[mb.pejvak]

I am using interDyMFoam as a solve and I want to have dynamic mesh rifinement based on velocity. The dynamicMeshDict is as follows:

 



/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dynamicFvMesh   dynamicRefineFvMesh;

dynamicRefineFvMeshCoeffs
{
    // How often to refine
    refineInterval  1;
    // Field to be refinement on
    field U;
    // Refine field between lower..upper
    lowerRefineLevel 0.0
    upperRefineLevel 0.001;
    // If value < unrefineLevel unrefine
    unrefineLevel   0.1;
    // Have slower than 2:1 refinement
    nBufferLayers   24;
    // Refine cells only up to maxRefinement levels
    maxRefinement   2;
    // Stop refinement if maxCells reached
    maxCells        100000000;

    // Stop autorefinement after n timesteps
    maxTimeAutoRefine   -1;

    // Flux field and corresponding velocity field. Fluxes on changed
    // faces get recalculated by interpolating the velocity. Use 'none'
    // on surfaceScalarFields that do not need to be reinterpolated.
    correctFluxes
    (
        (phi_0 U)
        (phi U)
    );
    // Write the refinement level as a volScalarField
    dumpLevel       false;
}


// ************************************************************************* //

But when I run the case I got the error

  it is not a volScalarField, it is a volVectorField

[LuckyTran]

The error says it all... U is a velocity field. Refinement is based on a yes/no criteria (more specifically, a scalar field with values between lowerRefineLevel and upperRefineLevel)... Supply a scalar field (i.e. one of the components of velocity or the velocity magnitude).

[mb.pejvak]

Thanks for your help. This is the primary question, what is the key word for velocity magnitude in openfoam. I mean

 mag(U)

or

 U.magnitude()

work or I have to do some coding

[LuckyTran]

You do have to do some coding. Velocity magnitude is (usually) not a registered field available at runtime.

If you tried it anyway right now, you'd probably get the error that it cannot find the field mag(U). I don't know exactly how you're using your solver and how often the mesh needs updating to actually present you the solution but..
there is a library of field function objects (one of them is mag) that can calculate the magnitude at runtime and write it into a volScalarField. You put this into your control dict.


If you don't need to refine the mesh during runtime, you could get away with just using the postProcess utility. But I can imagine nobody using a dynamic mesh is doing refinement this way.