[camoesas]

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 can´t find any information of how to calculate the initial values and which BC to set.

Is there any Information for that?
Thanks

[al_pr]

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]

HI Alex,

Thanks for the hint. I have now for kappat:

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

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

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<Type>(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:rintStack(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<double, Foam::fvPatchField, Foam::volMesh> const& Foam:bjectRegistry::lookupObject<Foam::Geometric Field<double, Foam::fvPatchField, Foam::volMesh> >(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<double>::fvMatrix(Foam::GeometricFi eld<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam"
#5 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricFi eld<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#6 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> 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]

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]

HI Alex,

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

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

[palmerlee]

Originally Posted by al_pr

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