CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... (
-   -   Conversion Fluent cas and dat file to OpenFoam (

matteo_gautero January 24, 2008 10:00

Hi to all, sorry for my engli
Hi to all,
sorry for my english; I am a newbie of OpenFoam. I have obtained several results for my problem with Fluent and now I want to work with OpenFoam using intermediate results obtained in Fluent so I want to convert .cas and .dat files to Openfoam files. I tried to use fluentMeshToFoam: it works very well with .msh file but it doesn't work with .cas and .dat files. Is it possible? Do you know some utility which do that?

I want to use OpenFoam because I have the possibility to exploit a linux based pc with more RAM and so I can refine the mesh and I hope to obtain better results. So,is the tool to refine the mesh present in OpenFoam good? Is there an open source or freeware program for linux that do a refine of the mesh with a GUI?

Thaks in advance,
Matteo Gautero.

francesco_b January 24, 2008 11:00

Hi Matteo, I've used fluent
Hi Matteo,

I've used fluentMeshToFoam with some .cas files and everything was ok. Which kind of errors do you have?



florian_krause January 24, 2008 11:28

Hi Matteo, when I use fluen
Hi Matteo,

when I use fluentMeshToFoam to convert a fluent .cas file (only mesh information) I have no problems.

But as I understand you correct, you want to convert your results (.cas and .dat files), than refine the mesh and run the job with OF?

This conversion would be a result and mesh conversion but fluentMeshToFoam only works for mesh conversion.

Somebody might correct me if I am worng regarding the fluentMeshToFoam converter


fra76 January 24, 2008 11:30

Hi Matteo, you must save case
Hi Matteo,
you must save case as ascii to let the compiler work. And if the mesh is 3D, my suggestion is to use fluent3DMeshToFoam.
About data file, I'm not aware about a converter... You can do the other way round, with foamDataToFluent (and foamMeshToFluent for the mesh).



matteo_gautero January 24, 2008 11:46

Hi to all, thanks for your an
Hi to all,
thanks for your answers. Yes Florian, I want to convert my results and than refine the mesh and run the case with OF. When I try to do this, the message error is:

Embedded blocks in comment or unknown:
Found end of section in unknown

for several lines and then OF print this message:

Number of cells: 736991
number of faces: 1524374
Number of points: 148787
0Dimension of grid: 12
(Dimension of grid: 2
Dimension of grid: 1
bDimension of grid: 3
edfDimension of grid: 1
Dimension of grid: 2
0Dimension of grid: 13
(Dimension of grid: 3
Dimension of grid: 1
Dimension of grid: 622
Dimension of grid: 24
Dimension of grid: 3

after this, OF stops. I think it's not possible to convert a .cas file after some iterations. So I will redo the itereations with the refined grid obtained by the first mesh used in Fluent. Anyway, I will try to convert the first .cas file containing the boundary conditions imposed in Fluent without iterations.

Matteo Gautero.

fra76 January 24, 2008 11:59

No, that's not true. There is
No, that's not true.
There is no conceptual difference between a Fluent cas file at "0" iterations and another one saved after a while.
With respect to the .msh file, the .cas file contains some extra fields that the converter usually skips.
As I wrote before, you MUST save your .cas file in ASCII, otherwise the converter doesn't work, and sometimes remains blocked without giving any outoput...


matteo_gautero January 25, 2008 03:49

Hi Francesco, you're right. I
Hi Francesco,
you're right. I tried to do what you said and it worked very well. The first messages were errors, i.e.

Embedded blocks in comment or unknown (
Found end of section in unknown )
Found end of section in unknown )

but then OF read the grid and I visualized it, it was ok.

Thanks to all for these explanations,

mrangitschdowcom April 2, 2008 10:36

I'm having problems processing
I'm having problems processing a .cas file that I had run fluent on and then did a grid refinement to tighten up the grid in the boundary layer (it resulted in hanging grids). fluent3dmeshtoFoam won't process it at all -- gives me an illegal block type 37 -- that's the label on a block of text in the case file which describes the fluent models used... Any ideas?

dmoroian April 2, 2008 10:59

As far as I know, grid refinem
As far as I know, grid refinement in fluent means hanging nodes, which fluent3DMeshToFoam doesn't know how to interpret.


fra76 April 3, 2008 02:32

fluent3DMeshToFoam is able to
fluent3DMeshToFoam is able to handle hanging nodes (fluentMeshToFoam isn't).
If it finds an unknown block, try to open the .cas file with a text editor end remove the corresponding lines. In a fluent mesh file, each block is enclosed by ( ).

Good luck!

All times are GMT -4. The time now is 09:04.