Error in generating mesh for an imported file from solidworks 1

[ansyiq]

I have imported a para solid file into ansys and tried this 3D model to mesh but i keep getting the following errors


"vOLUME CANNOT BE MESHED.More than 2 surface elements share a common element edge. Check line 29 on volume 1"

If i change the element size from 0 then i am getting this error

"Error meshing area 16. There is a problem with the orientation of the boundary loops".

 

[cbrn]

You have a topological problem with the parasolid file. It seems there is a "free" surface "unlinked" from the solid model and exactly superimposed to it, like the one you can get if you create an "offset face" with 0 offset.
If you can't find out why from the original SolidWorks model, then:
- try to import the SW geometry directly with the SW-to-Ansys plugin
- from SolidWorks, save to Parasolid, then re-open the file in SolidWorks, then re-save. This seems absurd, but in this case there will be a double topological and geometrical check and sometimes it fixes some little errors.
- ... or trivially go to "Numbering Controls -> Merge Items -> All" inside Ansys, and set some acceptable merging tolerance. Also this can sometimes give good result.
- ... or, inside Ansys, select only the volumes (solid bodies), then UNSELECT all the Areas "attached to -> volumes". If, by plotting the areas, you find at least one, then "select -> everything below -> selected areas" and delete all (Ansys won't delete objects that are linkes to other "things", it will eventually give you some warnings that you can discard). Then ALLSEL in order to get back your model.

Hope this helps in some way...

Regards

 

[ansyiq]

Hi cbrn,

I tried the option of save to parasolid and resave. I dont have the import SW option with me. I am posting the error in detail so that i can be more in specifi. I appreciate your help

Regards



*** ERROR *** CP = 12.188 TIME= 22:
Volume 1 cannot be meshed. More than 2 surface elements share a
common element edge. Check line 29 on volume 1.

*** ERROR *** CP = 12.438 TIME= 22:
Volume mesh failure - perhaps due to:
(1) Poorly shaped triangle facets: Mesh surfaces with triangular
elements, modify mesh control to get good triangular mesh, then VMESH
again.
(2) Complex geometry: Subdivide volume and try again.

 

[cbrn]

Hi,
probably the problem is not inherent to a topological problem but to a meshing problem. There may be a set of surfaces where it is impossible for the mesher to "come" to the signaled edge "from" two adjacent surfaces in a coherent way. Probably there is a 3-sides surface which ends in a sharp corner, or something like that. Try and see if another message comes such as:
"initial attempt on area ### failed. Trying to automatically correct and remesh".
But before all, follow Ansys' suggestion and select line 29 ALONE, just to find out WHERE in the model it is and then, via the "select entities -> area -> attached to -> selected lines", which are the areas connected to this problematic edge.

Hope it helps...

Regards