|
[Sponsors] |
OF extend 3.2: Mesh from fluent for conjugateHeatFoam |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 27, 2017, 07:44 |
OF extend 3.2: Mesh from fluent for conjugateHeatFoam
|
#1 |
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 |
Hello all,
I would like to export mesh from ansys wb as a fluent case file (.cas). I want them to be used for conjugateHeatFoam. As I understand the solver needs two mesh ; One for the solid and another for the fluid. What I tried- Trial 1 I tried to export the mesh of the whole geometry and used Code:
fluentMeshToFoam myMesh.cas -writeSets setsToZones -noFlipMap splitMeshRegions -cellZones -overwrite Trail 2- Export solid and fluid mesh separate I exported both cas files separate and followed: 1. Put fluid case file in the main folder. carried out Code:
fluentMeshToFoam myMesh.cas -writeSets setsToZones -noFlipMap splitMeshRegions -cellZones -overwrite It popped up with an error saying control dict is missing inside the solid folder. To give a try I created system folder inside it .(constant/solid/system) and carried out Code:
fluentMeshToFoam myMesh.cas -writeSets setsToZones -noFlipMap splitMeshRegions -cellZones -overwrite This generates separate meshes but results in error saying: Code:
reate time --> FOAM Warning : From function IOstream::compressionEnum(const word&) in file db/IOstreams/IOstreams/IOstream.C at line 74 bad compression specifier 'off', using 'uncompressed' Create mesh for time = 0 --> FOAM FATAL ERROR: Problem with patch-to-zone addressing for patch of_plate_to_air: some patch faces not found in interpolation zone From function void regionCouplePolyPatch::calcZoneAddressing() const in file meshes/polyMesh/polyPatches/constraint/regionCouple/regionCouplePolyPatch.C at line 120. Could someone suggest the right way to convert fluent mesh compatible for conjugatefoam from foam extend 3.2. Please find the case folder attached in : https://drive.google.com/open?id=0B6...FkxYkQ3N0UxMm8
__________________
Regards Manu |
|
February 1, 2017, 03:55 |
|
#2 |
New Member
Ngo Bao Chung
Join Date: Sep 2012
Posts: 14
Rep Power: 13 |
Hi Manu,
You may take a look at below thread: Best regards, Nguyen Chien. |
|
February 1, 2017, 04:00 |
|
#3 |
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 |
Dear Chung
I have used the same method as in the https://www.cfd-online.com/Forums/op...tml#post424703 This works fine for opefnoam solvers. But when using conjugateheatfoam from FOAMEXTEND, the mesh needs to be separat for both solid and fluid. both of them goes in different directories. Fluid mesh in the main Polymesh folder. The solid mesh goes ina folder corresponding to solid/polymesh. Thus it seems to be different from OF based method
__________________
Regards Manu |
|
February 1, 2017, 04:34 |
|
#4 |
New Member
Ngo Bao Chung
Join Date: Sep 2012
Posts: 14
Rep Power: 13 |
Hi Manu,
I just checked your case. I revised two lines and the mesh ran well. 1. In system/controlDict: line 46 : off --> uncompressed 2. In 0/materials: line 28: plate_to_air --> of_air_to_plate Hope this help! Best regards, Chien Nguyen. |
|
February 1, 2017, 04:39 |
|
#5 |
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 |
Thanks Chung, I will try to re-run my case with your suggestions.
Could you tell me whether you used the same steps I mentioned in this post. i.e you created an extra constant folder inside solid folder to convert fluentmeshtofoam for the solid region. Also I never merged the meshes.
__________________
Regards Manu |
|
February 1, 2017, 09:06 |
|
#6 |
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 |
Hai all
WHen I try to run conjugateheatfoam i get the following error Code:
[manuchakkingal@hpc11:rt_1_vf]$ conjugateHeatFoam /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | foam-extend: Open Source CFD | | \\ / O peration | Version: 3.2 | | \\ / A nd | Web: http://www.foam-extend.org | | \\/ M anipulation | For copyright notice see file Copyright | \*---------------------------------------------------------------------------*/ Build : 3.2 Exec : conjugateHeatFoam Date : Feb 01 2017 Time : 15:01:01 Host : hpc11 PID : 5033 CtrlDict : "/home/manuchakkingal/OpenFOAM/manuchakkingal-3.2-ext/run/rt_1_vf/system/controlDict" Case : /home/manuchakkingal/OpenFOAM/manuchakkingal-3.2-ext/run/rt_1_vf nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time --> FOAM Warning : From function IOstream::compressionEnum(const word&) in file db/IOstreams/IOstreams/IOstream.C at line 74 bad compression specifier 'off', using 'uncompressed' Create mesh for time = 0 --> FOAM FATAL ERROR: Region couple patch of_plate_to_air and its shadow of_air_to_plate on region region0. Clash on master-slave definition. This is not allowed. Please check your mesh definition. From function label regionCouplePolyPatch::shadowIndex() const in file meshes/polyMesh/polyPatches/constraint/regionCouple/regionCouplePolyPatch.C at line 763. FOAM aborting Aborted (core dumped) [manuchakkingal@hpc11:rt_1_vf]$ https://drive.google.com/open?id=0B6...Xg1SlNKNWh4bXc COuld someone suggest what could be going wrong
__________________
Regards Manu |
|
May 10, 2018, 07:29 |
Solution
|
#7 |
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 |
Current Folder structure:
case --> 0 , constant system 1. Place fluid mesh in the case folder. 2. Place solid mesh inside constant/solid 3. Create a dummy constant and system folder inside the case/constant/solid folder Run for solid Code:
cd constant/solid fluentMeshToFoam *.cas -writeZones cp -r constant/polyMesh . setSet -region solid -batch solid.setSet setsToZones -region solid -noFlipMap cd ../../ i.e we did cp -r constant/solid/constant/polyMesh constant/solid/ The dummy folders can be deleted Run for fluid Code:
fluentMeshToFoam *.cas -writeZones setSet -batch fluid.setSet setsToZones -noFlipMap with the regioncouple BC and associated lines as in the tutorial. Seems to work for me now. If any better method please share
__________________
Regards Manu |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[ICEM] Error reading 2D hybrid ICEM mesh into Fluent | Kloz | ANSYS Meshing & Geometry | 1 | June 6, 2016 13:45 |
Lift and Drag pattern change wit FLUENT 16 and 13 PISO for same mesh n solver setting | arunraj | FLUENT | 0 | June 2, 2016 22:58 |
FLUENT - ICEM / Segmentation Violation Error (Hybrid Mesh) | Joachim | ANSYS | 3 | April 24, 2016 16:52 |
[ICEM] Fluent reading wrong mesh type | Tommorrice | ANSYS Meshing & Geometry | 1 | March 15, 2016 17:32 |
[mesh manipulation] Importing Multiple Meshes | thomasnwalshiii | OpenFOAM Meshing & Mesh Conversion | 18 | December 19, 2015 18:57 |