[CloudBird]

Hello，everyone！ Recently， I am working on a jet simulation based on interFoam and I used adaptive mesh to refine the region near the interface. My geometry is an axisymmetric configuration with wedge boundary condition(see Fig1). During the simulation process, I found that the mesh near the symmetry axis whose boundary condition is empty didn't get refined(see Fig2). Fig 3 is the cellLevel field generated by the adaptive mesh code and you can see that the region near the symmetry axis is not in the refined area.

Fig.1 the geometry of my cases

Fig.2 the refined mesh near the interface

Fig.3 the cellLevel near the interface

This is my dynamicMeshDict:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dynamicFvMesh   dynamicRefineFvMesh;

// How often to refine
refineInterval  1;

// Field to be refinement on
field           alpha.liquid;

// Refine field in between lower..upper
lowerRefineLevel 0.01;
upperRefineLevel 0.99;

// If value < unrefineLevel unrefine
unrefineLevel   10;

// Have slower than 2:1 refinement
nBufferLayers   1;

// Refine cells only up to maxRefinement levels
maxRefinement   2;

// Stop refinement if maxCells reached
maxCells        200000;

// 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 none)
  (nHatf none)
  (rhoPhi none)
  (alphaPhi0.liquid none)
  (ghf none)
);

// Write the refinement level as a volScalarField
dumpLevel       true;


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

In my opinion, this error may related to the empty boundary condition which I apply to the axis. But I don't have any idea how to fix it.

I hope someone can help me out and any suggestion is welcome. Thanks in advance!

Kind regards,
CloudBird

[guin]

I wouldn't expect it to refine there. Adaptive mesh refinement in OF relies on the assumption of hexahedral elements. Wedges are not hexahedra, thus they are left unchanged...

[hjasak]

First, you can get rid of the pole patch either by removing it by hand if there are no faces or by collapsing the points first.

Second foam-extend actually provides adaptivity on polyhedral cells so the problem goes away.

Hrv

[CloudBird]

Originally Posted by guin

I wouldn't expect it to refine there. Adaptive mesh refinement in OF relies on the assumption of hexahedral elements. Wedges are not hexahedra, thus they are left unchanged...

Thank you~ I will try to give a tiny thickness in the axis and have a try (^-^)

[CloudBird]

Originally Posted by hjasak

First, you can get rid of the pole patch either by removing it by hand if there are no faces or by collapsing the points first.

Second foam-extend actually provides adaptivity on polyhedral cells so the problem goes away.

Hrv

Thank you, sir. I will try for the extend version