CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Bugs (https://www.cfd-online.com/Forums/openfoam-bugs/)
-   -   About chtMultiRegionFoam in parallel (v1.6) (https://www.cfd-online.com/Forums/openfoam-bugs/68194-about-chtmultiregionfoam-parallel-v1-6-a.html)

Zheng.Zhi September 9, 2009 22:31

About chtMultiRegionFoam in parallel (v1.6)
 
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 September 10, 2009 04:37

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

Zheng.Zhi September 10, 2009 05:14

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

mattijs September 10, 2009 07:25

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 September 15, 2009 06:00

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::printStack(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 September 15, 2009 10:47

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 September 15, 2009 21:50

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

autumn1012 September 16, 2009 01:46

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

cvv October 14, 2009 03:39

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::printStack(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 October 14, 2009 08:20

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

It is working now.

woody November 16, 2009 13:46

Hello Mattijs,

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

Thanks

Tobias


All times are GMT -4. The time now is 17:32.