porousBafflePressureFvPatchField.C

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | www.openfoam.com
     \\/     M anipulation  |
-------------------------------------------------------------------------------
    Copyright (C) 2011-2016 OpenFOAM Foundation
    Copyright (C) 2020 OpenCFD Ltd.
-------------------------------------------------------------------------------
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/>.
 
\*---------------------------------------------------------------------------*/
 
#include "porousBafflePressureFvPatchField.H"
#include "surfaceFields.H"
#include "turbulenceModel.H"
#include "addToRunTimeSelectionTable.H"
 
// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
 
Foam::porousBafflePressureFvPatchField::porousBafflePressureFvPatchField
(
    const fvPatch& p,
    const DimensionedField<scalar, volMesh>& iF
)
:
    fixedJumpFvPatchField<scalar>(p, iF),
    phiName_("phi"),
    rhoName_("rho"),
    D_(),
    I_(),
    length_(0),
    uniformJump_(false)
{}
 
 
Foam::porousBafflePressureFvPatchField::porousBafflePressureFvPatchField
(
    const fvPatch& p,
    const DimensionedField<scalar, volMesh>& iF,
    const dictionary& dict
)
:
    fixedJumpFvPatchField<scalar>(p, iF),
    phiName_(dict.getOrDefault<word>("phi", "phi")),
    rhoName_(dict.getOrDefault<word>("rho", "rho")),
    D_(Function1<scalar>::New("D", dict)),
    I_(Function1<scalar>::New("I", dict)),
    length_(dict.get<scalar>("length")),
    uniformJump_(dict.getOrDefault("uniformJump", false))
{
    fvPatchField<scalar>::operator=
    (
        Field<scalar>("value", dict, p.size())
    );
}
 
 
Foam::porousBafflePressureFvPatchField::porousBafflePressureFvPatchField
(
    const porousBafflePressureFvPatchField& ptf,
    const fvPatch& p,
    const DimensionedField<scalar, volMesh>& iF,
    const fvPatchFieldMapper& mapper
)
:
    fixedJumpFvPatchField<scalar>(ptf, p, iF, mapper),
    phiName_(ptf.phiName_),
    rhoName_(ptf.rhoName_),
    D_(ptf.D_.clone()),
    I_(ptf.I_.clone()),
    length_(ptf.length_),
    uniformJump_(ptf.uniformJump_)
{}
 
 
Foam::porousBafflePressureFvPatchField::porousBafflePressureFvPatchField
(
    const porousBafflePressureFvPatchField& ptf
)
:
    cyclicLduInterfaceField(),
    fixedJumpFvPatchField<scalar>(ptf),
    phiName_(ptf.phiName_),
    rhoName_(ptf.rhoName_),
    D_(ptf.D_.clone()),
    I_(ptf.I_.clone()),
    length_(ptf.length_),
    uniformJump_(ptf.uniformJump_)
{}
 
 
Foam::porousBafflePressureFvPatchField::porousBafflePressureFvPatchField
(
    const porousBafflePressureFvPatchField& ptf,
    const DimensionedField<scalar, volMesh>& iF
)
:
    fixedJumpFvPatchField<scalar>(ptf, iF),
    phiName_(ptf.phiName_),
    rhoName_(ptf.rhoName_),
    D_(ptf.D_.clone()),
    I_(ptf.I_.clone()),
    length_(ptf.length_),
    uniformJump_(ptf.uniformJump_)
{}
 
 
// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
 
void Foam::porousBafflePressureFvPatchField::updateCoeffs()
{
    if (updated())
    {
        return;
    }
 
    const surfaceScalarField& phi =
            db().lookupObject<surfaceScalarField>(phiName_);
 
    const fvsPatchField<scalar>& phip =
        patch().patchField<surfaceScalarField, scalar>(phi);
 
    scalarField Un(phip/patch().magSf());
 
    if (phi.dimensions() == dimMass/dimTime)
    {
        Un /= patch().lookupPatchField<volScalarField, scalar>(rhoName_);
    }
 
    if (uniformJump_)
    {
        Un = gAverage(Un);
    }
    scalarField magUn(mag(Un));
 
    const turbulenceModel& turbModel = db().lookupObject<turbulenceModel>
    (
        IOobject::groupName
        (
            turbulenceModel::propertiesName,
            internalField().group()
        )
    );
 
    const scalar t = db().time().timeOutputValue();
    const scalar D = D_->value(t);
    const scalar I = I_->value(t);
 
    jump_ =
        -sign(Un)
        *(
            D*turbModel.nu(patch().index())
          + I*0.5*magUn
         )*magUn*length_;
 
    if (internalField().dimensions() == dimPressure)
    {
        jump_ *= patch().lookupPatchField<volScalarField, scalar>(rhoName_);
    }
 
    if (debug)
    {
        scalar avePressureJump = gAverage(jump_);
        scalar aveVelocity = gAverage(Un);
 
        Info<< patch().boundaryMesh().mesh().name() << ':'
            << patch().name() << ':'
            << " Average pressure drop :" << avePressureJump
            << " Average velocity :" << aveVelocity
            << endl;
    }
 
    fixedJumpFvPatchField<scalar>::updateCoeffs();
}
 
 
void Foam::porousBafflePressureFvPatchField::write(Ostream& os) const
{
    fixedJumpFvPatchField<scalar>::write(os);
    os.writeEntryIfDifferent<word>("phi", "phi", phiName_);
    os.writeEntryIfDifferent<word>("rho", "rho", rhoName_);
    D_->writeData(os);
    I_->writeData(os);
    os.writeEntry("length", length_);
    os.writeEntry("uniformJump", uniformJump_);
}
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
    makePatchTypeField
    (
        fvPatchScalarField,
        porousBafflePressureFvPatchField
    );
}
 
// ************************************************************************* //