[S03r3n]

Hello togehter,

I have the issue that my simulation (simpleFoam, steady-state) converges for the case of low viscosity, but no convergence for high viscosity.
What can be the reason? Solver related?

For more details, here are the viscosity models:
- Low viscosity

transportModel  BirdCarreau;
nuInf [0 2 -1 0 0 0 0]    0;
nu0   [0 2 -1 0 0 0 0]    37.521;
k     [0 0 1 0 0 0 0]     0.25011;
n     [0 0 0 0 0 0 0]     0.11815;
a     [0 0 0 0 0 0 0]     1;

- High viscosity

transportModel  BirdCarreau;
nuInf [0 2 -1 0 0 0 0]    0;
nu0   [0 2 -1 0 0 0 0]    433.2756;
k     [0 0 1 0 0 0 0]     6.017543;
n     [0 0 0 0 0 0 0]     0.1327432;
a     [0 0 0 0 0 0 0]     1;

In addition, I have attached the convergence plots for both cases.

Below you can find my chosen solver settings and the mesh quality.

controlDict

application     simpleFoam;
startFrom       startTime;
startTime       0;
stopAt          endTime;
endTime         3000;
deltaT          1;
writeControl    timeStep;
writeInterval   100;
purgeWrite      1;
writeFormat     ascii;
writePrecision  6;
writeCompression off;
timeFormat      general;
timePrecision   6;
runTimeModifiable true;

fvSchemes

ddtSchemes
{
    default         steadyState;
}
gradSchemes
{
    default         Gauss linear;
}
divSchemes
{
    default         none;
    div(phi,U)      bounded Gauss linearUpwind grad(U);
    div((nuEff*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
    default         Gauss linear corrected;
}
interpolationSchemes
{
    default         linear;
}
snGradSchemes
{
    default         corrected;
}

fvSolution

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-10;
        relTol          0.1;
        smoother        GaussSeidel;
    }
    U
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-10;
        relTol          0.1;
    }
}
SIMPLE
{
    nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7;
    }
}

checkMesh

Checking geometry...
    Overall domain bounding box (-0.045 -0.045 -3.28327e-06) (0.045 0.045 0.396003)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (-3.07219e-15 2.25183e-15 -7.41942e-17) OK.
    Max cell openness = 4.00758e-16 OK.
    Max aspect ratio = 9.9936 OK.
    Minimum face area = 1.77711e-09. Maximum face area = 5.09394e-05.  Face area magnitudes OK.
    Min volume = 4.96432e-13. Max volume = 1.40176e-07.  Total volume = 0.00177843.  Cell volumes OK.
    Mesh non-orthogonality Max: 65.1136 average: 13.681
    Non-orthogonality check OK.
    Face pyramids OK.
 ***Max skewness = 8.30373, 25 highly skew faces detected which may impair the quality of the results
  <<Writing 25 skew faces to set skewFaces
    Coupled point location match (average 0) OK.

Failed 1 mesh checks.

[Alczem]

Hey,


Your mesh has some flaws that might be affecting your case, like non-orthogonal and skewed cells. You should configure fvSchemes and fvSolutions accordingly.


Try to set nNonOrthogonalCorrectors to 1 or even 2, and use limited 0.33 for snGradSchemes and Gauss linear limited 0.33 for the laplacian.


Instead of Gauss linear for the gradient scheme, leastSquares can handle skewed cells a bit better from what I have read.



Limiters can also help for the gradient schemes, for instance grad(U) cellLimited Gauss linear 1; and use first order for divergence schemes as long as the simulation is not stable.


If you can, ramp up your inlet velocity (if an inlet is used) over a few dozens iterations to avoid huge changes in the domain.


Hope it can help!

[S03r3n]

Thanks for your post!

The ramp-up of the inlet velocity (or in my case flow rate at the inlet) helped!

Originally Posted by Alczem

Hey,


Your mesh has some flaws that might be affecting your case, like non-orthogonal and skewed cells. You should configure fvSchemes and fvSolutions accordingly.


Try to set nNonOrthogonalCorrectors to 1 or even 2, and use limited 0.33 for snGradSchemes and Gauss linear limited 0.33 for the laplacian.


Instead of Gauss linear for the gradient scheme, leastSquares can handle skewed cells a bit better from what I have read.



Limiters can also help for the gradient schemes, for instance grad(U) cellLimited Gauss linear 1; and use first order for divergence schemes as long as the simulation is not stable.


If you can, ramp up your inlet velocity (if an inlet is used) over a few dozens iterations to avoid huge changes in the domain.


Hope it can help!

[rocketLauncher]

Hey,

Just in case you are still not achieving the desired solution - the increase in viscosity could be changing your reynolds enough that you are now in a higher turbulence regime than before. If that's the case, your mesh might need to be finer for the BL (assuming this is the type of case you are running). It's good to address the mesh issues via the solver settings, but might be worth to revisit the mesh itself