prghPressure: New pressure BC to allow the specification of a fixed...

prghPressure: New pressure BC to allow the specification of a fixed static-pressure distribution in the p_rgh field

src/finiteVolume/fields/fvPatchFields/derived/prghPressure/prghPressureFvPatchScalarField.C

+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2013 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 "prghPressureFvPatchScalarField.H"
+#include "addToRunTimeSelectionTable.H"
+#include "fvPatchFieldMapper.H"
+#include "volFields.H"
+#include "uniformDimensionedFields.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::prghPressureFvPatchScalarField::
+prghPressureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    fixedValueFvPatchScalarField(p, iF),
+    rhoName_("rho"),
+    p_(p.size(), 0.0)
+{}
+
+
+Foam::prghPressureFvPatchScalarField::
+prghPressureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    fixedValueFvPatchScalarField(p, iF),
+    rhoName_(dict.lookupOrDefault<word>("rhoName", "rho")),
+    p_("p", dict, p.size())
+{
+    if (dict.found("value"))
+    {
+        fvPatchScalarField::operator=
+        (
+            scalarField("value", dict, p.size())
+        );
+    }
+    else
+    {
+        fvPatchField<scalar>::operator=(p_);
+    }
+}
+
+
+Foam::prghPressureFvPatchScalarField::
+prghPressureFvPatchScalarField
+(
+    const prghPressureFvPatchScalarField& ptf,
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    fixedValueFvPatchScalarField(ptf, p, iF, mapper),
+    rhoName_(ptf.rhoName_),
+    p_(ptf.p_, mapper)
+{}
+
+
+Foam::prghPressureFvPatchScalarField::
+prghPressureFvPatchScalarField
+(
+    const prghPressureFvPatchScalarField& ptf
+)
+:
+    fixedValueFvPatchScalarField(ptf),
+    rhoName_(ptf.rhoName_),
+    p_(ptf.p_)
+{}
+
+
+Foam::prghPressureFvPatchScalarField::
+prghPressureFvPatchScalarField
+(
+    const prghPressureFvPatchScalarField& ptf,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    fixedValueFvPatchScalarField(ptf, iF),
+    rhoName_(ptf.rhoName_),
+    p_(ptf.p_)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::prghPressureFvPatchScalarField::autoMap
+(
+    const fvPatchFieldMapper& m
+)
+{
+    fixedValueFvPatchScalarField::autoMap(m);
+    p_.autoMap(m);
+}
+
+
+void Foam::prghPressureFvPatchScalarField::rmap
+(
+    const fvPatchScalarField& ptf,
+    const labelList& addr
+)
+{
+    fixedValueFvPatchScalarField::rmap(ptf, addr);
+
+    const prghPressureFvPatchScalarField& tiptf =
+        refCast<const prghPressureFvPatchScalarField>(ptf);
+
+    p_.rmap(tiptf.p_, addr);
+}
+
+
+void Foam::prghPressureFvPatchScalarField::updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    const scalarField& rhop = patch().lookupPatchField<volScalarField, scalar>
+    (
+        rhoName_
+    );
+
+    const uniformDimensionedVectorField& g =
+        db().lookupObject<uniformDimensionedVectorField>("g");
+
+    operator==(p_ - rhop*((g.value() & patch().Cf())));
+
+    fixedValueFvPatchScalarField::updateCoeffs();
+}
+
+
+void Foam::prghPressureFvPatchScalarField::write(Ostream& os) const
+{
+    fvPatchScalarField::write(os);
+    if (rhoName_ != "rho")
+    {
+        os.writeKeyword("rhoName")
+            << rhoName_ << token::END_STATEMENT << nl;
+    }
+    p_.writeEntry("p", os);
+    writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchScalarField,
+        prghPressureFvPatchScalarField
+    );
+}
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/prghPressure/prghPressureFvPatchScalarField.H

