CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   buoyantBoussinesqSimpleFoam and kappat (https://www.cfd-online.com/Forums/openfoam-solving/94440-buoyantboussinesqsimplefoam-kappat.html)

 camoesas November 16, 2011 05:28

buoyantBoussinesqSimpleFoam and kappat

HI OF Users,

I am simulating the flow over a hot board. I have done various Simulations with rhoSimpleFoam and buoyantSimpleFoam. Now I want to start a Simulation with the solver buoyantBoussinesqSimpleFoam. For that I have to specify the kappat, the 'kinematic turbulent thermal conductivity'.
But I canīt find any information of how to calculate the initial values and which BC to set.

Is there any Information for that?
Thanks

 al_pr November 16, 2011 08:27

Hello camoesas,

I found the following definition for the turbulent heat conductivity. It is the product of the heat capacity and the turbulent kinematic viscosity of your considered fluid. I found that in the following book (you can find it in google books): Innovative Food Processing Technologies: Advances in Multiphysics Simulation( Kai Knoerzer,Pablo Juliano,Peter Roupas).

But I think you don't need to specify it exactly. For the walls you have a wall function and for the "Inlet" you can use the "calculated" boundary conditon. For the "Outlet" it is zeroGradient.

I hope this helps.

Best regards

 camoesas November 16, 2011 10:40

1 Attachment(s)
HI Alex,

Thanks for the hint. I have now for kappat:

Inlet: calculated,
All Walls: kappatJayatillekeWallFunction;
and some empty and symmetry patches.

But my solition is aborting in the first iteration giving me this message:

Quote:
 Create time Create mesh for time = 0 Reading g Reading thermophysical properties Reading field T Reading field p_rgh Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Creating turbulence model Selecting RAS turbulence model kOmegaSST kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; gamma1 0.5532; gamma2 0.4403; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; c1 10; } Reading field kappat Calculating field g.h SIMPLE: convergence criteria field p_rgh tolerance 1e-05 field U tolerance 1e-06 field h tolerance 1e-06 field "(k|epsilon|omega)" tolerance 1e-06 Starting time loop Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 0.0002433629501, Final residual = 1.756349447e-07, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.002939968679, Final residual = 2.378267403e-06, No Iterations 1 DILUPBiCG: Solving for T, Initial residual = 1, Final residual = 0.03016392268, No Iterations 1 --> FOAM FATAL ERROR: request for volScalarField rho from objectRegistry region0 failed available objects of type volScalarField are 14 ( div(phi) rhok nut rAU k p_rgh nu gh p T omega p_rghPrevIter y kappat ) From function objectRegistry::lookupObject(const word&) const in file /home/camoesas/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 131. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 Foam::GeometricField const& Foam::objectRegistry::lookupObject >(Foam::word const&) const in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #3 Foam::buoyantPressureFvPatchScalarField::updateCoe ffs() in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #4 Foam::fvMatrix::fvMatrix(Foam::GeometricFi eld const&, Foam::dimensionSet const&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam" #5 Foam::fv::gaussLaplacianScheme::fvmLaplacianUncorrected(Foam::GeometricFi eld const&, Foam::GeometricField const&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #6 Foam::fv::gaussLaplacianScheme::fvmLaplacian(Foam::GeometricField const&, Foam::GeometricField const&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #7 in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam" #8 in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam" #9 in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam" #10 __libc_start_main in "/lib64/libc.so.6" #11 at /usr/src/packages/BUILD/glibc-2.11.3/csu/../sysdeps/x86_64/elf/start.S:116
What does this mean? Is this an error of my BC or of the numerical setup?
Thanks for any hints

I have uploaded the whole case but I had to delete U p files. I have adopted them for initialization from another simulation so they are to large...

 al_pr November 16, 2011 13:24

You have to define a reference for the density for the buoyantpressure boundary conditions.
...

HOT
{
type buoyantPressure;

rho rhok;

value \$internalField;
}

...

By the way, for the inlet it is better to define the pressure as zerogradient. Otherwise your problem is overdetermined.

I hope this will fix the problem. Good luck for your simulation!

Regards,
Alex

 camoesas November 17, 2011 09:18

HI Alex,

thank you very much for going throw my case! And for this valuable solution. Indeed it fixed my simulation. :cool:

But my pressure inlet is already zeroGradient. Do you mean the inlet for p_rgh?

 palmerlee February 26, 2014 08:39

Les

Quote:
 Originally Posted by al_pr (Post 332314) Hello camoesas, I found the following definition for the turbulent heat conductivity. It is the product of the heat capacity and the turbulent kinematic viscosity of your considered fluid. I found that in the following book (you can find it in google books): Innovative Food Processing Technologies: Advances in Multiphysics Simulation( Kai Knoerzer,Pablo Juliano,Peter Roupas). But I think you don't need to specify it exactly. For the walls you have a wall function and for the "Inlet" you can use the "calculated" boundary conditon. For the "Outlet" it is zeroGradient. I hope this helps. Best regards
Hi, Alex!

What about LES? Is it still the same way to set up boundary condition for kappat as you said? Or should I do it the way as nuSgs in tutorial cases, that is, to set all boundaries zeroGradient?

Best regards
Peter

 All times are GMT -4. The time now is 13:32.