[Zheng.Zhi]

When I use chtMultiRegionFoam to solve multiRegionHeater case in parallel, I want to set topAir_to_heater with kqRWallFunction and epsilonWallFunction boundary conditions. But there was the error said topAir_to_heater must be wall instead of directMappedWall. Is there any method to solver this problem?
Thanks!

[mattijs]

Do you get this error running non-parallel as well?

[Zheng.Zhi]

Yes，maybe the problem is the wall function needs wallFvPatch , but the directMappedWall is wallPolyPatch ?

[mattijs]

directMappedWall is derived from wallPolyPatch. The problem was that the finite volume equivalent wasn't derived from wallFvPatch. I pushed a fix to 1.6.x. Give it a go.

Thanks for reporting.

[autumn1012]

Here is another problem when I tried 1.6.x,

Solving for fluid region bottomAir
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Ux, Initial residual = 2.211858e-16, Final residual = 2.211858e-16, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 6.771384e-09, No Iterations 22
DILUPBiCG: Solving for Uz, Initial residual = 1.036037e-15, Final residual = 1.036037e-15, No Iterations 0
DILUPBiCG: Solving for h, Initial residual = 0.6044857, Final residual = 8.30665e-09, No Iterations 40
Min/max T:300 300
GAMG: Solving for p, Initial residual = 1, Final residual = 0.005459487, No Iterations 2
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (bottomAir): sum local = 0.001237545, global = 4.109187e-06, cumulative = 4.109187e-06
GAMG: Solving for p, Initial residual = 0.6006277, Final residual = 6.905954e-09, No Iterations 27
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (bottomAir): sum local = 2.018032e-09, global = -4.377309e-11, cumulative = 4.109143e-06
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::compressible::RASModels::epsilonWallFunction FvPatchScalarField::updateCoeffs() in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#4 Foam::compressible::RASModels::kEpsilon::correct() in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#5 main in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/chtMultiRegionFoam"
#6 __libc_start_main in "/lib64/libc.so.6"
#7 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception

Then I checked epsilonWallFunctionFvPatchScalarField and found there are some calculations like this

const scalarField& y = rasModel.y()[patch().index()];

forAll(nutw, faceI)
{
...
epsilon[faceCellI] = Cmu75*pow(k[faceCellI], 1.5)/(kappa_*y[faceI]);
...
}

So I modified chtMultiRegionFoam to output rasModel.y() of patch like bottomAir_to_heater, then I found all of them are 0, so the above error happened.

Is there any method to solver this problem? Thanks.

[mattijs]

I've just pushed a lot of changes to 1.6.x to do with wall-type recognition. Could you try again?

Thanks,

Mattijs

[autumn1012]

Ok, I will give a reply when I try again.

[autumn1012]

The problem has been solved. The multiRegionHeater case can be running in both non-parallel and parallel. Thank you for your update.

[cvv]

Hi,

Can someone perhaps post a link to the tutorial for chtMultiRegionFoam in 1.6? I tried the one from 1.5 but get the following error when I run the solver:
Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>


Not Implemented
Trying to construct an genericFvPatchField on patch bottomAir_to_rightSolid of field h#0 Foam::error:rintStack(Foam::Ostream&) at /opt/Op enFOAM/r1.6/debug/OpenFOAM-1.6/src/OSspecific/POSIX/printStack.C:203

I read on another thread that this may be due to the boundary type. In this case the type is solidWallTemperatureCoupled. Was this changed in 1.6?

Regards
Carel

[cvv]

..never mind, just did not read the instructions!

It is working now.

[woody]

Hello Mattijs,

are there other BC's like directMappedWall to make two regions interact?

Thanks

Tobias