OpenFOAM – adaptativeSimpleFoam

Dans cet article, nous proposons un solveur qui s’appuie sur l’estimateur d’erreur décrit dans ce billet.

L’idée est de proposer un solveur de type SIMPLE qui, a chaque pas de temps, calcule un estimateur d’erreur et raffine ou dé-raffine le maillage selon l’importance de l’erreur liée à la discrétisation.

  • files
adaptativeSimpleFoam.C

EXE = $(FOAM_APPBIN)/adaptativeSimpleFoam
  • options
EXE_INC = \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/incompressible/lnInclude \
    -I$(FOAM_DEV)/ressources/errorEstimation/lnInclude \
    -I$(LIB_SRC)/transportModels \
    -I$(LIB_SRC)/transportModels/incompressible/singlePhaseTransportModel \
    -I$(LIB_SRC)/dynamicFvMesh/lnInclude \
    -I$(LIB_SRC)/dynamicMesh/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \
    -I$(LIB_SRC)/sampling/lnInclude \
    -fpermissive
    

EXE_LIBS = \
    -lturbulenceModels \
    -lerrorEstimation \
    -lincompressibleTurbulenceModels \
    -lincompressibleTransportModels \
    -ldynamicFvMesh \
    -ltopoChangerFvMesh \
    -ldynamicMesh \
    -lfiniteVolume \
    -lmeshTools \
    -lfvOptions \
    -lsampling
  • createFields.H
/*
 * createFileds.h
 * 
 * Copyright 2018 arep <arep@debian01>
 * 
 * This program 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 2 of the License, or
 * (at your option) any later version.
 * 
 * This program 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 this program; if not, write to the Free Software
 * Foundation, Inc., 51 Franklin Street, Fifth Floor, Boston,
 * MA 02110-1301, USA.
 * 
 * 
 */

Info<< "Reading field p\n" << endl;
volScalarField p
(
    IOobject
    (
        "p",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

Info<< "Reading field U\n" << endl;
volVectorField U
(
    IOobject
    (
        "U",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

Info<< "Reading transportProperties\n" << endl;

IOdictionary transportProperties
(
    IOobject
    (
        "transportProperties",
        runTime.constant(),
        mesh,
        IOobject::MUST_READ_IF_MODIFIED,
        IOobject::NO_WRITE
    )
);

dimensionedScalar nu
(
    "nu",
    dimViscosity,
    transportProperties.lookup("nu")
);


Info<< "Creating field error\n" << endl;
volScalarField error
(
    IOobject
    (
        "error",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    mesh,
    dimensionedScalar("error", dimensionSet(0,1,-1,0,0,0,0), Foam::scalar(0))
);

#include "createPhi.H"


label pRefCell = 0;
scalar pRefValue = 0.0;
setRefCell(p, simple.dict(), pRefCell, pRefValue);
mesh.setFluxRequired(p.name());


singlePhaseTransportModel laminarTransport(U, phi);

autoPtr<incompressible::turbulenceModel> turbulence
(
    incompressible::turbulenceModel::New(U, phi, laminarTransport)
);

#include "createMRF.H"<br>
  • UEqn.H
    // Momentum predictor

    MRF.correctBoundaryVelocity(U);

    tmp<fvVectorMatrix> tUEqn
    (
        fvm::div(phi, U)
      + MRF.DDt(U)
      + turbulence->divDevReff(U)
     ==
        fvOptions(U)
    );
    fvVectorMatrix& UEqn = tUEqn.ref();

    UEqn.relax();

    fvOptions.constrain(UEqn);

    if (simple.momentumPredictor())
    {
        solve(UEqn == -fvc::grad(p));

        fvOptions.correct(U);
    }
  • pEqn.H
{
    volScalarField rAU(1.0/UEqn.A());
    volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p));
    surfaceScalarField phiHbyA("phiHbyA", fvc::flux(HbyA));
    MRF.makeRelative(phiHbyA);
    adjustPhi(phiHbyA, U, p);

    tmp<volScalarField> rAtU(rAU);

    if (simple.consistent())
    {
        rAtU = 1.0/(1.0/rAU - UEqn.H1());
        phiHbyA +=
            fvc::interpolate(rAtU() - rAU)*fvc::snGrad(p)*mesh.magSf();
        HbyA -= (rAU - rAtU())*fvc::grad(p);
    }

    tUEqn.clear();

    // Update the pressure BCs to ensure flux consistency
    constrainPressure(p, U, phiHbyA, rAtU(), MRF);

    // Non-orthogonal pressure corrector loop
    while (simple.correctNonOrthogonal())
    {
        fvScalarMatrix pEqn
        (
            fvm::laplacian(rAtU(), p) == fvc::div(phiHbyA)
        );

        pEqn.setReference(pRefCell, pRefValue);

        pEqn.solve();

        if (simple.finalNonOrthogonalIter())
        {
            phi = phiHbyA - pEqn.flux();
        }
    }

    #include "continuityErrs.H"

    // Explicitly relax pressure for momentum corrector
    p.relax();

    // Momentum corrector
    U = HbyA - rAtU()*fvc::grad(p);
    U.correctBoundaryConditions();
    fvOptions.correct(U);
}
  • eEqn.H
/*
 * eEqn
 * 
 * Copyright 2018 arep <arep@debian01>
 * 
 * This program 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 2 of the License, or
 * (at your option) any later version.
 * 
 * This program 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 this program; if not, write to the Free Software
 * Foundation, Inc., 51 Franklin Street, Fifth Floor, Boston,
 * MA 02110-1301, USA.
 * 
 * 
 */
            errorEstimate<vector> eEqn
            (
                resError::div(phi, U)
              - resError::laplacian(nu, U)
             ==
               -fvc::grad(p)
            );

	    error=mag(eEqn.error());

  • adaptativeSimpleFoam.C
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2016 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
 * Copyright 2018 arep <arep@debian01>
 * 
 * This program 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 2 of the License, or
 * (at your option) any later version.
 * 
 * This program 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 this program; if not, write to the Free Software
 * Foundation, Inc., 51 Franklin Street, Fifth Floor, Boston,
 * MA 02110-1301, USA.

Application
    adaptativeSimpleFoam

Description
    Steady-state solver for incompressible, turbulent flow with remeshing capabilities
    using the SIMPLE algorithm.

\*---------------------------------------------------------------------------*/

#include "fvCFD.H"
#include "dynamicFvMesh.H"
#include "singlePhaseTransportModel.H"
#include "turbulentTransportModel.H"
#include "simpleControl.H"
#include "fvOptions.H"
#include "errorEstimate.H"
#include "resError.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argc, char *argv[])
{
    #include "postProcess.H"

    #include "setRootCase.H"
    #include "createTime.H"
    #include "createDynamicFvMesh.H"
    #include "createControl.H"
    #include "createFields.H"
    #include "createFvOptions.H"
    #include "initContinuityErrs.H"

    turbulence->validate();

    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //





   // Calculate absolute flux from the mapped surface velocity
   //phi = mesh.Sf() & Uf;

    while (simple.loop())
    {


        Info<< "Time = " << runTime.timeName() << nl << endl;

	mesh.update();

        // --- Pressure-velocity SIMPLE corrector
        {
            #include "UEqn.H"
            #include "pEqn.H"
	    #include "eEqn.H"
        }

        laminarTransport.correct();
        turbulence->correct();


        runTime.write();

        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
            << nl << endl;
    }

    Info<< "End\n" << endl;

    return 0;
}


// ************************************************************************* //