[esma]

Hi All,

I have been struggling to import .msh files from fluent to OpenFOAM.
please note this is different from the mesh generated in the ANSYS Workbench mesh module.

The reason is Workbench mesh doesn't have Polyhedral. So I produce the mesh via Fluent and write it from fluent mesh in msh file. When imported in OpenFOAM and applying the fluent3DMeshToFoam command, I get the following message. Has anyone else faced the same problem?

--> FOAM FATAL ERROR: (openfoam-2206)
Do not understand characters: �
on line 1

From virtual int yyFlexLexer::yylex()
in file fluent3DMeshToFoam.L at line 765.

FOAM exiting

I copy a simple mesh file attached if you could check will be appreciated to see if you get the same message.

Thanks in advance

[AtoHM]

Had a similar problem once, does dos2unix on the .msh file help?
Also make sure to not zip the meshing file when exporting from Fluent.

[esma]

Much appreciated for the tip, you are my savior. Yes it appears to be working now.

procedures for the future

- once you generated your mesh in WB => open fluent file and read the mesh and convert to Polyhedral mesh within fluent => save a case file *.cas

- now launch Fluent from windows (not in WB), and select its Meshing module (not the solution)
- file-->write -->mesh ... Un-tick the "write binary file" box to ensure your file will be in ASCII format. and per AtoHM guides above, don't select the type as compressed file. in the version I have it's called CFF Mesh Files (*.msh.h5).

- import the {name}.msh file into OpenFOAM
- type command dos2unix {name}.msh
(in case you don't have that command run sudo apt install dos2unix)

now your mesh is ready for fluent3DMeshToFoam {name}.msh

[saeed jamshidi]

Hi,
I'm going to import fluent mesh to openfoam like yours.
I'm following your steps, but I have come up with the below error!
whoud you please tell me how can I fix it?
Thanks.

myfoam@DESKTOP-TK3D7CI:~$ cd $FOAM_RUN/tutorials/incompressible/pimpleFoam/laminar/cylinder2D/
myfoam@DESKTOP-TK3D7CI:~/OpenFOAM/myfoam-v2112/run/tutorials/incompressible/pimpleFoam/laminar/cylinder2D$ ls
0.orig  clean  constant  ff.msh.h5  foam.foam  run  system
myfoam@DESKTOP-TK3D7CI:~/OpenFOAM/myfoam-v2112/run/tutorials/incompressible/pimpleFoam/laminar/cylinder2D$ dos2unix ff.msh.h5
dos2unix: Binary symbol 0x1A found at line 2
dos2unix: Skipping binary file ff.msh.h5
myfoam@DESKTOP-TK3D7CI:~/OpenFOAM/myfoam-v2112/run/tutorials/incompressible/pimpleFoam/laminar/cylinder2D$ fluent3DMeshToFoam ff.msh
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2112                                  |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112
Arch   : "LSB;label=32;scalar=64"
Exec   : fluent3DMeshToFoam ff.msh
Date   : Oct 18 2023
Time   : 19:49:32
Host   : DESKTOP-TK3D7CI
PID    : 1671
I/O    : uncollated
Case   : /home/myfoam/OpenFOAM/myfoam-v2112/run/tutorials/incompressible/pimpleFoam/laminar/cylinder2D
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

--> FOAM Warning :
    From void* Foam::dlLibraryTable::openLibrary(const Foam::fileName&, bool)
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 188
    Could not load "libadaptiveFvMesh.so"
libadaptiveFvMesh.so: cannot open shared object file: No such file or directory


--> FOAM FATAL ERROR: (openfoam-2112 patch=220610)
: file "ff.msh" not found

    From int main(int, char**)
    in file fluent3DMeshToFoam.L at line 844.

FOAM exiting

myfoam@DESKTOP-TK3D7CI:~/OpenFOAM/myfoam-v2112/run/tutorials/incompressible/pimpleFoam/laminar/cylinder2D$

[LuckyTran]

OpenFOAM can't find a common library. You have an installation error. Check all your environmental variables.

[saeed jamshidi]

Dear LuckyTran, thanks for reply.
Do you mean there is a problem with installation of dos2unix or other?
Because I can run through current library with blockmesh!

[LuckyTran]

Well it is true that you do have an openfoam installation error but it may be unrelated. You may run into more errors one day depending on which tools you use.

You have a binary .msh file and it needs to be ascii to work.

[saeed jamshidi]

The key point is in preference/Default format for I/O must be Legacy, and when we want to export mesh we should follow as below:

Mesh file: mesh.msh

files of type: *.msh.h5

Then copy mesh.msh into your openfoam library and execute fluent3DMeshToFoam mesh.msh.

you will come up with the error:

--> FOAM FATAL ERROR: (openfoam-2112 patch=220610)
Do not understand characters: [
    on line 431473

    From virtual int yyFlexLexer::yylex()
    in file fluent3DMeshToFoam.L at line 764.

FOAM exiting

open mesh file with edditor and find "[" and delete it. If you execute fluent3DMeshToFoam mesh.msh again it will work properly.

[rockerboy]

It seems to me as if the surface mesh is also imported, which is visible in Paraview. How can I fix this? It overlaps with the volume mesh.

[haribabupv354]

did u find how to hide the surface mesh view in the paraview?
?

[nguyenhung97]

For those who may concern,

I think the problem is you are using very latest version of Ansys Fluent. You can solve the problem as follows:

Try meshing in latest version (etc., Ansys fluent 2024) -> export .msh file in legacy format in ascii mode (.msh.gz) -> use Ansys fluent 2017 to import the .msh file -> export .cas using 2017 version. Now you can import to OpenFOAM using fluent3DToFoam .cas file.