+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2013 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/>.
+
+Class
+    Foam::prghPressureFvPatchScalarField
+
+Group
+    grpGenericBoundaryConditions
+
+Description
+    This boundary condition provides static pressure condition for p_rgh,
+    calculated as:
+
+        \f[
+            p_rgh = p - \rho g h
+        \f]
+
+    where
+    \vartable
+        p_rgh   | Pseudo hydrostatic pressure [Pa]
+        p       | Static pressure [Pa]
+        h       | Height in the opposite direction to gravity
+        \rho    | density
+        g       | acceleration due to gravity [m/s2]
+    \endtable
+
+    \heading Patch usage
+
+    \table
+        Property     | Description             | Required    | Default value
+        rhoName      | rho field name          | no          | rho
+        p            | static pressure         | yes         |
+    \endtable
+
+    Example of the boundary condition specification:
+    \verbatim
+    myPatch
+    {
+        type            prghPressure;
+        rhoName         rho;
+        p               uniform 0;
+        value           uniform 0; // optional initial value
+    }
+    \endverbatim
+
+SeeAlso
+    Foam::fixedValueFvPatchScalarField
+
+SourceFiles
+    prghPressureFvPatchScalarField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef prghPressureFvPatchScalarField_H
+#define prghPressureFvPatchScalarField_H
+
+#include "fixedValueFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+         Class prghPressureFvPatchScalarField Declaration
+\*---------------------------------------------------------------------------*/
+
+class prghPressureFvPatchScalarField
+:
+    public fixedValueFvPatchScalarField
+{
+
+protected:
+
+    // Protected data
+
+        //- Name of phase-fraction field
+        word rhoName_;
+
+        //- Static pressure
+        scalarField p_;
+
+
+public:
+
+    //- Runtime type information
+    TypeName("prghPressure");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        prghPressureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        prghPressureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given
+        //  prghPressureFvPatchScalarField onto a new patch
+        prghPressureFvPatchScalarField
+        (
+            const prghPressureFvPatchScalarField&,
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Construct as copy
+        prghPressureFvPatchScalarField
+        (
+            const prghPressureFvPatchScalarField&
+        );
+
+        //- Construct and return a clone
+        virtual tmp<fvPatchScalarField> clone() const
+        {
+            return tmp<fvPatchScalarField >
+            (
+                new prghPressureFvPatchScalarField(*this)
+            );
+        }
+
+        //- Construct as copy setting internal field reference
+        prghPressureFvPatchScalarField
+        (
+            const prghPressureFvPatchScalarField&,
+            const DimensionedField<scalar, volMesh>&
+        );
+
+        //- Construct and return a clone setting internal field reference
+        virtual tmp<fvPatchScalarField> clone
+        (
+            const DimensionedField<scalar, volMesh>& iF
+        ) const
+        {
+            return tmp<fvPatchScalarField>
+            (
+                new prghPressureFvPatchScalarField(*this, iF)
+            );
+        }
+
+
+    // Member functions
+
+        // Access
+
+            //- Return the rhoName
+            const word& rhoName() const
+            {
+                return rhoName_;
+            }
+
+            //- Return reference to the rhoName to allow adjustment
+            word& rhoName()
+            {
+                return rhoName_;
+            }
+
+            //- Return the static pressure
+            const scalarField& p() const
+            {
+                return p_;
+            }
+
+            //- Return reference to the static pressure to allow adjustment
+            scalarField& p()
+            {
+                return p_;
+            }
+
+
+        // Mapping functions
+
+            //- Map (and resize as needed) from self given a mapping object
+            virtual void autoMap
+            (
+                const fvPatchFieldMapper&
+            );
+
+            //- Reverse map the given fvPatchField onto this fvPatchField
+            virtual void rmap
+            (
+                const fvPatchScalarField&,
+                const labelList&
+            );
+
+
+        // Evaluation functions
+
+            //- Update the coefficients associated with the patch field
+            virtual void updateCoeffs();
+
+
+        //- Write
+        virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //