[kirli]

Hello Foamers.

I am kind of new in OpenFoam..

I am trying to run SimpleFoam turbulence simulation on a 3D geometry.
It is a kind of pipe with flow splitter. The fluid is water (one phase).

I got this kind of error:

DILUPBiCG: Solving for Ux, Initial residual = 1.96286e-14, Final residual = 1.96286e-14, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 3.56233e-14, Final residual = 3.56233e-14, No Iterations 0
DILUPBiCG: Solving for Uz, Initial residual = 1.38946e-13, Final residual = 1.38946e-13, No Iterations 0
DICPCG: Solving for p, Initial residual = 1, Final residual = 2.63715e+06, No Iterations 1001
time step continuity errors : sum local = 7.66448e+73, global = 1.60172e+66, cumulative = 1.60172e+66
[3] #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #2 in "/lib/libc.so.6"
[3] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

What is the reason for the negative K?
Thanks

[kirli]

I believe that the problem is in the mesh.

I have made a CAD model (solidWorks) and then mesh it in salome. Import it in UNV format to OpenFoam

[shyam]

Hi Kirli,
Most of us go through this problem of bounding epsilon or omega. Some of things which helped me are the following, which are taken from various threads of CFD-online.

check your mesh using the command checkMesh and look for non-orthogonality, if its between
a. 0 to 50 full corrected scheme is applicable,
b. 50 to 70 limited correction is required,
c. 70 to 80 stability possible, accuracy compromised,
d. above 80 stability very difficult to attain

For case b use the following settings in fvSchemes

gradSchemes
{
default faceLimited leastSquares 0.5;
}
laplacianSchemes
{
default Gauss linear limited 0.33;
}
snGradSchemes
{
default limited 0.33;
}

for case c and d I would suggest to revisit your mesh.

[Manoj Paithane]

Originally Posted by shyam

Hi Kirli,
Most of us go through this problem of bounding epsilon or omega. Some of things which helped me are the following, which are taken from various threads of CFD-online.

check your mesh using the command checkMesh and look for non-orthogonality, if its between
a. 0 to 50 full corrected scheme is applicable,
b. 50 to 70 limited correction is required,
c. 70 to 80 stability possible, accuracy compromised,
d. above 80 stability very difficult to attain

For case b use the following settings in fvSchemes

gradSchemes
{
default faceLimited leastSquares 0.5;
}
laplacianSchemes
{
default Gauss linear limited 0.33;
}
snGradSchemes
{
default limited 0.33;
}

for case c and d I would suggest to revisit your mesh.

what to do when mesh non orthogonality fall in between 70 to 80?
how to avoid K and epsilon bounding..?


Simulation show this type of iteration
Solving for fluid region fluid
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCGStab: Solving for Ux, Initial residual = 2.21117e-05, Final residual = 3.763e-08, No Iterations 1
DILUPBiCGStab: Solving for Uy, Initial residual = 0.000157765, Final residual = 1.72667e-08, No Iterations 1
DILUPBiCGStab: Solving for Uz, Initial residual = 0.00014488, Final residual = 2.0605e-08, No Iterations 1
DILUPBiCGStab: Solving for O2, Initial residual = 0.000226158, Final residual = 2.88741e-07, No Iterations 1
DILUPBiCGStab: Solving for H2O, Initial residual = 0.000183538, Final residual = 2.31311e-07, No Iterations 1
DILUPBiCGStab: Solving for h, Initial residual = 7.57334e-05, Final residual = 2.42469e-09, No Iterations 1
Min/max T:359.675 873.567
GAMG: Solving for p_rgh, Initial residual = 0.00126951, Final residual = 4.47571e-06, No Iterations 1
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 5.48993e-09, global = 1.49437e-09, cumulative = 1.49437e-09
Min/max rho:42.5686 103.34
GAMG: Solving for p_rgh, Initial residual = 8.0525e-06, Final residual = 7.49119e-08, No Iterations 4
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 9.41727e-11, global = 3.81731e-12, cumulative = 1.49819e-09
Min/max rho:42.5686 103.34
DILUPBiCGStab: Solving for epsilon, Initial residual = 8.46681e-06, Final residual = 6.31942e-09, No Iterations 1
bounding epsilon, min: -10.8933 max: 719259 average: 7597.29
DILUPBiCGStab: Solving for k, Initial residual = 3.15017e-05, Final residual = 5.1379e-08, No Iterations 1

Solving for solid region metal
DICPCG: Solving for h, Initial residual = 6.85466e-05, Final residual = 2.75706e-11, No Iterations 1
Min/max T:305.063 791.245
ExecutionTime = 8076.51 s ClockTime = 8290 s

Region: fluid Courant Number mean: 0.035771 max: 0.598896
Region: metal Diffusion Number mean: 2.45178e-05 max: 0.000784157
deltaT = 3.88385e-05
Time = 0.19064

[vince_cfd]

I'm running a turbulent chtMultiRegionFoam case and I can't reach convergence. I used the checkMesh tool and found:

Mesh non-orthogonality Max: 85.1202 average: 19.8936
*Number of severely non-orthogonal (> 70 degrees) faces: 25401.
Non-orthogonality check OK.
<<Writing 25401 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 3.6605 OK.
Coupled point location match (average 0) OK.

My total faces are 2335052, so about 1% of the faces are above the recommended value of 80 (and 70). Is it likely my convergence problems come from this, or is it alright to have some faces over the recommended value?


Greetings

[ARTisticCFD]

Originally Posted by vince_cfd

I'm running a turbulent chtMultiRegionFoam case and I can't reach convergence. I used the checkMesh tool and found:

Mesh non-orthogonality Max: 85.1202 average: 19.8936
*Number of severely non-orthogonal (> 70 degrees) faces: 25401.
Non-orthogonality check OK.
<<Writing 25401 non-orthogonal faces to set nonOrthoFaces

I think the non-orthogonality check is passed. However, 85 seems to be quite skewed. See whether you can improve on it.

Originally Posted by vince_cfd

My total faces are 2335052, so about 1% of the faces are above the recommended value of 80 (and 70). Is it likely my convergence problems come from this, or is it alright to have some faces over the recommended value?

Could you give more details? Could you comment on the ranges of Courant number during your run?

[vince_cfd]

check post below

[vince_cfd]

Hey, thank you for your reply. I already answered this morning, but somehow my answer got lost in the aether.

Originally Posted by ARTisticCFD

I think the non-orthogonality check is passed. However, 85 seems to be quite skewed. See whether you can improve on it.

Im already working on it, but Im not to sure if I can. The geometry is a spiral, so its destined to have some non-orthogonality.

Originally Posted by ARTisticCFD

Could you give more details? Could you comment on the ranges of Courant number during your run?

Some details: metal temperature 70°C, cooling water temperature 30°C. Reynolds ranging from 7500-15000. Turbulence modeled with kOmegaSST.
Courant Number is set to max. 1.0, but reaches about 1.2 during the working part of the simulation. After approx. 0.04s the "good-looking" values start spiraling out of control and within 1-2 timesteps they print negative temperatures, negative rho and courant number arround 1e7.

Any ideas on what is happening? I can provide more information if needed.

Greetings