[jnagy]

Comments and questions are welcomed on the article Salehi and Nilsson, OpenFOAM for Francis Turbine transients, OpenFOAM Journal, November 2021, https://doi.org/10.51560/ofj.v1.26.

[manupanand]

Originally Posted by jnagy

Comments and questions are welcomed on the article Salehi and Nilsson, OpenFOAM for Francis Turbine transients, OpenFOAM Journal, November 2021, https://doi.org/10.51560/ofj.v1.26.

Hi, thank you for your contribution. I would like to know how do you convert ICEM mesh and Turbogrid mesh to Open FOAM format

[hani]

Originally Posted by manupanand

Hi, thank you for your contribution. I would like to know how do you convert ICEM mesh and Turbogrid mesh to Open FOAM format

A common way to do that is to write out in Fluent *.msh format and then use fluentMeshToFoam or fluent3dMeshToFoam to convert it to OpenFOAM format.

[salehi144]

Originally Posted by manupanand

Hi, thank you for your contribution. I would like to know how do you convert ICEM mesh and Turbogrid mesh to Open FOAM format

As Håkan explained, we usually export an ICEM case to Fluent's *.msh format and then convert them into OpenFOAM format through fluent3DMeshToFoam. In the case of TurboGrid, the mesh is first sent to ICEM and then exported to Fluent format.

Just make sure to write an ASCII file *.msh file when exporting with ICEM as OpenFOAM's fluent3DMeshToFoam cannot handle binary files.

Saeed

[Lor_enz]

I hope you can give me some hints on that.


As you mentioned, i would like to use a turbogrid mesh for openfoam. As cgnstofoam is not very updated, i wanted to use your workaround with ICEM.
However, when loading the mesh (unstructured cgns) into ICEM i get the error Error: No grid connectivity for zone.


After that error, the mesh loads "without" a problem, and let me export as well without an error. However fluent3dtofoam fails as well as loading the .msh in fluent.

There must be some error in the conversion process. I am using Turbogrid (R2022R2) with ICEM (R2020R2).



greetings Lorenz

[salehi144]

Hi Lorenz,

I usually do not export from Turbogrid and then import to ICEM. I use Workbench and in that case, one can just simply "connect" the two Turbogrid and ICEM modules. Then, ICEM will be able to read the Turbogrid mesh properly. Hopefully, this was the answer you were looking for. Otherwise, let me know.

Saeed

[Lor_enz]

Hello Saeed,

thanks for you quick reply. Unfortunatly the problem does not resolve by dragging directly in workbench. The error contuines to be the same: No grid connectivity information for zone 1

I checked if it is some error in my geometry that leads to turbogrid failure as I have developed a new CAD program for turbomachinery, that is also capable of exporting to turbogrid. But also using the Ansys Bladedesigner did not resolve it.

Strangly i have observed that i cannot import in standard Fluent the CGNS file either. However fluent let me process the CGNS mesh, when importing it during the activated turbomachinery workflow that is provided in fluent.
Neither do i have an issue when using CFX.

Problem, i require the mesh for OpenFoam, so i am bound to get somehow the turbogrid to .msh, in order to export it.

I am using Ansys 2022R2.



Merry Christmas,

Lorenz

[Lor_enz]

As direct implementation did not work for me (at least in R2022), however this worked more me:

1. Create Turbgrid mesh
   • export as .cgns
2. Load into fluent using the turbomachine workflow (important)
   • Important change IO-filetype to Legacy
   • Write file as .cas
3. Open .cas file in ICEM (does not have to be in wb)
4. Write mesh now as .msh
5. Use fluent3DMeshToFoam *.msh

Complicated workaround, but at least a way,

@saeeh, what version are you using?


greetings Lorenz

[salehi144]

I'm glad that it worked for you in the end. It has been a while since I used TurboGrid but I think I have used different versions (R2022 also) and they all worked the way I explained (directly from Turbogrid to ICEM and then export to *.msh).