CFD Online Discussion Forums - GAMG hexa vs. tetrahedron meshes

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

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - GAMG hexa vs. tetrahedron meshes (https://www.cfd-online.com/Forums/openfoam/78273-gamg-hexa-vs-tetrahedron-meshes.html)

GAMG hexa vs. tetrahedron meshes

Hello Foamers!

Has anybody experience to set up GAMG for hexa or tetraeder? On tet, Do I have to increase, for instance, smoother iteration or merge levels?

Cheers in advance

Hi Claus,

in my opinion it doesn't matter for GAMG if you are using hexas or tetras. A good choice of settings for my projects is:

Code:

solvers

{

    U                                   // linear equation system solver for U

    {

        solver          smoothSolver;   // solver type

        smoother        GaussSeidel;    // smoother type

        tolerance       1e-06;          // solver finishes if either absolute

        relTol          0.01;           // tolerance is reached or the relative

                                        // tolerance here

        nSweeps         1;              // setting for smoothSolver

        maxIter         100;            // limitation of iterations number

    }

    pd                                  // linear equation system solver for pd

    {

        solver          GAMG;           // very efficient multigrid solver

        tolerance       1e-07;          // solver finishes if either absolute

        relTol          0.001;          // tolerance is reached or the relative

                                        // tolerance here

        minIter         3;              // a minimum number of iterations

        maxIter         100;            // limitation of iterions number

        smoother        DIC;            // setting for GAMG

        nPreSweeps      1;              // 1 for pd, set to 0 for all other!

        nPostSweeps     2;              // 2 is fine

        nFinestSweeps   2;              // 2 is fine

        scaleCorrection true;           // true is fine

        directSolveCoarsestLevel false; // false is fine

        cacheAgglomeration on;          // on is fine; set to off, if dynamic

                                        // mesh refinement is used!

        nCellsInCoarsestLevel 500;      // 500 is fine,

                                        // otherwise sqrt(number of cells)

        agglomerator    faceAreaPair;   // faceAreaPair is fine

        mergeLevels     1;              // 1 is fine

    }

}

Important to note:
- nPreSweeps must be 0 for other equation systems than pressure
- to use the minIter option you must patch GAMG sources in most OpenFOAM versions
- cacheAgglomeration must be switched off when using dynamic mesh refinement

Playing with the options don't give remarkable speedup for my problems.

Martin

Thanks MartinB, the informations are valueable for me! However, there is one question concernins the option nCellsInCorseLeve: Why the sqrt of the cells? Have you an paper or something like that?

Cheers

Hi Claus,
I found the hint for sqrt(#cells) in the forum some time ago and made a note in my fvSolution template without paying too much attention to it...

This might be an interesting thread (especially the links to the PDFs), if you want to use some variants of AMG:
http://www.cfd-online.com/Forums/ope...41dev-svn.html
However it could be some work to integrate these solvers and preconditioners in the newer OpenFOAM versions.

Martin

Do you probaly mean: If I have n processors then I have to take (total no. cells)^(1/n)?

I mean: sqrt(1000000) = 1000
But: I never tested it in more detail... my value of 500 was fine, changing it had no big influence on my computation speed.
You can test it out: start your simulation, change the value after a few iterations and check the new iteration times. Then make another change and check again...

Many other posts in the forum prefer values of 10 to 30 for nCellsInCoarsestLevel...
http://www.cfd-online.com/OpenFOAM_D...tml?1162930507

Martin

FYI: For future reference, the link on the previous post is for the following thread in the new forum format: http://www.cfd-online.com/Forums/ope...rsus-iccg.html

Hi,

Thank you for your assistance. I am wondering: where do these values stem from? Specifically, why does nPreSweeps need to be 1 for pd?

-Mimi

Quick answer: I can never remember off-hand which equations have a symmetric A matrix and which ones have an asymmetric A matrix... but the "nPreSweeps" has to be set to 1 probably because the "pd" (pressure) equation is the opposite type of symmetry from the other equations.

Thanks for responding. I have an easier simpler question. What encompasses one iteration? In the log file, I'll get something like "GAMG: Solving for pd, Initial residual = 3.833447548e-13, Final residual = 3.908110229e-15, No Iterations 2."

What are the two iterations? Is that one V cycle? multiple V cycles? I can't seem to find a good answer anywhere.

-Mimi

Quick answer: I don't know what a V-cycle technically is, but the number of iterations is how many iterations it does to try and solve the "A*x=b" equation.
It (usually) does not include how many intermediate passes it does within the matrix solver, e.g. pre/post-sweeps are not accounted by the number of iterations.

In foam-extend, you can find:

the GAMG solver code in the folder "$FOAM_SRC/foam/matrices/lduMatrix/solvers/AMG";
the GAMG preconditioner at "$FOAM_SRC/foam/matrices/lduMatrix/preconditioners/GAMGPreconditioner".

As a quick reference, the number of iterations increments can be seen in this do-while cycle: $FOAM_SC/foam/matrices/lduMatrix/solvers/AMG/GAMGSolverSolve.C starting line 82 and in line 103 is where the number of iterations increases.

Thanks for your help! So it looks like one iteration IS one V-cycle. The V Cycle goes from fine to coarse and then fine again.