• Copy tutorial test case mixerVessel2D:

  # run
  # cp -r $FOAM_TUTORIALS/multiphase/interFoam/laminar/\
  mixerVessel2D/ .
  # cd mixerVessel2D

• Test case is already preset

   

• Test case is set for solver interFoam

   

• Solver interFoam is unsteady solver based on PISO algorithm

   

• Solver interFoam solves motion of 2 incompressible, isothermal immiscible fluids using a VOF (volume of fluid) phase-fraction based interface capturing approach

   

• Computational mesh consists of blocks made in blockMesh application

   

• Mesh is set using makeMesh script:

  # cat makeMesh

   

#!/bin/sh

m4 < system/blockMeshDict.m4 > system/blockMeshDict
blockMesh
topoSet
setsToZones -noFlipMap

• Line 1: just stating that script is a bash type

   

• Line 3: using m4 (macro processor) define variable for blockMesh^14.1

   

• Line 4: run application blockMesh

   

• Line 5: create set of cells cellSet using utility topoSet. The cellSet is called rotor.

   

• In recent versions of the tutorial the fourth and fifth lines are redundant, as the cell zone is defined directly in the file blockMeshDict – note well the name rotor inserted into the definition of some hex-es. Mentioned lines thus actually convert a cell zone to cell set and back.

   

• Line 6: convert cellSet rotor to a cellZone (mesh part)

   

• Build the mesh:

  # ./makeMesh