ICEM to Static Structural
 

Hello,

I am working on transferring surface meshes generated by Avizo software to Ansys for mechanical and thermal modelling. I followed steps below.

import surface mesh (.stl) to ICEM CFD as mesh, then create geometry through mesh to facets command, then repair geometry
-> Create volume mesh by octree, then repair mesh
-> connect ICEM model to FE modeler on Ansys workbench
-> connect FE modeler model to static structural model

https://www.cfd-online.com/Forums/at...1&d=1505839998

I think the flow chart should be correct but unfortunately I couldn't manage to get successfully generated parasolid geometry in FE modeler, therefore I couldn't use it in static structural. Surface mesh has over 2 million elements so I think it should be enough to create a convenient geometry and surface mesh. So I am certainly doing wrong at some point. Now I can still use final mesh in the static structural but then I cannot apply any force or fixed support because I cannot select only one face

Anyone can help me to find out what is the problem and how can I fix it.

Thank you for advance.

Hi,

You’re procedure is correct, nevertheless it’s not because you have a lot of elements (2M) that it guarantees you a successful parasolid geometry extraction in FE modeler. Do you have more details regarding the failure -> you should check under “problematic faces” that should be created in FE modeler when the solver failed the conversion.

You have several solutions:

• Improve the surface mesh with Avizo tools (I know that there should be some options there but used it a long time ago)
  
• Play around in ICEM with the repair tool / build topology tool
  
• Use tools to smooth the stl file (like Meshlab)
  
• Import the STL directly into Ansys Spaceclaim and rmb on mesh > convert to solid to generate a geometry file from the STL.
  
• Use directly the volume mesh you derived from ICEM and use it into Ansys structural / thermal (link it to the “model” component instead of the “geometry” component). You can’t apply a force or fixed support as they are scoped to geometrical entities but you can apply it directly on the selected nodes using command snippets with the corresponding APDL commands (using CMSEL and D commands for both thermal and structural DOF constraints on nodes -> look at the Ansys help > Mechanical APDL > Command Reference )

There could be other options but I often use one of the previously listed methods to get the job done.

Have fun ;)

Hi, thank you for your suggestions. I already did every possible improvements available in avizo, so it is probably the best one i can get. SpaceClaim can work but it takes too much time. Yesterday i tried with apdl commands on the selected nodes and it worked somehow, but still need to convert initial mesh to a normal geometry. The problem as you mentioned, problematic faces. I got 674 problematic face errors (i will check and share exact error message as soon as possible), so it was not huge shock to failed to get proper initial geometry after all. My surface is not flat and thus i think angle based skin detection doesn't work correctly. I used 15 degrees of tolerance angle, but maybe the correct approach should be detection by curvature method.

Yes, it’s a bit tricky and I had to deal with the same issues several times. There is not a “perfect” approach, depending on sample you try to analyse one of the above mentioned option can work in one case but not in the other…

To understand a bit more the “problematic faces” of FE modeller you can take a simple cylinder and mesh it in ICEM without attributing any “mesh face attribute”. So when you import it in FE modeller you’ll end up with one single component (see picture).

https://i.imgur.com/T9mwASB.png

If you insert a geometry tool (initial geometry) you’ll end up with problematic faces as the geometry can’t be described with a single surface (as you've started from 1 component).

https://i.imgur.com/KYDMqVb.png


So you’ll need to delete the initial component generated upon import and then start playing with the skin detection tool parameters (as you suggest either detection by curves or angle) also change the “forbid close components”.

https://i.imgur.com/4WpVRm3.png

Once you’ve initial geometry is successful you can rmb and convert it to a Parasolid. Once created you can still use the sew tool to glue the resulting components together.

https://i.imgur.com/2u3Q4o1.png

Good luck ;)

Hi,
Thanks for the discussion. Recently I have generated a volumetric mesh from STL file in ICEM and want to do the static structural fem in Ansys workbench. It seems that the "Geometry" component must be specified (present "?") instead of just linking to "Model" before I can proceed. I wonder why "File-Import Geometry-Faceted-STL" can't define as "Geometry". Do I need to create a geometry file from the STL? Your help is highly appreciated!
Crayon