|
[Sponsors] |
February 1, 2017, 10:40 |
Cell Zones in fluent
|
#1 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Dear all,
my name is Tobias Holzmann and I am normally using OpenFOAM. However, a colleague has a meshing problem that I meshed with snappyHexMesh (FOAM mesher). Sofar so good, However, this mesh contains 4 regions. For me it is not possible to transform the information of the cellZones that I create during the meshing stage into fluent. It is lost after conversion to a fluent mesh. Now the question. Is it possible to define a cellZone in the actual mesh based on e.g. STL / STEP data inside Fluent? I think it should be possible, or not? Any suggestion of your expertise is welcomed.
__________________
Keep foaming, Tobias Holzmann |
|
February 1, 2017, 11:03 |
|
#2 | |
Senior Member
Kushal Puri
Join Date: Nov 2013
Posts: 182
Rep Power: 12 |
Quote:
What you can try is open the mesh in ICEM and export it again. |
||
February 1, 2017, 12:00 |
|
#3 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Hmm okay but do you mean to create the cellZonrs in ICEM? Because in the msh file there is no information about cellZones after converting from foam mesh to fluent mesh.
Sent from my HTC One mini using CFD Online Forum mobile app
__________________
Keep foaming, Tobias Holzmann |
|
February 1, 2017, 12:21 |
|
#4 | |
Senior Member
Kushal Puri
Join Date: Nov 2013
Posts: 182
Rep Power: 12 |
Quote:
|
||
February 1, 2017, 14:03 |
|
#5 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
The conversion from foam mesh to fluent mesh does not contain the information of the cell zones ... Thats why I ask. So I have to create the cellZones somehow different.
__________________
Keep foaming, Tobias Holzmann |
|
February 2, 2017, 20:47 |
|
#6 |
New Member
XX
Join Date: Apr 2013
Posts: 6
Rep Power: 13 |
you can mesh the model using fluent mesh mode
|
|
February 3, 2017, 06:13 |
|
#7 |
Member
carno
Join Date: Mar 2009
Posts: 70
Rep Power: 17 |
Probably you need to revisit your foamMeshToFluent code. I know you are quite expert in OF, but did you give -writeZones after your converter command? If there is no cellzones in converted mesh, you can not create in Fluent. In ICEM you can create cellzones if it is simple to select.
|
|
February 3, 2017, 07:29 |
|
#8 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Dear gjitmawa, your suggestion is nice but you may read my question. The reason why I was asking was due to the fact that:
@Carno. Thanks for your kind words and that you think that I have a big expertize in FOAM. However, I already checked the sources of foamMeshToFluent and unfortunately there is nothing included that treats the cellZones. Well, I was asking my colleague to make some simple fluent mesh with cellZones in order to check out the syntax of the *.msh file in order to enable implement the zone transformation. This was not possible because he always got binary files which I could not check out. Of course I gave him some suggestions from other people in »How to export ASCII files« but I did not get an ASCII file. Well, the problem is solved now because he went back to the fluent mesher. So finally, there is no need for me to go deeper into the topic. Thanks for all replies.
__________________
Keep foaming, Tobias Holzmann |
|
February 4, 2017, 01:24 |
|
#9 |
Member
carno
Join Date: Mar 2009
Posts: 70
Rep Power: 17 |
Another thing I thought is, just make regions instead of zones.
Code:
splitMeshRegions -cellZones Anyways that problem is solved.. |
|
February 8, 2017, 09:27 |
|
#10 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Dear Carno,
thanks for the hint. I did not check it because what we get after your command is like single-meshes and then the question would be, how can I convert it? For sure, I can convert each single region into a msh mesh but my colleague said that he need only "one" mesh file with all information. I even do not know if that is correct because I also expect FLUENT to be able to load 2 - 3 different "domains" and couple them. At last, he was also complaining that I have to make the "shadow" walls in a way that FLUENT recognize it itself. Don't know because I never used FLUENT. Just can trust his sentences (even if I do not want because there should be a way) :P
__________________
Keep foaming, Tobias Holzmann |
|
April 21, 2017, 05:31 |
|
#11 |
Senior Member
Kal-El
Join Date: Apr 2017
Location: Finland
Posts: 150
Rep Power: 9 |
||
February 5, 2018, 10:16 |
foamToEnsightParts
|
#12 |
Member
Arvind Jay
Join Date: Sep 2012
Posts: 96
Rep Power: 14 |
Try foamToEnsightParts: Translates OpenFOAM data to Ensight format. An Ensight part is created for each cellZone and patch.
Ensight files can be imported in fluent with cellzones. Cheers: -Jay |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Connecting three fluid zones in Ansys Fluent 12 | tobiasz | FLUENT | 0 | April 29, 2016 11:43 |
How to create matching mesh zones so that periodic boundary can be created in Fluent | cgoodale1 | STAR-CCM+ | 3 | February 29, 2016 12:34 |
Journal file error | magicalmarshmallow | FLUENT | 3 | April 4, 2014 12:25 |
Cell centroid and cell volume in general, and in Fluent | zmester | Main CFD Forum | 3 | October 17, 2009 11:05 |
Fluent on Cell Processor | DC | FLUENT | 2 | March 14, 2008 12:01 |