I have a sheet body which have a bolt hole at the middle.So i have to split it into three bodies ,i have swept the end bodies but the middle one i have extruded from a 2D mesh. I have connected them through mesh mating.My results seems pathetic.

Re: Assembly FEM. Partially meshed problem

All I see are solid meshes in your images. I can't tell at all where you expect the mesh mating conditions to be. Mesh mating conditions is designed to connect solid bodies together at shared face boundaries. It won't connect manually extruded meshes to other meshes. If that's your expectation, then your expectation is wrong, and I agree the result would be pathetic. Why can't you sweep all of the bodies and avoid extruding solid elements from a 2D mesh?

 

Regards,

Mark

Re: Assembly FEM. Partially meshed problem

Hi Mak

Thanks for reply.

1.The body is not sweepable that's the reason i had swept one portion and extruded the other .

If you could see image-1 you can find two hole on the top view.This has to be splitted into two bodies to achieve a hex mesh.

2.I do wonder why doesn't a mesh mating works between extuded and swept body.

Glue Coincident mesh mating-makes both the geometry and the meshes match between the source and the target faces.So mesh and goemetry gets glued eventhough i split them into two halves.By what ever ways i have created a mesh all nodes had to match.

3.If you could see results (the last image in earlier post ) it was about to split into two halves

4.I haven't associated the extuded mesh with the geometry as i am using NX8 .i doubt i dont have that option to associate extruded mesh and the geomerty .I hope when i associate them and using mesh mating condtion guess the results got to be ok.

5.I haven't tried it yet as i have to try them in NX10.

 

 

 

 

Re: Assembly FEM. Partially meshed problem

Mesh mating supports mating of bodies created from different design features and assembly components. I'm not sure why you're having problems getting a mesh mating condition between your swept body and your extruded body. As long as the bodies have coincident faces where you'd expect the mesh mating condition, then you should be able to generate a mesh mating condition. 

 

Maybe the simplest way for you to do this would be to unite your two bodies into a single body. Then split the body into two using Split Body and a datum plane. Turn ON the option to automatically create mesh mating conditions. In the FEM you'll end up with 2 bodies that share a face at the split's datum plane and meshes will be connected at that face.

 

Regards,

Mark