CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   buoyantBoussinesqSimpleFoam and kappat (http://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,
Outlet: zeroGradient
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<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::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<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::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 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 15:31.