Remesh or generate a volume from imported mesh in ANSYS 2

[jiligeo]

Dear friends,

Normally a mesh is generated based on volume definition, is it possible to do it in opposite direction, namely to remesh or generate a volume from imported mesh in ANSYS?
Actually, for a biomechanical model, I have generated tetrahedral meshes in Amira software and imported it to ANSYS. (The import file contains the nodes and elements using N and EN commands)
As the quality of mesh is not good for FE analysing, I am interesting to change it in ANSYS.

Regards
Jalil

 

[cbrn]

Hi,
no, there is no direct "reverse-engineering" way to build a volume from a mesh. It would be something like rebuilding a waveform from a MP3 coding in audio, if you see what I mean...
If you have enough time to spend upon it, you could anyway:
1- identify the nodes at key locations of your model
2- create keypoints on these nodes
3- create lines (ANSYS calls "line" anything is 1-dimensional: can be straight line, spline, arc,...) connecting these keypoints; if you deal with free-form surfaces, this may be a bit tedious and needs a rigorous approach in order to correctly redefine the geometry
4- create areas through the lines
5- build volumes from areas

You may need several different volumes and several boolean operations in order to achieve this, but it's not impossible.

Good luck!

Regards

 

[ermpadt]

Jilil,

Yes, there are a couple of ways to do this. The difference is if you want to have the same surface mesh or if you want the mesh to be totaly different.

In version 11.0, you will be able to do this with the FE Modeler module. The resulting mesh will not have the same surface nodes as your original mesh.

You have been able to do it for years with ICEM CFD/ AI*Environment wich are other ANSYS, Inc. Products. This is the same approach that converts your external element faces into a faceted geometry representation and meshes it.

You can also do it in ANSYS now with the FVMESH command. You would need to "skin" your previous mesh with an ESURF then FVMESH. The elements will line up on the surface with your orignial mesh, so you can't refine with this option.

Hope this helps

Eric
PADT, Inc.

http://www.padtinc.com

Eric Miller

http://www.padtinc.com

 

[cbrn]

Hi,
Eric, what you say is very interesting, but I'm getting a bit confused about the result of the methods you describe:
- I don't know how v.11 FE-Modeler will work, but, unless it incorporates an engine for point-cloud interpolation and surface/volume reconstruction (an engine like this is nowadays costing as much as ANSYS-structural itself), it will most probably create a faceted-area geometry, which is definitely not the original one. Could be useful in many situations, but not for curved surfaces. Anyway, we're speaking about the future...
- ESURF will overlay surface elems upon existing solid elems, so I think it's hardly useful to Jalil: you say yourself that one "can't refine with this option"
- FVMESH will rebuild solid mesh starting from surface mesh, but once again: how would Jalil become independent from the original mesh?
- All this considered, I believe that, if we want to avoid manually rebuilding the geometry, it's far better to directly use local refinements.
- The case where your method 100% applies is if the existing mesh is satisfactory at the exterior ("skin") so one can keep it with ESURF, while the solid mesh "inside" has to be rebuild, so one can use FVMESH. Take care anyway to the fact that FVMESH is supported only by a subset of elements / meshers.

Regards

 

[jiligeo]

Dear friends, thanks a lot for your answers and sorry for delay in reply. I have used your idea and the results are as below.
As I explained before, the Amira output is nodes and elements and we can import them in ANSYS as nodes and elements or keypoints and solid volumes.
Because of the huge number of solid volumes (approximately 500 000) after 4 hours I could not import the volumes in ANSYS.
Another AMIRA output is exterior surface elements . I have imported them to ANSYS as Area successfully (approximately 10000 surface elements)but creating an arbitrary volume by areas was not successful after 4 hour.
Do you have any idea about the required time for this operation?

Regards
Jalil