Previous: Dynamic mesh refinement Up: Dynamic mesh refinement Next: Combination of dynamic and
This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.
Test case: damBreakWithObstacle
- Local mesh refinement tutorial
- Copy tutorial test case damBreakWithObstacle:
# cd $FOAM_RUN
# cp -r $FOAM_TUTORIALS/\
/multiphase/interFoam/laminar/damBreakWithObstacle ./ - Test case is already set up
- Three-dimensional flow of two fluids
- A simple model of dam break. A water column is released in the box with obstacle.
Figure: damBreakWithObstacle geometry
dynamicFvMesh dynamicRefineFvMesh;
dynamicRefineFvMeshCoeffs
{
// How often to refine
refineInterval 1;
// Field to be refinement on
field alpha.water;
// Refine field inbetween lower..upper
lowerRefineLevel 0.001;
upperRefineLevel 0.999;
// 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)
(alphaPhi none)
(ghf none)
);
// Write the refinement level as a volScalarField
dumpLevel true;
}
- Run test case:
# ./Allrun
# paraFoam 9.2
Figure: Mesh refinement/unrefinement, side view
Figure: Phase magnitude in different times
Previous: Dynamic mesh refinement Up: Dynamic mesh refinement Next: Combination of dynamic and