prghUniformDensityHydrostaticPressureFvPatchScalarField: New boundary condition for p_rgh

Sets the boundary values of p_rgh corresponding to a constant density hydrostatic
pressure distribution.

Description
    This boundary condition provides a hydrostatic pressure condition for p_rgh,
    calculated as:

        \f[
            p_{rgh} = p_{ref} - (\rho - \rho_0) g (h - h_{ref})
        \f]

    where
    \vartable
        p_{rgh}    | Pseudo hydrostatic pressure [Pa]
        p_{ref}    | Static pressure at hRef [Pa]
        h          | Height in the opposite direction to gravity
        h_{ref}    | Reference height in the opposite direction to gravity
        \rho       | Density field
        \rho_{ref} | Uniform reference density at boundary
        g          | Acceleration due to gravity [m/s^2]
    \endtable

Usage
    \table
        Property     | Description               | Required    | Default value
        pRef         | Reference static pressure | yes         |
        rhoRef       | Reference density         | yes         |
        rho          | Density field name        | no          | rho
    \endtable

    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            prghUniformDensityHydrostaticPressure;
        rhoRef          1000;
        p               0;
        value           uniform 0; // optional initial value
    }
    \endverbatim

src/finiteVolume/Make/files

@@ -192,6 +192,7 @@ $(derivedFvPatchFields)/translatingWallVelocity/translatingWallVelocityFvPatchVe
 $(derivedFvPatchFields)/turbulentInlet/turbulentInletFvPatchFields.C
 $(derivedFvPatchFields)/turbulentIntensityKineticEnergyInlet/turbulentIntensityKineticEnergyInletFvPatchScalarField.C
 $(derivedFvPatchFields)/uniformDensityHydrostaticPressure/uniformDensityHydrostaticPressureFvPatchScalarField.C
+$(derivedFvPatchFields)/prghUniformDensityHydrostaticPressure/prghUniformDensityHydrostaticPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/uniformFixedGradient/uniformFixedGradientFvPatchFields.C
 $(derivedFvPatchFields)/uniformFixedValue/uniformFixedValueFvPatchFields.C
 $(derivedFvPatchFields)/uniformInletOutlet/uniformInletOutletFvPatchFields.C

src/finiteVolume/fields/fvPatchFields/derived/prghUniformDensityHydrostaticPressure/prghUniformDensityHydrostaticPressureFvPatchScalarField.C

