Use on OpenFOAM

Export UNV file Mesh_1 and copy in /hgasca/OpenFOAM/run/case/

ideasUnvToFoam Mesh_1.unv
checkMesh

Go to /case/constant/polyMesh and open bondary file:

 /*--------------------------------*- C++ -*----------------------------------*\
   =========                 |
   \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
    \\    /   O peration     | Website:  https://openfoam.org
     \\  /    A nd           | Version:  7
      \\/     M anipulation  |
 \*---------------------------------------------------------------------------*/
 FoamFile
 {
     version     2.0;
     format      binary;
     class       polyBoundaryMesh;
     location    "1e-05/polyMesh";
     object      boundary;
 }
 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

 9
 (
  frontAndBack_pos
  {
      type            wedge;
      inGroups        List<word> 1(wedge);
      nFaces          76728;
      startFace       151207;
  }
  inlet
  {
      type            patch;
      nFaces          61;
      startFace       227935;
  }
  wall
  {
      type            wall;
      inGroups        List<word> 1(wall);
      nFaces          1559;
      startFace       227996;
  }
  positive_pres
  {
      type            wall;
      inGroups        List<word> 1(wall);
      nFaces          58;
      startFace       229555;
  }
  negative_pres
  {
      type            wall;
      inGroups        List<word> 1(wall);
      nFaces          55;
      startFace       229613;
  }
  moving_wall
  {
      type            wall;
      inGroups        List<word> 1(wall);
      nFaces          1200;
      startFace       229668;
  }
  outlet
  {
      type            patch;
      nFaces          55;
      startFace       230868;
  }

  Axis
  {
      type            patch;
      nFaces          2154;
      startFace       2400868;
  }

  frontAndBack_neg
  {
      type            wedge;
      inGroups        List<word> 1(wedge);
      nFaces          76728;
      startFace       230923;
  }
)

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

The kind of boundaries are as appear before

In the next Step collapseEdges the Axis boundary could be reduced and it will appear with zero nFaces, you must delete this boundary in the new time generated folder i.e 5e-06/polyMesh and to change the number of boundaries from 9 to 8 for this case

collapseEdges

it creates a new time i.e case/5e-06. Then replace /constant/polyMesh Mesh by new_time/polyMesh mesh and review names of boundaries. Copy the case/0 files into the new_time folder.

openFoam Flies

Files Folder 5e-06

constant folder

Pay special attention to transportProperties

system folder

Here there are important files: - collapseDict is necessary to run the collapseDict command. - decomposeParDict sets the parallel running decomposition. - setFieldsDict sets the phases into the geometry as an initial conditions. The subsecuent time steps must maintain the phase equilibrium in other way the run could diverge.

The last three must be generated by:

foamGet streamlines
foamGet probes
foamGet residuals

Ann edit to customize the parameters. Then in controlDict append:

functions
{
    #includeFunc streamlines
    #includeFunc  residuals
    #includeFunc  probes.cfg
}

The results of them will be find in the case/postProcessinf folder

Actions

checkMesh

If errors review your mesh know use the solver pimpleFOAM with one or more processors

decomposePar

checkMesh

renumberMesh

Then in the case folder create a file called hostfile with this content:

localhost slots=8

The number of slots corresponds to the procesors to be use. Run the parallel processes with:

mpirun -hostfile hostfile -np 8 pimpleFoam -parallel >log

or

mpirun.openmpi -hostfile hostfile -np 8 pimpleFoam -parallel >log

Depending on your system configuration.

And finally you could review the convergence by:

foamMonitor -logscale ./postProcessing/residuals/5e-06/residuals.dat