[EphemeralMemory]

Hey, all, thanks for reading this post.

I have a few questions about meshing... for one, which applications work well with relatively large and complicated STL files.

Currently, I use Gambit 2.4.6 to turn ~30K Element STL Meshes into ~1.5 Million Element .msh files which can be read into Fluent. My problem is, I use the Windows version, which is a 32bit application. I can create the mesh files, but it takes a veeeeery long time, and if something goes wrong, its back to ground zero. I am guessing that since gambit is a 32 bit application on my 64 bit machine, I can create big meshes because my computer has sufficient memory, but Gambit can only utilize 4 GB at a time.

I understand that Linux has a 64 bit Gambit application, is this true? Where can I find this?

Additionally, I have access to Ansys 12.1. I also found that there is Ansys Designmodule or Ansys Meshing, but I don't know if my version has those particular applications. I have used ICEM, but that cannot volumetrically mesh STL files.

Does anyone have any ideas?

[PSYMN]

Actually, ICEM CFD is great at meshing from STL files... It has a lot of specialized tools for facet cleanup (so good that some customers use us as a milling preprocessor). It is also patch independent, which means it can walk over the little flaws that faceted geometry often has. It can also easily combine Facets and Nurbs (imported geometry or created in ICEM CFD). It can also generate very large meshes very efficiently...

You can use one of the top down ICEM CFD methods to generate a mesh on the STL as geometry, or you can use a bottom up method (such as Delaunay with TGlib AF) to fill from the STL as a mesh...

I would be happy to help you get going with ICEM CFD.

[EphemeralMemory]

Wow, thank you for your help. My problem is, I work with biomedical applications, so the STL files I have are usually complicated and riddled with problem elements.

I know the basic interface for ICEM CFD, as in, how to upload the STL file geometry and meshes. My problem is, when I load the mesh, I do not know how to volumetrically mesh the facets.

In gambit, you would delete the virtual geometry, and convert all of the points/vertices/faces to real geometry, and then mesh. What is the ICEM CFD equivelant of this?

Also, one more annoying question: can you export .msh files after all is said and done?

Thanks a lot btw.

[PSYMN]

ICEM CFD has lots of tools that I couldn't explain over a short post, but to compare with your GAMBIT process description...

The ICEM CFD process would be to import Geometry => STL... (Or import it as mesh and then "Edit => mesh to facets" to convert it to geometry.)

Do you have a region around this brain? Or are you meshing inside of it? Or both? Create a material point(s) (Geometry Tab = Create Body) inside each area you want meshed (Solid, Fluid, Squishy, or whatever part name you want).

Assuming your model was roughly closed, you would go to the mesh tab to set your sizes on the geometry.

Under "Mesh => Global Params" you can set up things like Max size, etc.

Under "Mesh => Compute Mesh", select the tetra/Hybrid method called "Octree (Robust)" and apply/compute.

Tada...

If it gives you any trouble (probably due to leakage), you may need to do some facet repairs (but then Gambit wouldn't have got very far either). You may also want to do feature extractions with the build topology tool, etc. Have you tried any of the Tetra tutorials? Where are you on the learning curve?

[EphemeralMemory]

Oh, I see.

I tried this before; however, I did not hink it was a correct representation because I couldn't see any interior elements... When I used Gambit, it showed all of the interior elements shaded a different color. Is there a way to view the interior elements?

Additionally, when I import the geometry, it looks as if some connections are made, and not others: the STL input seems very fragmented.

Thanks again for your help

[PSYMN]

Try some tutorials to get a grip on the basics (such as viewing mesh).

In the mean time, you can view a cutplane several ways. One is up in the "view" menu, but usually just right click on the mesh branch of the display tree to display or manage my cutplane.

Once the cutplane is on, you can turn on the volume mesh branch of the tree...

You could also check mesh info to see how many volume elements you got, or check the mesh quality to see where the worst volume elements are, etc.

Best regards,

Simon