@@ -0,0 +1,179 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2018 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 "prghUniformDensityHydrostaticPressureFvPatchScalarField.H"
+#include "addToRunTimeSelectionTable.H"
+#include "fvPatchFieldMapper.H"
+#include "volFields.H"
+#include "uniformDimensionedFields.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::prghUniformDensityHydrostaticPressureFvPatchScalarField::
+prghUniformDensityHydrostaticPressureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    fixedValueFvPatchScalarField(p, iF),
+    pRef_(0),
+    rhoRef_(0),
+    rhoName_("rho")
+{}
+
+
+Foam::prghUniformDensityHydrostaticPressureFvPatchScalarField::
+prghUniformDensityHydrostaticPressureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    fixedValueFvPatchScalarField(p, iF, dict, false),
+    pRef_(readScalar(dict.lookup("pRef"))),
+    rhoRef_(readScalar(dict.lookup("rhoRef"))),
+    rhoName_(dict.lookupOrDefault<word>("rho", "rho"))
+{
+    if (dict.found("value"))
+    {
+        fvPatchScalarField::operator=
+        (
+            scalarField("value", dict, p.size())
+        );
+    }
+    else
+    {
+        fvPatchField<scalar>::operator=(pRef_);
+    }
+}
+
+
+Foam::prghUniformDensityHydrostaticPressureFvPatchScalarField::
+prghUniformDensityHydrostaticPressureFvPatchScalarField
+(
+    const prghUniformDensityHydrostaticPressureFvPatchScalarField& ptf,
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    fixedValueFvPatchScalarField(ptf, p, iF, mapper),
+    pRef_(ptf.pRef_),
+    rhoRef_(ptf.rhoRef_),
+    rhoName_(ptf.rhoName_)
+{}
+
+
+Foam::prghUniformDensityHydrostaticPressureFvPatchScalarField::
+prghUniformDensityHydrostaticPressureFvPatchScalarField
+(
+    const prghUniformDensityHydrostaticPressureFvPatchScalarField& ptf
+)
+:
+    fixedValueFvPatchScalarField(ptf),
+    pRef_(ptf.pRef_),
+    rhoRef_(ptf.rhoRef_),
+    rhoName_(ptf.rhoName_)
+{}
+
+
+Foam::prghUniformDensityHydrostaticPressureFvPatchScalarField::
+prghUniformDensityHydrostaticPressureFvPatchScalarField
+(
+    const prghUniformDensityHydrostaticPressureFvPatchScalarField& ptf,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    fixedValueFvPatchScalarField(ptf, iF),
+    pRef_(ptf.pRef_),
+    rhoRef_(ptf.rhoRef_),
+    rhoName_(ptf.rhoName_)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::prghUniformDensityHydrostaticPressureFvPatchScalarField::
+updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    const scalarField& rhop = patch().lookupPatchField<volScalarField, scalar>
+    (
+        rhoName_
+    );
+
+    const uniformDimensionedVectorField& g =
+        db().lookupObject<uniformDimensionedVectorField>("g");
+
+    const uniformDimensionedScalarField& hRef =
+        db().lookupObject<uniformDimensionedScalarField>("hRef");
+
+    dimensionedScalar ghRef
+    (
+        mag(g.value()) > small
+      ? g & (cmptMag(g.value())/mag(g.value()))*hRef
+      : dimensionedScalar("ghRef", g.dimensions()*dimLength, 0)
+    );
+
+    operator==
+    (
+        pRef_ - (rhop - rhoRef_)*((g.value() & patch().Cf()) - ghRef.value())
+    );
+
+    fixedValueFvPatchScalarField::updateCoeffs();
+}
+
+
+void Foam::prghUniformDensityHydrostaticPressureFvPatchScalarField::write
+(
+    Ostream& os
+) const
+{
+    fvPatchScalarField::write(os);
+    os.writeKeyword("pRef") << pRef_ << token::END_STATEMENT << nl;
+    os.writeKeyword("rhoRef") << rhoRef_ << token::END_STATEMENT << nl;
+    writeEntryIfDifferent<word>(os, "rho", "rho", rhoName_);
+    writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchScalarField,
+        prghUniformDensityHydrostaticPressureFvPatchScalarField
+    );
+}
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/prghUniformDensityHydrostaticPressure/prghUniformDensityHydrostaticPressureFvPatchScalarField.H

