CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[Commercial meshers] foamMeshToFluent does not write zones

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes
  • 3 Post By manju819

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 12, 2012, 15:46
Default foamMeshToFluent does not write zones
  #1
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 13
doubtsincfd is on a distinguished road
foamMeshToFluent does not write zones.
Is there anyway to convert cellZones from OF to Fluent?
doubtsincfd is offline   Reply With Quote

Old   October 13, 2012, 04:16
Default
  #2
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,963
Blog Entries: 45
Rep Power: 124
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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
__________________
wyldckat is offline   Reply With Quote

Old   October 18, 2012, 13:30
Default
  #3
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 13
doubtsincfd is on a distinguished road
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.
doubtsincfd is offline   Reply With Quote

Old   October 18, 2012, 15:31
Default
  #4
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,963
Blog Entries: 45
Rep Power: 124
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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
__________________
wyldckat is offline   Reply With Quote

Old   May 15, 2013, 09:49
Default
  #5
New Member
 
Michael Mackenzie
Join Date: Apr 2013
Posts: 3
Rep Power: 10
MikeMac is on a distinguished road
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:

Code:
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
MikeMac is offline   Reply With Quote

Old   December 1, 2014, 07:42
Default foamMeshToFluent does not write zones
  #6
Member
 
Manjunath Reddy
Join Date: Jun 2013
Posts: 47
Rep Power: 10
manju819 is on a distinguished road
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
arvindpj, KaLium and Shadab like this.
manju819 is offline   Reply With Quote

Old   April 21, 2017, 05:36
Default
  #7
Senior Member
 
KaLium's Avatar
 
Kal-El
Join Date: Apr 2017
Location: Finland
Posts: 150
Rep Power: 6
KaLium is on a distinguished road
Quote:
Originally Posted by manju819 View Post
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.
KaLium is offline   Reply With Quote

Old   October 24, 2019, 11:30
Default
  #8
New Member
 
Andy S.
Join Date: Jun 2018
Posts: 13
Rep Power: 5
TheMadHungarian is on a distinguished road
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
TheMadHungarian is offline   Reply With Quote

Old   October 29, 2019, 09:48
Default
  #9
Member
 
rupak504's Avatar
 
Lolita
Join Date: Aug 2016
Posts: 91
Rep Power: 6
rupak504 is on a distinguished road
Quote:
Originally Posted by TheMadHungarian View Post
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
rupak504 is offline   Reply With Quote

Old   October 29, 2019, 09:57
Default
  #10
New Member
 
Andy S.
Join Date: Jun 2018
Posts: 13
Rep Power: 5
TheMadHungarian is on a distinguished road
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.
TheMadHungarian is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[snappyHexMesh] Debug option in snappy / Write volScalarField with cellLevel for postprocessing Ruli OpenFOAM Meshing & Mesh Conversion 1 March 30, 2014 08:57
Skipping Zones 1337Hal FLUENT 0 April 6, 2009 21:19
Phase locked average in run time panara OpenFOAM 2 February 20, 2008 14:37
about seperating zones Bono FLUENT 1 October 8, 2005 06:08
Patch-Different values to different zones Pradeep FLUENT 0 April 26, 2005 08:50


All times are GMT -4. The time now is 19:11.