CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   chtMultiRegionFoam - different mesh on the 2 sides of a coupled boundary (http://www.cfd-online.com/Forums/openfoam/107363-chtmultiregionfoam-different-mesh-2-sides-coupled-boundary.html)

turbulencious September 25, 2012 09:37

chtMultiRegionFoam - different mesh on the 2 sides of a coupled boundary
 
solver: chtMultiRegionFoam
version: 2.1-1
BC: compressible::turbulentTemperatureCoupledBaffleMix ed

dear FOAMers,

I hope everything is fine on your side.

I am using chtMultiRegionFoam and expectedly, I would like to have a more densed mesh in the fluid and a less densed mesh in the solid.

Is it possible? and if yes, have anybody already achieved it and can give me some guidelines?

thanks a lot

thomasnwalshiii September 27, 2012 09:41

coinciding mesh
 
I believe that for the default cht... solver you need coinciding surface meshes in order to transfer the energy between the different regions. You'd have to edit the boundary conditions to incorporate a ggi interface. I remember one of the presentation from the 2011 workshop at Penn State was on a multi-physics solver (conjugatedFsiFoam maybe) and the presenter went through the steps needed to implement this.

Here is the link to the powerpoint slides, http://www.personal.psu.edu/dab143/O...ven_slides.pdf. They only briefly mention how to implement it towards the end. Has anyone in this forum accomplish such a feat?

turbulencious September 28, 2012 04:50

thanks Thomas

dhruv October 12, 2012 07:46

Any Solutions??
 
Hi,

Were you able to solve this problem? Did you implement AMI/GGI on the patches? I have the same kind of problem, but I am not able to figure out how to use AMI in chtMultiRegionFoam.

Any help is greatly appreciated.

Thanks,
Dhruv.

Quote:

Originally Posted by turbulencious (Post 383537)
solver: chtMultiRegionFoam
version: 2.1-1
BC: compressible::turbulentTemperatureCoupledBaffleMix ed

dear FOAMers,

I hope everything is fine on your side.

I am using chtMultiRegionFoam and expectedly, I would like to have a more densed mesh in the fluid and a less densed mesh in the solid.

Is it possible? and if yes, have anybody already achieved it and can give me some guidelines?

thanks a lot


anothr_acc July 18, 2014 15:43

Hey everyone! I now also need this functionality. Does anybody know if CHT and AMI can be used at the same time, on the same boundary in OF2.3.0 ?

Please say yes!

Best regards,

Mark.

anothr_acc July 24, 2014 05:58

Quote:

Originally Posted by anothr_acc (Post 502200)
Hey everyone! I now also need this functionality. Does anybody know if CHT and AMI can be used at the same time, on the same boundary in OF2.3.0 ?

Please say yes!

Best regards,

Mark.

Answered my own question. In short, yes! Try it:

in constant/copper/polyMesh/blockMeshDict:

Code:

boundary {
  copper_to_iron { sampleRegion iron; samplePatch iron_to_copper;
    type mappedWall;

    sampleMode nearestPatchFaceAMI;
    //sampleMode nearestPatchFace;

    offsetMode uniform; offset (0 0 0);
    faces ( (2 6 5 1) ) ; } // anti-clock looking in.
    }


in constant/iron/polyMesh/blockMeshDict:

Code:

boundary {
  iron_to_copper { sampleRegion copper; samplePatch copper_to_iron;
    type mappedWall;

    sampleMode nearestPatchFaceAMI;
    //sampleMode nearestPatchFace;

    offsetMode uniform; offset (0 0 0);
    faces ( ( 3 0 4 7 ) ) ; }
    }

And as long as there are no cells on the interface plane with no coupling to a boundary condition, this runs and provides better matching for power into the system and power out of the system for slightly different sized of differently meshed regions than the nearestPatchFace sampleMode.

Best regards,

Mark.


All times are GMT -4. The time now is 20:29.