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! 
Do you get this error running nonparallel as well?

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

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. 
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 = 2.211858e16, Final residual = 2.211858e16, No Iterations 0 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 6.771384e09, No Iterations 22 DILUPBiCG: Solving for Uz, Initial residual = 1.036037e15, Final residual = 1.036037e15, No Iterations 0 DILUPBiCG: Solving for h, Initial residual = 0.6044857, Final residual = 8.30665e09, 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 = 4.109187e06, cumulative = 4.109187e06 GAMG: Solving for p, Initial residual = 0.6006277, Final residual = 6.905954e09, No Iterations 27 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (bottomAir): sum local = 2.018032e09, global = 4.377309e11, cumulative = 4.109143e06 #0 Foam::error::printStack(Foam::Ostream&) in "/home/fxy/OpenFOAM/OpenFOAM1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/fxy/OpenFOAM/OpenFOAM1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #2 ?? in "/lib64/libc.so.6" #3 Foam::compressible::RASModels::epsilonWallFunction FvPatchScalarField::updateCoeffs() in "/home/fxy/OpenFOAM/OpenFOAM1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so" #4 Foam::compressible::RASModels::kEpsilon::correct() in "/home/fxy/OpenFOAM/OpenFOAM1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so" #5 main in "/home/fxy/OpenFOAM/OpenFOAM1.6.x/applications/bin/linux64GccDPOpt/chtMultiRegionFoam" #6 __libc_start_main in "/lib64/libc.so.6" #7 _start at /usr/src/packages/BUILD/glibc2.9/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. 
I've just pushed a lot of changes to 1.6.x to do with walltype recognition. Could you try again?
Thanks, Mattijs 
Ok, I will give a reply when I try again.

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

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/OpenFOAM1.6/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 
..never mind, just did not read the instructions!
It is working now. 
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 11:25. 