[doubtsincfd]

foamMeshToFluent does not write zones.
Is there anyway to convert cellZones from OF to Fluent?

[wyldckat]

Greetings Omkar,

From this post: http://www.cfd-online.com/Forums/ope...tml#post353952 post #12 - I would guess that you have to first convert the zones to sets and only then you can run foamMeshToFluent.

Best regards,
Bruno

[doubtsincfd]

Hi Bruno,

OF is not converting sets or zones to fluent mesh format.
Or maybe I am going wrong somewhere.

I am attaching one of the tutorials. If you run Allrun and see the constant/polymesh folder, you will find a porous zone defined in constant/polymesh/sets folder as well as in in the file constant/polymesh/cellZones

Now if I run foamMeshToFluent and read the mesh in Fluent, the porous zones are not read by fluent.

[wyldckat]

Hi Omkar,

The file didn't get attached. Anyway, I've used the tutorial "compressible/rhoPimpleFoam/ras/angledDuct" as an example.
Indeed the file generated by foamMeshToFluent doesn't seem to do what you want it to do...

In Fluent, are you able to use a field for selecting which cells should be converted to a porous region? If so, then it's possible for you to use setFields to fill the cellSet with any value you want on a dummy field. Then use the OpenFOAM variant 1.6-ext, which has the utility foamDataToFluent, for converting said dummy field into compatible data and then use Fluent to select cells based on a field and change said cells to porous mesh!

Last but not least: in theory, it should be possible to create a modified application of foamDataToFluent or foamMeshToFluent for converting cellSets...

Best regards,
Bruno

[MikeMac]

Hi Bruno and Omkar,

I just came across this forum and I'm trying to do a similar thing for reading the mesh with Fluent and/or EnSight. I like Bruno's idea of creating "dummy" fields to be converted. The only thing is that I'm trying to write a script that makes sHM more user-friendly so that I can convert my co-workers from using Harpoon to sHM. So ideally I'd like there to be very little manual work in Fluent/EnSight in terms of selecting and changing fields.

Are you aware of another way to do this? Or has any development been done to fix this? For instance, in one mesh I have three zones: surf_prism, surf_sphere, and surf_box. I see that when I try to open the mesh in Fluent, I get the following message:

Building...
     mesh
     materials,
     interface,
     domains,
     zones,
	Skipping zone surf_prism (not referenced by grid).
	Skipping zone surf_sphere (not referenced by grid).
	Skipping zone surf_box (not referenced by grid).
	symmetry
	ground
	outlet
	inlet
	interior-1
	fluid-1
Done.

And when I open the .msh file in an editor, I see that all the other zones have grid dimensions, but not my surfaces. I get similar results with EnSight as well.

Any other ideas? Or should I just accept that there isn't a simple way to do this at the moment.

Thanks!!

Mike

[manju819]

Hii Mike,
split the zones using the splitMeshRegions -cellZones -overwrite and convert the mesh using foamToEnsightParts and read the ensight format in fluent.

Regards,
Manjunath

[KaLium]

Originally Posted by manju819

Hii Mike,
split the zones using the splitMeshRegions -cellZones -overwrite and convert the mesh using foamToEnsightParts and read the ensight format in fluent.

Regards,
Manjunath

I had similar approach and it works.

[TheMadHungarian]

I used foamMeshToFluent from openFoam 7 and noticed that the boundary regions from the OF mesh are tagged as "39" in the Fluent mesh file. According to the Fluent mesh file format, these should be "45".



So at the end of the Fluent mesh file you will see this after foamMeshToFluent:


...

(39 (12 wall ground)())
...


so change the "39" to a "45" for each boundary zone:
...

(45 (12 wall ground)())
...


Andy

[rupak504]

Originally Posted by TheMadHungarian

I used foamMeshToFluent from openFoam 7 and noticed that the boundary regions from the OF mesh are tagged as "39" in the Fluent mesh file. According to the Fluent mesh file format, these should be "45".



So at the end of the Fluent mesh file you will see this after foamMeshToFluent:


...

(39 (12 wall ground)())
...


so change the "39" to a "45" for each boundary zone:
...

(45 (12 wall ground)())
...


Andy

I did the same thing....i.e. first I converted OpenFOAM mesh to fluent mesh using fluentMeshtoFoam. It was 39, which I changed to 45. Then I opened that in Fluent, it gave critical error. can you please help?

regards

[TheMadHungarian]

Sorry, I can't help, I do not use Fluent. I just used the Fluent format to convert the mesh from OpenFOAM to the .VOG format used by Loci/CHEM.