simpleFoam with Launder-Sharma Model
 

Hello everyone,
I'm a new user with openfoam. Now i want to use simpleFoam with Launder-Sharma Low-Re Model. There's only one time step calculated. Then a erro as below is displayed.

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model LaunderSharmaKE
LaunderSharmaKECoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}


Starting time loop

Time = 0.1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0606568, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.995352, Final residual = 0.0222388, No Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00735996, No Iterations 6
DICPCG: Solving for p, Initial residual = 0.00365507, Final residual = 3.33199e-05, No Iterations 63
DICPCG: Solving for p, Initial residual = 2.37913e-05, Final residual = 8.92903e-07, No Iterations 30
time step continuity errors : sum local = 4.57548e-05, global = -4.42317e-06, cumulative = -4.42317e-06
#0 Foam::error::printStack(Foam::Ostream&) in "/usr/local/OpenFOAM/1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/usr/local/OpenFOAM/1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/usr/local/OpenFOAM/1.6/lib/li
#4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::sh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/usr/local/OpenFOAM/1.6/lib/linux64GccDPO
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMeshField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/usr/local/OpenFOAM/1
#6 Foam::incompressible::RASModels::LaunderSharmaKE:: correct() in "/usr/local/OpenFOAM/1.6/lib/linux64GccDPOpt/libincompressible
#7 main in "/usr/local/OpenFOAM/1.6/applications/bin/linux64GccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib64/libc.so.6"
#9 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116
Floating exception

I cann't get any useful information from the erro.
The p, U, k, nut, epsilon are gaven as boundary condition.
My question is, can simpleFoam be used with LS Model or did I do something wrong?

Hi,

simpleFoam is able to use LaunderSharma,

look at following posting:
http://www.cfd-online.com/Forums/ope...us-values.html

You must be careful with your inlet bc's for k and epsilon.

Regards Thomas

Hi Thomas,
Thanks for the reply.
why cannot i set the k and epsilon not equal 0 for the boundary condition at wall? That was the problem of me.
Regards Yang

I think you are not allowed to divide through zero.

Hi Examosty,

why would you set non-zero values at solid walls for k and epsilon? Launder-Sharma turbulence model is so called "low reynolds number" closure ad its damping function, values of constants, etc. are derived on the basis of zero values for k and epsilon (at solid walls)!

I really suggest that you grab your hands on the following book David C. Wilcox, Turbulence Modelling For CFD

Cheers,
Primoz

Hi Primoz,
that's what i thought and what i did, set k and epsilon at solid wall equal 0. Then the error as i've replayed in the beginning occurred. As Thomas said, it's a problem of dividing through zero.
Regards,
June

now I am getting the point! I do not know exactly how the Launder-Shrama is incorporated in OpenFoam, but "the general" theory for solid wall behaviour is (at lest I think so):

• since there are no velocity fluctuations in a near wall region (viscous forces are predominant) the turbulence kinetic energy is 0 at solid wall
• for dissipation of turbulence kinetic energy "low Re" closures solves "modified" equation for epsilon

epsilon_mod=epsilon-D

• so actually, you are prescribing boundary conditions for "modified epsilon", which is zero at solid wall

Hope this helps,
Primoz

Hello Foamers!
I'm a new user in OpenFoam. I appreciate your helps and tips and I'm gratefull for that. My problem is incompressible flow through radial diffuser with low Reynolds number. I want to use LaunderSharmaKE turb. model without wall functions.

1) I deleted nut file and k and epsilon files were setted with fixedValue for wall boundary conditions. The k and epsilon values on the wall I fixed with zero and close to zero (1e-10). In these two situations floting point exception ocurred.

2) Can someone check my attachement files to find out if I made a mistake?

3) I don't understand what "value" below Intensity really does mean. The value of turb. kinetic energy (k) will be calculated based on turb. intensity, so why set this value? Please, can someone clear it me?

inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.03;
value uniform 0.3;
}



Thanks!

You cannot set the epsilon to zero close to the wall for LaunderSharmaKE. I will try my best to explain.


LaunderSharmaKE is a low-RE turbulence model implemented in OpenFOAM. As such, the original formulation of k-epsilon turbulence model is meant as a high-Re model. Now by low and high-Re, I mean the local Reynolds number i.e. the Reynolds number at the first layer of cells that are in contact with the wall. When you have a very small value for the height of the first cell, your Reynolds number definition being Uy/\nu means that the value of Re is also low. Remember that the velocity U is also small close to the wall. These two small values makes the LOCAL reynolds number a small number and hence low-Re. For low-Re models, you need a y+ ~ 1 so that viscous sub-layer is resolved.


Now coming to epsilon. So epsilon is nothing but the turbulence dissipation. if you take a plot of the variation of dissipation as a function of y+, you will see that the dissipation actually decreases as you move away from the wall with the value being the highest at the wall and a small peak observed in the buffer layer. This makes sense right? Dissipation according to the turbulence energy cascade is caused by small scales and the small scales are present close to the wall. So by extension, you will have dissipation close to the wall. The small peak observed in the buffer layer is to balance the production of turbulent kinetic energy that peaks in the same region.


This now should answer your question - you cannot have epsilon (or turbulence dissipation) at the wall to be zero. This will cause an imbalance in your system where the excess production of kinetic energy is not dissipated. If you use a LaunderShamraKE which is a low-Re turbulence model, you need to explicitly specify the value of epsilon at the wall. In case of a high-Re turbulence model such as the regular formulation of the k-epsilon model, the point will lie somewhere in the log-law region (by point, i mean the height of the first cell adjacent to the wall). So in this case too you will have to specify the value and the wall-function will ensure the correct estimation of the epsilon in the region between the first cell-centroid and the wall.


In case of k, the production of turbulence kinetic energy is approximated as the product of the turbulent stress and the mean velocity gradient. Now in CFD codes, there is a hard limit that is set wherein, the turbulent kinetic energy is set to zero if it is below a y+ of 11.5 and it is set to the product of the wall shear stress and mean velocity gradient if y+ is greater than this value.