[giovanni.medici]

Dear All,

I'm running a test case with sonicDyMFoam solver of supersonic external aerodynamics.
The simple test case is basically a coarse mesh of an half sphere in half (far-field cylinder). The mesh is unstructured tetra.

I slightly modify the solver to save grad(p) and then what I'm trying (unsucessfully) to achieve is mesh refinement when high pressure gradients are encountered (so to better capture shockwaves).

The "patched" solver compiled successfully, and saves, as expected, the PGrad variable.

I added a dynamicMeshDict file (below) in the constant/ folder, but when the case runs, in the log reports that no cell is currently selected to be refined/unrefined.

dynamicMeshDict:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



dynamicFvMesh dynamicRefineFvMesh;
   dynamicRefineFvMeshCoeffs
   {
       refineInterval 100;
       field PGrad;
       lowerRefineLevel   1e4;
       upperRefineLevel   1e6; 
       unrefineLevel 2;
       nBufferLayers 4;
       maxRefinement 4;
       maxCells 2000000;
       correctFluxes (( phi U ));
       dumpLevel true;
   }

Representative part of the log file:

Courant Number mean: 0.00366043 max: 0.273355
Time = 1e-05

Selected 0 cells for refinement out of 77833.
Selected 0 split points out of a possible 0.
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
rhoEqn max/min : 0.035079 0.00980862
PIMPLE: iteration 1
DILUPBiCGStab:  Solving for Ux, Initial residual = 5.45536e-05, Final residual = 2.39771e-11, No Iterations 2
DILUPBiCGStab:  Solving for Uy, Initial residual = 0.000384717, Final residual = 1.37344e-10, No Iterations 2
DILUPBiCGStab:  Solving for Uz, Initial residual = 0.0026547, Final residual = 5.29768e-10, No Iterations 2
DILUPBiCGStab:  Solving for e, Initial residual = 0.000205737, Final residual = 1.21308e-10, No Iterations 2
DILUPBiCGStab:  Solving for p, Initial residual = 0.000450696, Final residual = 6.1073e-14, No Iterations 3
DILUPBiCGStab:  Solving for p, Initial residual = 3.89561e-06, Final residual = 1.02284e-13, No Iterations 2
DILUPBiCGStab:  Solving for p, Initial residual = 1.06994e-06, Final residual = 3.20422e-14, No Iterations 2
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.0582e-15, global = 6.10016e-16, cumulative = 7.44534e-15
DILUPBiCGStab:  Solving for p, Initial residual = 6.35212e-07, Final residual = 2.41879e-14, No Iterations 2
DILUPBiCGStab:  Solving for p, Initial residual = 3.89155e-07, Final residual = 7.95415e-13, No Iterations 2
DILUPBiCGStab:  Solving for p, Initial residual = 2.84734e-07, Final residual = 6.14724e-13, No Iterations 2
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.23169e-15, global = 4.35367e-16, cumulative = 7.88071e-15
ExecutionTime = 1.58 s  ClockTime = 2 s

Is there any limitation to tetra meshes, or am I missing some relevant file in 0/ or system/ folders?

Sorry, it is probably quite straightforward, but I went through the openfoam wiki, obviously this great forum, but apparently I'm missing something, and can't figure it out...

I tried various combinations of parameters (lowerRefineLevel / upperRefineLevel) and also more conventional fields (p T), as well as serial and parallel runs, but none worked successfully.

Thanks, any help is appreciated.

I'm using openFOAMv1612.

[Tobi]

Hi,

the dynamicRefine library works with the hexRef8 library. As you can imagine, it is only possible for hexaeder. After starting the solver you should get a new file named protectedCells or something like that in the constant/polyMesh folder. There you will find the cells that are excluded from the refinement. In your particular case I guess all cells are inside. As far as I know, SimScale has a library which works for tetraeder meshes but out of the box I don't know a standard library in foam which handles that. At least not in the refinement library.

To solve it, you have to make your own library.

[giovanni.medici]

Thanks Tobi for the fast and comprehensive answer. Will definitely try with hexa mesh.


Sent from my iPhone using CFD Online Forum mobile app