[aki_yafuji]

Hi to everyone!
I am Aki, a beginner in OpenFOAM.

I am intrested in adaptive mesh refinement and I managed to find
"dynamicMeshDict" dictionary, but I am not sure how it works...
Would you tell me a condition of the refinement? The mesh is refined
automatically when the velocity (or the Courant number) exceeds a given value?

And, I am not sure coefficients in the dictionary...

constant/dynamicMeshDict
--------------------------------------
dynamicFvMesh dynamicRefineFvMesh;

dynamicRefineFvMeshCoeffs
{
refineInterval 1;
field alpha1;
lowerRefineLevel 0.001;
upperRefineLevel 0.999;
unrefineLevel 10;
nBufferLayers 1;
maxRefinement 2;
maxCells 200000;
correctFluxes
(
(
phi
U
)
);
dumpLevel true;
}
--------------------------------------

I have performed some tutorials, so I guess "maxRefinement" means the max
refinement number. But I cound only understand it. I can not understand
what "refineInterval" and "maxCells" mean. And what are "lowerRefineLevel"
and "upperRefineLevel"...?
I would be grateful if you could provide me the meanings of them.

Thanks in advance!

Aki

[KrisT]

As far as I understand:

refineInterval - specifies how often (every n:th timestep) the grid should be refined.

maxCells - limits the number of cells, should never be greater than the given number, an approximate number.

lowerRefineLevel - grid gets refined if "alpha1" is lower than this value.

upperRefineLevel - grid gets refined if "alpha1" is bigger than this value.

[aki_yafuji]

Dear KrisT

Thank you very much for your help!
I have performed some tutorials by changing them.
May I ask one more question???
What is "correctFluxes" ? These values are corrected each time step?

Aki

[KrisT]

Originally Posted by aki_yafuji

Dear KrisT

Thank you very much for your help!
I have performed some tutorials by changing them.
May I ask one more question???
What is "correctFluxes" ? These values are corrected each time step?

Aki

Not sure about this one. Something about fluxes to correct when refining (phi), and variable they can be ineterpolated from (U).

[idefix]

Hello,

I looked into the code and find following:
nBufferLayer: Number of layers between different refinement levels
I understand it in that way: nBufferLayer 1 means:
a cell, which was refined once, can only be a neighbour of a cell which is not refined or refined twice. But this cell can´t be a neighbour of a cell which is refined three times.

In a tutorial I found the definitoin for maxRefinement:
maxRefinement means the number of refinements that are allowed for one cell.

But does everybody know what "unrefineLevel" mean?

Thanks a lot

[idefix]

has nobody an idea what it could mean?

I would be really happy to get some help

[potentialFoam]

Dear Foamers,

I have another question concerning the settings in the dynamicMeshDict-file. I would like to refine a tip vortex dynamically, so with the pimpleDyMFoam-solver.

As entry 'field' in dynamicMeshDict I would like to use something like Lambda2.
How can I tell the solver to calc this field?

[potentialFoam]

Finally, I programmed a new solver based on pimpleDyMFoam. There, I calculated the nedded scalar field (like Lambda2). In constant/dynamicMeshDict I specify the variables that prescribe the refinement and so it works

[afrotimy]

Originally Posted by potentialFoam

Finally, I programmed a new solver based on pimpleDyMFoam. There, I calculated the nedded scalar field (like Lambda2). In constant/dynamicMeshDict I specify the variables that prescribe the refinement and so it works

Hi Peter,

Is this new solver working with dynamicRefineFvMesh in 2D ?

[potentialFoam]

Hi Francis,

what do you mean with 'dynamicRefineFvMesh'? I didn't try but I think it should work in 2D - why not?

Regards,
Peter

[opencfd]

The dynamic refinement is cutting cells 2x2x2 - in all directions, so you would create mesh cells in directions you are not solving for. Which would be not such a problem, but you are creating also non-orthogonality and you will have parasitic fluxes in the direction you are not solving for and your solution is loosing precision at least.

[potentialFoam]

Thanks! That's correct. So it works, but not in the desired way.

[kk415]

Hi Everyone,


Isn't there any way to control the division of cells in 2D ? or Isn't there any way to make the division orthogonal always ?

[K.C.]

Does it mean, that the actual implementation of dynamicMeshRefinement can only deal with hexahedra cells?
That would mean it is useless if I have tetrahedras in my mesh?