@@ -0,0 +1,206 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2018 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::prghUniformDensityHydrostaticPressureFvPatchScalarField
+
+Group
+    grpGenericBoundaryConditions
+
+Description
+    This boundary condition provides a hydrostatic pressure condition for p_rgh,
+    calculated as:
+
+        \f[
+            p_{rgh} = p_{ref} - (\rho - \rho_0) g (h - h_{ref})
+        \f]
+
+    where
+    \vartable
+        p_{rgh}    | Pseudo hydrostatic pressure [Pa]
+        p_{ref}    | Static pressure at hRef [Pa]
+        h          | Height in the opposite direction to gravity
+        h_{ref}    | Reference height in the opposite direction to gravity
+        \rho       | Density field
+        \rho_{ref} | Uniform reference density at boundary
+        g          | Acceleration due to gravity [m/s^2]
+    \endtable
+
+Usage
+    \table
+        Property     | Description               | Required    | Default value
+        pRef         | Reference static pressure | yes         |
+        rhoRef       | Reference density         | yes         |
+        rho          | Density field name        | no          | rho
+    \endtable
+
+    Example of the boundary condition specification:
+    \verbatim
+    <patchName>
+    {
+        type            prghUniformDensityHydrostaticPressure;
+        rhoRef          1000;
+        p               0;
+        value           uniform 0; // optional initial value
+    }
+    \endverbatim
+
+See also
+    Foam::fixedValueFvPatchScalarField
+
+SourceFiles
+    prghUniformDensityHydrostaticPressureFvPatchScalarField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef prghUniformDensityHydrostaticPressureFvPatchScalarField_H
+#define prghUniformDensityHydrostaticPressureFvPatchScalarField_H
+
+#include "fixedValueFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+   Class prghUniformDensityHydrostaticPressureFvPatchScalarField Declaration
+\*---------------------------------------------------------------------------*/
+
+class prghUniformDensityHydrostaticPressureFvPatchScalarField
+:
+    public fixedValueFvPatchScalarField
+{
+
+protected:
+
+    // Protected data
+
+        //- Reference Static pressure
+        scalar pRef_;
+
+        //- Reference density
+        scalar rhoRef_;
+
+        //- Name of phase-fraction field
+        word rhoName_;
+
+
+public:
+
+    //- Runtime type information
+    TypeName("prghUniformDensityHydrostaticPressure");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        prghUniformDensityHydrostaticPressureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        prghUniformDensityHydrostaticPressureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given
+        //  prghUniformDensityHydrostaticPressureFvPatchScalarField
+        //  onto a new patch
+        prghUniformDensityHydrostaticPressureFvPatchScalarField
+        (
+            const prghUniformDensityHydrostaticPressureFvPatchScalarField&,
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Construct as copy
+        prghUniformDensityHydrostaticPressureFvPatchScalarField
+        (
+            const prghUniformDensityHydrostaticPressureFvPatchScalarField&
+        );
+
+        //- Construct and return a clone
+        virtual tmp<fvPatchScalarField> clone() const
+        {
+            return tmp<fvPatchScalarField >
+            (
+                new prghUniformDensityHydrostaticPressureFvPatchScalarField
+                (
+                    *this
+                )
+            );
+        }
+
+        //- Construct as copy setting internal field reference
+        prghUniformDensityHydrostaticPressureFvPatchScalarField
+        (
+            const prghUniformDensityHydrostaticPressureFvPatchScalarField&,
+            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 prghUniformDensityHydrostaticPressureFvPatchScalarField
+                (
+                    *this,
+                    iF
+                )
+            );
+        }
+
+
+    // Member functions
+
+        // Evaluation functions
+
+            //- Update the coefficients associated with the patch field
+            virtual void updateCoeffs();
+
+
+        //- Write
+        virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/uniformDensityHydrostaticPressure/uniformDensityHydrostaticPressureFvPatchScalarField.H

@@ -2,7 +2,7 @@
   =========                 |
   \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
    \\    /   O peration     |
-    \\  /    A nd           | Copyright (C) 2011-2016 OpenFOAM Foundation
+    \\  /    A nd           | Copyright (C) 2011-2018 OpenFOAM Foundation
      \\/     M anipulation  |
 -------------------------------------------------------------------------------
 License
@@ -37,11 +37,11 @@ Description
 
     where
     \vartable
-        p_{hyd} | hyrostatic pressure [Pa]
+        p_{hyd} | Hyrostatic pressure [Pa]
-        p_{ref} | reference pressure [Pa]
+        p_{ref} | Reference pressure [Pa]
-        x_{ref} | reference point in Cartesian co-ordinates
+        x_{ref} | Reference point in Cartesian co-ordinates
-        \rho    | density (assumed uniform)
+        \rho    | Density (assumed uniform)
-        g       | acceleration due to gravity [m/s2]
+        g       | Acceleration due to gravity [m/s2]
     \endtable
 
 Usage