foamRun.C

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2022-2023 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.
 
    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.
 
    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.
 
    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.
 
Application
    foamRun
 
Description
    Loads and executes an OpenFOAM solver module either specified by the
    optional \c solver entry in the \c controlDict or as a command-line
    argument.
 
    Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
    pseudo-transient and steady simulations.
 
Usage
    \b foamRun [OPTION]
 
      - \par -solver <name>
        Solver name
 
      - \par -libs '(\"lib1.so\" ... \"libN.so\")'
        Specify the additional libraries loaded
 
    Example usage:
      - To run a \c rhoPimpleFoam case by specifying the solver on the
        command line:
        \verbatim
            foamRun -solver fluid
        \endverbatim
 
      - To update and run a \c rhoPimpleFoam case add the following entries to
        the controlDict:
        \verbatim
            application     foamRun;
 
            solver          fluid;
        \endverbatim
        then execute \c foamRun
 
\*---------------------------------------------------------------------------*/
 
#include "argList.H"
#include "solver.H"
#include "pimpleSingleRegionControl.H"
#include "setDeltaT.H"
 
using namespace Foam;
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
int main(int argc, char *argv[])
{
    argList::addOption
    (
        "solver",
        "name",
        "Solver name"
    );
 
    #include "setRootCase.H"
    #include "createTime.H"
 
    // Read the solverName from the optional solver entry in controlDict
    word solverName
    (
        runTime.controlDict().lookupOrDefault("solver", word::null)
    );
 
    // Optionally reset the solver name from the -solver command-line argument
    args.optionReadIfPresent("solver", solverName);
 
    // Check the solverName has been set
    if (solverName == word::null)
    {
        args.printUsage();
 
        FatalErrorIn(args.executable())
            << "solver not specified in the controlDict or on the command-line"
            << exit(FatalError);
    }
    else
    {
        // Load the solver library
        solver::load(solverName);
    }
 
    // Create the default single region mesh
    #include "createMesh.H"
 
    // Instantiate the selected solver
    autoPtr<solver> solverPtr(solver::New(solverName, mesh));
    solver& solver = solverPtr();
 
    // Create the outer PIMPLE loop and control structure
    pimpleSingleRegionControl pimple(solver.pimple);
 
    // Set the initial time-step
    setDeltaT(runTime, solver);
 
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
    Info<< nl << "Starting time loop\n" << endl;
 
    while (pimple.run(runTime))
    {
        solver.preSolve();
 
        // Adjust the time-step according to the solver maxDeltaT
        adjustDeltaT(runTime, solver);
 
        runTime++;
 
        Info<< "Time = " << runTime.userTimeName() << nl << endl;
 
        // PIMPLE corrector loop
        while (pimple.loop())
        {
            solver.moveMesh();
            solver.fvModels().correct();
            solver.prePredictor();
            solver.momentumPredictor();
            solver.thermophysicalPredictor();
            solver.pressureCorrector();
            solver.postCorrector();
        }
 
        solver.postSolve();
 
        runTime.write();
 
        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
            << nl << endl;
    }
 
    Info<< "End\n" << endl;
 
    return 0;
}
 
 
// ************************************************************************* //