[manuc]

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

fluentMeshToFoam myMesh.cas -writeSets
setsToZones -noFlipMap
splitMeshRegions -cellZones -overwrite

This doesnt work as the mesh components correpsonding to both solid and fluid are present in the polymesh folder in all files.

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

fluentMeshToFoam myMesh.cas -writeSets
setsToZones -noFlipMap
splitMeshRegions -cellZones -overwrite

2. Put solid .cas file in folder solid inside constant folder.
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

fluentMeshToFoam myMesh.cas -writeSets
setsToZones -noFlipMap
splitMeshRegions -cellZones -overwrite

This generates separate meshes but results in error saying:

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

[chienfm]

Hi Manu,
You may take a look at below thread:

https://www.cfd-online.com/Forums/op...n-problem.html

Best regards,
Nguyen Chien.

[manuc]

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

[chienfm]

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.

[manuc]

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.

[manuc]

Hai all
WHen I try to run conjugateheatfoam
i get the following error

[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]$

The testcase is attached in the following link
https://drive.google.com/open?id=0B6...Xg1SlNKNWh4bXc

COuld someone suggest what could be going wrong

[manuc]

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

cd constant/solid
fluentMeshToFoam *.cas -writeZones
cp -r constant/polyMesh .
setSet -region solid -batch solid.setSet
setsToZones -region solid -noFlipMap
cd ../../

We copied the new Polymesh folder from the dummy constant folder, just outside
i.e we did
cp -r constant/solid/constant/polyMesh constant/solid/
The dummy folders can be deleted
Run for fluid

fluentMeshToFoam *.cas -writeZones
setSet -batch fluid.setSet
setsToZones -noFlipMap

Modify boundary conditions in the constant/polyMesh/boundary and constant/solid/polyMesh/boundary

with the regioncouple BC and associated lines as in the tutorial.

Seems to work for me now. If any better method please share