CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] ICEM 12.1 - car meshing (

T_Portolon July 23, 2011 16:12

ICEM 12.1 - car meshing
Hi everyone,

I'm facing a little trouble in surface meshing with ICEM 12.1. Using the mesh type "all tri" and mesh method "patch dependent", I have had as result, that the boundaries of the surface are meshed with quad elements, instead of triangular elements. How can I solve this problem?

Thanks in advance


PSYMN July 24, 2011 23:21

You have set a "width" setting on your curves.

This is typically used for FEA to create "washers". They would combine this with a bolt spider to stiffen those regions.

Go back and set the width on the curves to zero... If you are setting the sizes on the parts and want to set a width to the surfaces but not the curves, that can be done (look for the checkbox option on the Params by Parts pop up)...


T_Portolon July 25, 2011 18:30

Curve & surface meshing (and one more question)

Thanks for the help! Actually, I'm following these steps to obtain a surface mesh:
1. mesh the curves (width may vary, depending on the location)
2. mesh the surfaces (applying size in the mesh, different from Gambit)
It usually works, but with the tetra elements on the boundaries.

I didn't mesh the volume, yet. It's because when I try to run the volume meshing, the program goes wrong, creating something around 14 million elements, and gets stuck. What am I doing wrong?

Thanks again


PSYMN July 26, 2011 14:06

paradigm shift
Skip the first step...

Just set sizes on your geometry (curves are required, surfaces are bonus) and go straight to meshing the surfaces with patch conforming...

Alternatively, you could also just skip right to volume meshing with the Octree Tetra... It has many advantages and is probably the easiest way to go.

Try a couple tutorials to help transition you from a Gambit mind set to an ICEM CFD mind set... If you keep thinking with the Gambit paradigm, you will miss most of the ICEM CFD advantages.

If tutorials are too much work, at least take a look at some movies on youtube or the customer portal. Here is one about skipping right to volume mesh...

Have fun with it.


T_Portolon July 26, 2011 19:57

Direct volume meshing

I made the mesh as you said, and it was ok.
Now, I gonna try to use a density around the model, to refine the mesh a little bit.
I used to work with ICEM as I did it with Gambit (meshing edges, faces and volumes, in this order).

Thanks again!


T_Portolon August 18, 2011 16:39

Delaunay for tetras
1 Attachment(s)
Hi Simon,

I made some volume meshes with octree, and it was ok. Now I'm trying to use Delaunay, to reduce the number of cells (around 3-4 million). I tried to use densities around the car body, but the final mesh reached 9 million of cells.

Using Delaunay, the problem is the volume mesh is created around the volume (wind tunnel) that I want to mesh.

Do you know how can I fix this?



PSYMN August 20, 2011 23:54

Was your tunnel surface meshed?

I would suggest starting with your Octree mesh... Then delete the volume mesh, smooth the heck out of the rest with Laplace turned on... Then smooth once more without Laplace, then run delaunay from that.

It will keep your surface mesh, make it nicer and then fill in the volume with delaunay.

Best regards,


T_Portolon August 22, 2011 17:53


The surfaces were meshed before delaunay volume meshing. For first, I selected "mesh internal domains", and meshed the volume. I think I had a problem with the geometry. Then, I saved it in parasolid format, and repaired with SolidWorks resources.

And so, I meshed the volume following your recommendations, and it was right again.



T_Portolon August 29, 2011 20:31

Case and data transfering
Hi Simon

Thanks for helping with ICEM. Do you work with Fluent? I've been using a
8-processor machine to run the simulations. When I try to open those files in my machine (4-processor), it doesn't work.

Thanks in advance


PSYMN September 1, 2011 22:57

I don't know what the problem is, but it doesn't matter that one machine had 8 cpus and the other had 4...

maalan February 7, 2012 05:08

Hi, Simon!! I am facing a 3D hexa mesh of a car with ICEM CFD by using the o-grid. I find it such tool very useful and I am getting very good results. My car model is within a wind tunnel and separated 50 cm from the ground so I am having trouble in meshing the zone under the car.

I find it your help in this forum very useful!!
Thanks in advance!

All times are GMT -4. The time now is 00:20.