uniformTotalPressureFvPatchScalarField.C

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2015 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/>.
 
\*---------------------------------------------------------------------------*/
 
#include "uniformTotalPressureFvPatchScalarField.H"
#include "addToRunTimeSelectionTable.H"
#include "fvPatchFieldMapper.H"
#include "volFields.H"
#include "surfaceFields.H"
 
// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
 
Foam::uniformTotalPressureFvPatchScalarField::
uniformTotalPressureFvPatchScalarField
(
    const fvPatch& p,
    const DimensionedField<scalar, volMesh>& iF
)
:
    fixedValueFvPatchScalarField(p, iF),
    UName_("U"),
    phiName_("phi"),
    rhoName_("none"),
    psiName_("none"),
    gamma_(0.0),
    pressure_()
{}
 
 
Foam::uniformTotalPressureFvPatchScalarField::
uniformTotalPressureFvPatchScalarField
(
    const fvPatch& p,
    const DimensionedField<scalar, volMesh>& iF,
    const dictionary& dict
)
:
    fixedValueFvPatchScalarField(p, iF),
    UName_(dict.lookupOrDefault<word>("U", "U")),
    phiName_(dict.lookupOrDefault<word>("phi", "phi")),
    rhoName_(dict.lookupOrDefault<word>("rho", "none")),
    psiName_(dict.lookupOrDefault<word>("psi", "none")),
    gamma_(readScalar(dict.lookup("gamma"))),
    pressure_(DataEntry<scalar>::New("pressure", dict))
{
    if (dict.found("value"))
    {
        fvPatchField<scalar>::operator=
        (
            scalarField("value", dict, p.size())
        );
    }
    else
    {
        const scalar t = this->db().time().timeOutputValue();
        fvPatchScalarField::operator==(pressure_->value(t));
    }
}
 
 
Foam::uniformTotalPressureFvPatchScalarField::
uniformTotalPressureFvPatchScalarField
(
    const uniformTotalPressureFvPatchScalarField& ptf,
    const fvPatch& p,
    const DimensionedField<scalar, volMesh>& iF,
    const fvPatchFieldMapper& mapper
)
:
    fixedValueFvPatchScalarField(p, iF),  // Don't map
    UName_(ptf.UName_),
    phiName_(ptf.phiName_),
    rhoName_(ptf.rhoName_),
    psiName_(ptf.psiName_),
    gamma_(ptf.gamma_),
    pressure_(ptf.pressure_, false)
{
    patchType() = ptf.patchType();
 
    // Set the patch pressure to the current total pressure
    // This is not ideal but avoids problems with the creation of patch faces
    const scalar t = this->db().time().timeOutputValue();
    fvPatchScalarField::operator==(pressure_->value(t));
}
 
 
Foam::uniformTotalPressureFvPatchScalarField::
uniformTotalPressureFvPatchScalarField
(
    const uniformTotalPressureFvPatchScalarField& ptf
)
:
    fixedValueFvPatchScalarField(ptf),
    UName_(ptf.UName_),
    phiName_(ptf.phiName_),
    rhoName_(ptf.rhoName_),
    psiName_(ptf.psiName_),
    gamma_(ptf.gamma_),
    pressure_(ptf.pressure_, false)
{}
 
 
Foam::uniformTotalPressureFvPatchScalarField::
uniformTotalPressureFvPatchScalarField
(
    const uniformTotalPressureFvPatchScalarField& ptf,
    const DimensionedField<scalar, volMesh>& iF
)
:
    fixedValueFvPatchScalarField(ptf, iF),
    UName_(ptf.UName_),
    phiName_(ptf.phiName_),
    rhoName_(ptf.rhoName_),
    psiName_(ptf.psiName_),
    gamma_(ptf.gamma_),
    pressure_(ptf.pressure_, false)
{}
 
 
// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
 
void Foam::uniformTotalPressureFvPatchScalarField::updateCoeffs
(
    const vectorField& Up
)
{
    if (updated())
    {
        return;
    }
 
    scalar p0 = pressure_->value(this->db().time().timeOutputValue());
 
    const fvsPatchField<scalar>& phip =
        patch().lookupPatchField<surfaceScalarField, scalar>(phiName_);
 
    if (psiName_ == "none" && rhoName_ == "none")
    {
        operator==(p0 - 0.5*(1.0 - pos(phip))*magSqr(Up));
    }
    else if (rhoName_ == "none")
    {
        const fvPatchField<scalar>& psip =
            patch().lookupPatchField<volScalarField, scalar>(psiName_);
 
        if (gamma_ > 1.0)
        {
            scalar gM1ByG = (gamma_ - 1.0)/gamma_;
 
            operator==
            (
                p0
               /pow
                (
                    (1.0 + 0.5*psip*gM1ByG*(1.0 - pos(phip))*magSqr(Up)),
                    1.0/gM1ByG
                )
            );
        }
        else
        {
            operator==(p0/(1.0 + 0.5*psip*(1.0 - pos(phip))*magSqr(Up)));
        }
    }
    else if (psiName_ == "none")
    {
        const fvPatchField<scalar>& rho =
            patch().lookupPatchField<volScalarField, scalar>(rhoName_);
 
        operator==(p0 - 0.5*rho*(1.0 - pos(phip))*magSqr(Up));
    }
    else
    {
        FatalErrorInFunction
            << " rho or psi set inconsitently, rho = " << rhoName_
            << ", psi = " << psiName_ << ".\n"
            << "    Set either rho or psi or neither depending on the "
               "definition of total pressure.\n"
            << "    Set the unused variables to 'none'.\n"
            << "    on patch " << this->patch().name()
            << " of field " << this->dimensionedInternalField().name()
            << " in file " << this->dimensionedInternalField().objectPath()
            << exit(FatalError);
    }
 
    fixedValueFvPatchScalarField::updateCoeffs();
}
 
 
void Foam::uniformTotalPressureFvPatchScalarField::updateCoeffs()
{
    updateCoeffs(patch().lookupPatchField<volVectorField, vector>(UName_));
}
 
 
void Foam::uniformTotalPressureFvPatchScalarField::write(Ostream& os) const
{
    fvPatchScalarField::write(os);
    writeEntryIfDifferent<word>(os, "U", "U", UName_);
    writeEntryIfDifferent<word>(os, "phi", "phi", phiName_);
    os.writeKeyword("rho") << rhoName_ << token::END_STATEMENT << nl;
    os.writeKeyword("psi") << psiName_ << token::END_STATEMENT << nl;
    os.writeKeyword("gamma") << gamma_ << token::END_STATEMENT << nl;
    pressure_->writeData(os);
    writeEntry("value", os);
}
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
    makePatchTypeField
    (
        fvPatchScalarField,
        uniformTotalPressureFvPatchScalarField
    );
}
 
// ************************************************************************* //