CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)
-   -   [Commercial meshers] Error in polyhedral-mesh (Fluent Meshing) conversion to OpenFOAM. (https://www.cfd-online.com/Forums/openfoam-meshing/204600-error-polyhedral-mesh-fluent-meshing-conversion-openfoam.html)

ACLT July 27, 2018 07:33
Error in polyhedral-mesh (Fluent Meshing) conversion to OpenFOAM.
 
4 Attachment(s)
Hi everyone,

I am using the ACT extension* to convert ANSYS Meshing meshes to polyhedral meshes and everything seem to be ok in Fluent. Then, I tried to convert the mesh to OpenFOAM and after many errors the conversion was successful. However, when I visualized the mesh I realized that the polyhedrons were not well-converted. The polyhedrons seem to be divided and I don't know why can be the reason, or if I am missing some extra command needed.

Thanks in advance!


:)

*When I used only FluentMeshing to generate the mesh and not ACT, the same occurs.

akidess July 27, 2018 08:34
https://www.cfd-online.com/Forums/op...-paraview.html

ACLT August 16, 2018 02:45
Thank you very much!

kagen816 October 27, 2018 13:10
Quote:
Originally Posted by ACLT (Post 700679)
Hi everyone,

I am using the ACT extension* to convert ANSYS Meshing meshes to polyhedral meshes and everything seem to be ok in Fluent. Then, I tried to convert the mesh to OpenFOAM and after many errors the conversion was successful. However, when I visualized the mesh I realized that the polyhedrons were not well-converted. The polyhedrons seem to be divided and I don't know why can be the reason, or if I am missing some extra command needed.

Thanks in advance!


:)

*When I used only FluentMeshing to generate the mesh and not ACT, the same occurs.
Hi ACLT,

Could you tell me how you import the polyhedral mesh from fluent into openFoam? I am now straggling with it. thank you very much.

ACLT October 29, 2018 02:50
Hi kagen816!


Once you have the mesh in Fluent, you need to save the .cas with the "binary files" option deactivate. Then, in OpenFOAM use the command "fluent3DmeshToFoam your_name_case.cas" and now an error appears always to me. It says something like "Do not understand characters ; ", so you need to open the file with vim or another editor, then find the ";" character and delete it (In my meshes it appears always two times). Finally, another time with the command fluent3DmeshToFoam, it should work.


Hope it works for you! If you need more information, don't hesitate to tell me :)

kagen816 October 29, 2018 12:36
Quote:
Originally Posted by ACLT (Post 713324)
Hi kagen816!


Once you have the mesh in Fluent, you need to save the .cas with the "binary files" option deactivate. Then, in OpenFOAM use the command "fluent3DmeshToFoam your_name_case.cas" and now an error appears always to me. It says something like "Do not understand characters ; ", so you need to open the file with vim or another editor, then find the ";" character and delete it (In my meshes it appears always two times). Finally, another time with the command fluent3DmeshToFoam, it should work.


Hope it works for you! If you need more information, don't hesitate to tell me :)
Hi ACLT，

It works very well! Thank you very much!

Best Regards.

rezaeimahdi June 22, 2022 03:36
Quote:
Originally Posted by ACLT (Post 713310)
Hi kagen816!


Once you have the mesh in Fluent, you need to save the .cas with the "binary files" option deactivate. Then, in OpenFOAM use the command "fluent3DmeshToFoam your_name_case.cas" and now an error appears always to me. It says something like "Do not understand characters ; ", so you need to open the file with vim or another editor, then find the ";" character and delete it (In my meshes it appears always two times). Finally, another time with the command fluent3DmeshToFoam, it should work.


Hope it works for you! If you need more information, don't hesitate to tell me :)
Hi,

I just posted it here for the guys working with Ansys 2021 R2 or newer versions:

In these versions, you don't have that binary option in saving mesh files as suggested by ACLT

Also, in "Behavioral Change Messages" it is mentioned that: "The default mesh file format is changed to the Common Fluids Format (CFF) with an extension of *msh.h5. "

To be able to write a file.cas in ASCII format in fluent:

First, you need to change as follow:

File-->Preferences-->Default Format for I/O--->Legacy


Then in fluent console, type:

Code:
/file> binary-legacy-files
Write binary files? [yes] no
/file> write-case
The rest of the process in OpenFOAM is same as ACLT suggested.

Also please note that if you don't need the polyhedral mesh generated in fluent and just want to export a mesh from Ansys Mesher, then:

Ansys mesher --> file --> options --> meshing --> export --> format of input file --> ASCII

Enjoy!


All times are GMT -4. The time now is 00:33.