1

Previous: Relaxation of the computation Up: Test case: motorBike Next: Gnuplot – convergence monitoring

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

  • Test case is preset

     

  • Copy the initial conditions in 0.orig/ to 0/ :

    # cp -r 0.orig/* 0

  • Run in parallel
  • In file system/decomposeParDict set number of regions e.g. to 2. You have to update the hierarchicalCoeffs so as their product gives desired number of subdomains.
  • Decomposition method hierarchical

     

    /*--------------------------------*- 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;
        object      decomposeParDict;
    }
    
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
    
    numberOfSubdomains 2;
    
    method          hierarchical;
    // method          ptscotch;
    
    simpleCoeffs
    {
        n               (4 1 1);
        delta           0.001;
    }
    
    hierarchicalCoeffs
    {
        n               (2 1 1);
        delta           0.001;
        order           xyz;
    }
    
    manualCoeffs
    {
        dataFile        "cellDecomposition";
    }
    

  • Mesh is split:
    # decomposePar
  • If your simulation crashes or diverges in the early stage of computation, it can be caused by a rough intial guess. Therefore the potentialFoam is a good tool to initialize the computation
  • Generate starting fields by potentialFoam run in parallel
    # mpiexec -np 2 potentialFoam -noFunctionObjects -parallel
  • Option -noFunctionObjects switch off executing of functions defined in controlDict
  • Run computation in parallel on background forwarding output to file log.simpleFoam
    # mpiexec -np 2 simpleFoam -parallel > log.simpleFoam &
  • Parameter -np 2 means number of processes and must correspond with numberOfSubdomains in system/decomposeParDict
  • Use reconstructPar utility and view results in paraview

    # reconstructPar

    # paraFoam 7.4

openfoam tutorial motor bike pressure velocity

Figure: OpenFOAM tutorial motorbike. Pressure and velocity fields view

  • This test case can be run using Allrun script
  • Basically, the script contains the steps described in this Section