[onlyacan]

Hallo everyone,

I have developed a melting/solidification solver based on buoyantBoussinesqPimpleFoam. It was applied to melt of a cylinderical geometry. Now I have to calculate the temperature of the container (solid) with the melt. So I studied the chtMultiRegionFoam, but I found that it's quite difficult to directly integrate the code to my code because of may things such as the "setRegionFluidFields.H" etc. However I understand that basic steps are

1. create fields of each mesh (per region)
2. in each time step, update fields by solving PDEs seperately
3. coupled through the boundary condition "compressible::turbulentTemperatureCoupledBaffleMi xed"

it was also confirmed by the old presentation about "conjugate heat transfer" by Craven and Campbell 2011, link: http://www.google.de/url?sa=t&rct=j&...yET3qTlotFMBEg

I have also done the toturials for chtMultiRegionFoam, but what I want is simply to calculate T for solid coupled with exsting models in melt.

Based on their hints, I extends the laplacianFoam to a very simple heat transfer code for testing/learning purpose. In that code, simple do following steps:
1. create mesh for solid and liquid separately: fvMesh solidMesh, fvMesh liquidMesh
2. create T fields sperately:

      volScalarField Tsolid
    (
        IOobject
        (
            "T",
            runTime.timeName(),
            solidMesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        solidMesh
    );

    volScalarField Tliquid
    (
        IOobject
        (
            "T",
            runTime.timeName(),
            liquidMesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        liquidMesh
    );

3. solving T equations for solid and liquid one after another.

(take the liquid as an example)

{
volScalarField& T = Tliquid;
dimensionedScalar& DT = DTliquid;
            
            solve
            (
                fvm::ddt(T) - fvm::laplacian(DT, T)
            );
}

Test result and problem


I have tested it in a very simple geometry: two blocks of two regions connected by a interface. It was created by blockMesh and splitMeshRegions -cellZones -overwrite. The just created code "chtTFoam" works fine if the BC on interfaces "Solid_to_liquid" and "liquid_to_Solid" are set to e.g. zeroGradient. But If I set them to "compressible::turbulentTemperatureCoupledBaffleMi xed" for conjugate heat transfer, the solver said:

-> FOAM FATAL IO ERROR:
Unknown patchField type compressible::turbulentTemperatureCoupledBaffleMix ed for patch type mappedWall

the patchField type "compressible::turbulentTemperatureCoupledBaffleMi xed" is even not in the list of the valid patch Field.

Question:

1. does anyone know which boundary condition is suitable for such a simple condition?

2. in the above mentioned presentation, the method "Dirichlet-Neumann partitioned Multi-region" was used, but the my first option is not to bluid the boundary condition by myself according to their description. Is there any existing BC?

3. why "compressible::turbulentTemperatureCoupledBaffleMi xed" is not known by the solver? I have included those headers from chtMultiRegionFoam.

Thanks a lot for helping and discussion!

best regards,
Can

[onlyacan]

Thanks to some hints from some colleagues, it works now!
One has to add the libraries in Make/option:
then solver know the boundary condition "compressible::turbulentTemperatureCoupledBaffleMi xed"

EXE_LIBS = \
    -lcompressibleTransportModels \
    -lfluidThermophysicalModels \
    -lsolidThermo \
    -lspecie \
    -lturbulenceModels \
    -lcompressibleTurbulenceModels \
    -lmeshTools \
    -lfiniteVolume \
    -lradiationModels \
    -lfvOptions \
    -lregionModels \
    -lsampling

[c3scriven]

Could you please post you solver in order to understand how are you implementing conjugate heat transfer into buoyantBoussinesqPimpleFoam?.
I'm also trying to modify fabian roesler solver from melting problem: looking for appropriate solvers
but I don't know how to implement chtMultiRegionFoam.

[AmalSoman]

Dear onlyacan,
I tried doing what you did but didn't work. I am relatively new to OpenFOAM. It would be helpful you can share all the changes you made in buoyantbuossinesq pimple foam. I am trying to model incompressible liquid inside a solid cavity with heat transfer from the solid boundaries.


Any suggestion for solving this problem will be great.