CFD Online Discussion Forums - low reynolds re turbulence boundary and yPlus values

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - low reynolds re turbulence boundary and yPlus values (https://www.cfd-online.com/Forums/openfoam-solving/71475-low-reynolds-re-turbulence-boundary-yplus-values.html)

Quote:

Originally Posted by sebastian (Post 342905)

For me it does not make any sense to set k and epsilon to zeroGradient at the wall. I recently had a look in the original paper and they use k = epsilon = 0 there, which is conform to my understanding of a low-Re-model so far.
Concerning the turbulent viscosity mut or nut, I have tested a calculated as well as a zeroGradient boundary condition. There was no difference difference in both calculations.

Just for a comparison I have tested k and epsilon with a zeroGradient bc. This results in an unphysical thickening of the boundary layer.

Sebastian

Hi,
I agree with you about the value of k and epsilon near the wall. If the reynolds is low then the value of k and espilon should be low too.
However in the sonicFoam/nacaAirfoil tutorial (compressible case) k and epsilon are have a high fixed value (several thousands).
In incompressible/boundaryFoam/boundaryLaunderSharma (incompressible case) k and epsilon have a very low value at the wall (around 1e-10 for both).

I just don't understand on what is based this difference, and why this is different for compressible and incompressible fluid.

Hi malaboss,

Do you find something wich can explain why there is this difference?

Valentin

Well,
I just watch the boundary conditions of both cases (nacaairfoil and boundaryLaunderSharma) which use LaunderSharma.
In nacaAirfoil, wall function are used while it should be low Re wall function or nothing at all in a low Re model. This could explain the high values of k at wall, and as a conclusion, Naca Airfoil would not be a good example to understand which boundary conditions we have to set for a Low Re model.
See : http://www.cfd-online.com/Wiki/Low-R...els#References for boundary conditions

Be careful though, I may be wrong since I don't know how you use a wall function at the wall for a compressible case like naca airfoil. I tried to see how wall fucntion are implemented in Launder and Sharma models, but all I found was this : http://www.cfd-online.com/Forums/ope...k-e-model.html which states that Launder and Sharma was conceived for incompressible cases. About the general implementation of wall function in compressible cases, it seems like there is no big difference with the incompressible. http://jullio.pe.kr/fluent6.1/help/html/ug/node451.htm
I did not manage to see the y+ value of the naca airfoil case as I could not run the case.

Please tell me if you find something new and more relevant !

Thank you for your help malaboss :)
I don't know if launder-sharma is correct in the compressible cases but it is in the list of tubulent models available in compressible.
I will give a try to this model in my case and will say if it's ok.

Do you know the boundary conditions for nut and alphat that I have to give at walls? I found posts wich say zeroGradient but I'm not sure about this.

If we keep on reasoning as we did just before, nut should be set to zero (fixed value) on the wall. There is no turbulence so there is no turbulence viscosity, that is, no viscosity due to turbulence.

For alpha t (again i'm not an expert for compressible flows) it represents the thermal diffusivity, proportionnal to thermal conductivity. Near the wall we have nearly no turbulence, so no convection, hence no conductivity. To me, you can fix the value to zero for alpha t.

Where did you find the Boundary conditions you are talking about, as it doesn't match my thoughts ?

I agree with you. According to me zeroGradient doesn't have any sense.

Quote:

Originally Posted by jishnusoni (Post 254151)

Hello All,

I am trying to simulate an impingingjet using the simpleFoam in OF1.6.x. I am trying to follow the threads and tried different things. But I am still getting the same error. I am posting my error and attaching my initial bc. Your support will be greatly appreciated.

Time = 759

DILUPBiCG: Solving for Ux, Initial residual = 0.364807, Final residual = 0.0331038, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.401396, Final residual = 0.0185339, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.439448, Final residual = 0.0046591, No Iterations 1
GAMG: Solving for p, Initial residual = 0.569614, Final residual = 0.00428777, No Iterations 66
time step continuity errors : sum local = 3.14096e+42, global = 3.09629e+39, cumulative = 6.80133e+40
DILUPBiCG: Solving for epsilon, Initial residual = 1.08298e-09, Final residual = 1.08298e-09, No Iterations 0
DILUPBiCG: Solving for k, Initial residual = 0.000115294, Final residual = 2.84805e-06, No Iterations 2
ExecutionTime = 47327.3 s ClockTime = 48069 s

Time = 760

DILUPBiCG: Solving for Ux, Initial residual = 0.506818, Final residual = 0.00973123, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.603294, Final residual = 0.0122224, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.280386, Final residual = 0.00518198, No Iterations 2
GAMG: Solving for p, Initial residual = 0.0695246, Final residual = 0.000686704, No Iterations 30
time step continuity errors : sum local = 1.41992e+43, global = 4.71133e+41, cumulative = 5.39147e+41
DILUPBiCG: Solving for epsilon, Initial residual = 3.87187e-11, Final residual = 3.87187e-11, No Iterations 0
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.0894909, No Iterations 1
bounding k, min: -7.27376e+51 max: 5.05817e+89 average: 5.17561e+84
ExecutionTime = 47386.5 s ClockTime = 48159 s

Time = 761

DILUPBiCG: Solving for Ux, Initial residual = 0.417362, Final residual = 0.0145424, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.51114, Final residual = 0.0224704, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.376437, Final residual = 0.0288099, No Iterations 1
GAMG: Solving for p, Initial residual = 0.629327, Final residual = 0.00528483, No Iterations 8
time step continuity errors : sum local = 1.11456e+78, global = 4.87405e+75, cumulative = 4.87405e+75
DILUPBiCG: Solving for epsilon, Initial residual = 4.23728e-09, Final residual = 4.23728e-09, No Iterations 0
#0 Foam::error::printStack(Foam::Ostream&) in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#5 Foam::lduMatrix::solverPerformance Foam::solve<double>(Foam::tmp<Foam::fvMatrix<doubl e> > const&) in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModels::kEpsilon::correct () in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#7 main in "/home/jish/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib/libc.so.6"
#9 _start at /build/buildd/eglibc-2.10.1/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception

thanks

regards
jish

Hi, I have simulated impinging jet before and it succeed even without initialization
1) What is the turbulence model in openfoam used? Is it a Low-Re or high-Re model.
My suggestion would be Low-Re model as impinging jet involves complex physics that the standard wall function approach might not be able to predict well. From you initial condition settings (epsilonWallFunction, kqRWallFunction, nutSpalartAllmarasWallFunction you are using a high-Re model right?) I tried modelling in fluent impinging jet axisymmetric - use realisable KE and enhanced wall treatment. I attended a course by fluent that taught us that for complex physics it is better to use enhanced wall treatment. In OpenFOAM, there is no equivalent enhanced wall treatment in the Hi-Re Realisable ke model so another way to get around this is to use Low-Re model such as laundersharmaKE which contains damping functions to resolve boundary layer flow. Some people suggest using nut_wall: nutSpalartAllmarasWallFunction or nutSpalartAllmarasStandardWallFunction to make a Hi-Re model looks like low-Re model. I do not think this is right way to do. I have read the thread somewhere on this matter. So strongly recommend to try LaunderSharmaKE.

2) How does your geometry looks like? can you draw out the problem?

3) What are your fvSchemse and fvSolution? Sometimes these are the things that cause continuity to blow up.

4) For nut, is there any reason you use nutSpalartAllmarasStandardWallfunction over nutkWallFunction if using Hi-Re model? Any advantage?