MRFSimpleFoam

From OpenFOAMWiki
Revision as of 07:01, 31 March 2008 by Dmoroian (Talk | contribs)

1 MRFSimpleFoam

1.1 Introduction

This tutorial is aimed to generating the mesh in Gambit, importing and solving it with MRFSimpleFoam. It applies to OpenFoamVersion

1.2 Mesh Generation and Import

  1. generate two cylinders (r1=0.5 h1=1; r2=0.25, h2=0.5) and one cube (h3=0.3)
    Domain generation
  2. substract cylinder 2 from 1 (maintain cylinder 2)
  3. substract cube 3 from cylinder 2
  4. define continuum types (zones): rotor for cylinder 2, and stator for cylinder 1
    Rotor/Stator domain
  5. define boundaries (inlet, outlet, cubeWall, cylindricWall, sliderFace), and couple the interfaces (sliderFace)
    Boundaries
  6. define the coupled interface as INTERIOR
    Couple interfaces
  7. generate tetrahedral mesh (0.05 size)
    Mesh
  8. export as mrf.msh
  9. import mesh in OpenFoam:
 fluentMeshToFoam ./ simulation geom/mrf.msh -writeSets -writeZones

1.3 Solver Running

Before you start the solver, another modification is needed: change in all the dictionaries the patch cubeWall with rotor and cylindricWall with stator. Of course you could name this patches as it should from the beginning in Gambit, but I considered that in this way it will be clearer since the same name rotor appears in two places: zone and patch.

The rotational axis, and the angular velocity are specified using a dictionary file named constant/MRFZones.

The solver can be started as:

MRFSimpleFoam ./ simulation

It is advisable to start with very low angular velocities, even better to use potentialFoam as an initialization step. potentialFoam runs directly on the case withouth any other modifications.

In the case I ran, I started with potentialFoam, then I increased gradually the angular velocity from 0, 10, 20, 50, to 100 rad/s.

1.4 Postprocessing

Pressure distribution in a middle cross section is shown in the next figure:
Pressure distribution