[floquation]

Originally Posted by Santiago

You use the SIMPLE loops (or as you call them, outer) in an attempt to stabilize (make the simulation more robust) the run by introducing artificial viscosity via a relaxation flux. Is important to recall that some of the time schemes in OF add some sort of numerical flux in the convective term. Thus, repetitive SIMPLE iterations will add to this spurious flux. Note that This "error" is inversely proportional to delta t. In an orthogonal grid, such flux may become a 'false friend' if your Co becomes too small. So, if your grid is not bad, Why do you need more than one SIMPLE loop?

I can see how such an artificial flux may result in outer/SIMPLE iterations not converging. When the relaxation is turned off for the final timestep (here: iteration 200), the residuals do again converge, because the artificial flux is "turned off"?
What remains is the question "why use more than one iteration": That's to make sure that your system of equations are solved properly. Within one outer/SIMPLE iteration, the alpha/VOF equation would only be solved once using the old pressure and velocity fields. (Evidently, pressure and velocity are already being iterated using the inner/PISO iterations.) To correctly solve for the entire system of equations, you'd thus need to iterate, don't you?
If I combine what you said with what I think to be true, then one should use little outer/SIMPLE iterations together with no relaxation for the best result? (Unless relaxation is needed, because the mesh is poor / system is ill-posed / etc., for which the system needs stabilisation.)

[mszeto715]

Thank you for the response Joaran. How have people learned to use PIMPLE correctly before Tobias Holzmann's publication? It's surprising to me that the usage explained by Dr. Holzmann is not a template in any of the OpenFOAM tutorials. Perhaps this is an artifact of OpenFOAM being open-source code. I have even found that it is not applicable to some of the PIMPLE-related solvers like heatTransfer/chtMultiRegionFoam (though I guess they are just outdated). I would like to better understand the context behind this correct usage (i.e., using residual controls, setting the number of outer loops to some high value). Also, are there other sources that describe strategies for configuring the settings? Many thanks for your attention. -Mimi

[joaran]

Originally Posted by mszeto715

Thank you for the response Joaran. How have people learned to use PIMPLE correctly before Tobias Holzmann's publication? It's surprising to me that the usage explained by Dr. Holzmann is not a template in any of the OpenFOAM tutorials. Perhaps this is an artifact of OpenFOAM being open-source code. I have even found that it is not applicable to some of the PIMPLE-related solvers like heatTransfer/chtMultiRegionFoam (though I guess they are just outdated). I would like to better understand the context behind this correct usage (i.e., using residual controls, setting the number of outer loops to some high value). Also, are there other sources that describe strategies for configuring the settings? Many thanks for your attention. -Mimi

Hi mszeto715,



I actually haven't found any better information about the configuration of fvSolution than Holzmann's book. I think that the best way to learn to use OpenFOAM is playing with it, making mistakes, and search in this forum and/or googling your errors to find an answer. I suppose though it'd be better to take a course, if you can afford it. And ultimately all the information is contained in the installation files, be it a comment, or a program line, so I'd recommend you try to learn how to read the files and make an effort to understand what the main lines do. For that, it's a really good idea to spend some time taking a tutorial on C++.
Sorry for not being such a help, this was just my (tiny) experience using OpenFOAM.


Joa

[tatadocomo]

I am also simulting rising bubble in interfoam. The mesh is very refined as of size D/40 where D is diameter of bubble. The p_rgh is taking 1000 iteration to converge which is slowing my simulation. Kindly suggest what to do

[Akimlav]

how to remove message?!

[Akimlav]

tatadocomo,
this helped me to reduce p_rgh iterations:

"rho.*"
{
solver PCG;
preconditioner DIC;
tolerance 1e-8;
relTol 0;
minIter 1;
}

p_rgh
{
solver PCG;
preconditioner
{

preconditioner GAMG;
tolerance 1e-08;
relTol 0;
nVcycles 2;
smoother DICGaussSeidel;
nPreSweeps 2;
nPostSweeps 2;
nFinestSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;

}
tolerance 1e-08;
relTol 0;
maxIter 50;
}

[vonboett]

for non-newtonian fluids I recommend in addition to use for "alpha.*" the smoothSolver with symGaussSeidel smoother and MulesCorr yes. No explanation why, just a standard i use to get good results. If the grid has some non-orthogonality I use some nNonOrthogonalCorrectors within PIMPLE, together with laplacianShemes Gauss linear limited 0.33 and ddtSchemes backward in fvSchemes...
Most instabilities I get are due to density gradients caused by different alpha values at the atmospheric boundary or at an inlet. I "survive" such moments by temporally switching from backward to Euler in such cases, combined with a local modification of alpha at these boundaries using setFields.

[GeekCFD]

Originally Posted by Akimlav

tatadocomo,
this helped me to reduce p_rgh iterations:

Hey Akimlav,
You are forcefully keeping the maximum number of iterations for p_rgh to be low (50). What was the 'final residual' after each time step for p_rgh in your case?
I want to know as I am also facing the same problem(~1000 iterations); and tried reducing the no. of iterations by assigning 'max_iter = 200', however the solution diverged. (final_residual was close to 1.)
In the end, I had to coarse the mesh which brought down the iterations to ~300 and also improved the final_residual value, but at the expense of the accuracy.

I think that using the vanLeer scheme for p_rgh can do the trick, but I have not checked it yet.
Hoping to hear from you!!

Regards,
GeekCFD