Previous: Test case description Up: Test case: mixerVessel Next: Test case: Multiphase Mixer
This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.
Test case set-up
- Computational mesh set up can be found in file system/blockMeshDict.m4
- File .m4 is a Linux macroprocessor script creating file blockMeshDict
- Application blockMesh can be run using script makeMesh
- Go to directory mixerVessel2D and run the script makeMesh:
# ./makeMesh - MRF properties are set in file MRFProperties in directory constant:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: dev | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object MRFProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // MRF1 { cellZone rotor; active yes; // Fixed patches (by default they 'move' with the MRF zone) nonRotatingPatches (); origin (0 0 0); axis (0 0 1); omega 104.72; } // ************************************************************************* // - Area, in which MRF takes effect is defined via cellZone. The cell zone name is rotor and it was created automatically with the mesh.
- Parameter origin stands for coordinates of a point on the axis of rotation.
- Parameter axis is the direction vector (x,y,z) of the axis of rotation.
- Parameter omega stands for angular velocity [rad/s]
- The turbulence set-up can be found in the file turbulenceProperties in directory constant:
simulationType RAS; RAS { RASModel kEpsilon; turbulence on; printCoeffs on; } - Turbulence model we use is
- Alternatives are e.g.:
LRR
LamBremhorstKE
LaunderGibsonRSTM
LaunderSharmaKE
LienCubicKE
LienCubicKELowRe
LienLeschzinerLowRe
NonlinearKEShih
RNGkEpsilonSpalartAllmaras
kEpsilon
kOmega
kOmegaSST
kkLOmega
laminar
qZeta
realizableKE
v2f - In file constant/transportProperties the kinematic viscosity nu is set up:
transportModel Newtonian; nu [ 0 2 -1 0 0 0 0 ] 1e-05;
- transportModel set to Newtonian means Newtonian fluid flow (viscosity is constant).
- If we want a shorter write interval, we can set this in the computation configuration file system/controlDict :
endTime 500; deltaT 1; writeControl timeStep; writeInterval 50;
- Run the computation:
# simpleFoam > log &
- Results can be viewed in paraview:
# paraFoam
Figure: Velocity magnitude, pressure distribution
Previous: Test case description Up: Test case: mixerVessel Next: Test case: Multiphase Mixer