SRFWallVelocityFvPatchVectorField: New BC for walls rotating in the SRF

    Wall-velocity condition to be used in conjunction with the single rotating
    frame (SRF) model (see: FOAM::SRFModel)

    The condition applies the appropriate rotation transformation in time and
    space to determine the local SRF velocity of the wall.

        \f[
            U_p = - U_{p,srf}
        \f]

    where
    \vartable
        U_p     = patch velocity [m/s]
        U_{p,srf} = SRF velocity
    \endvartable

    The normal component of \f$ U_p \f$ is removed to ensure 0 wall-flux even
    if the wall patch faces are irregular.

    \heading Patch usage

    Example of the boundary condition specification:
    \verbatim
    myPatch
    {
        type            SRFWallVelocity;
        value           uniform (0 0 0);    // Initial value
    }
    \endverbatim

src/finiteVolume/Make/files

@@ -426,6 +426,7 @@ $(SRF)/SRFModel/SRFModel/SRFModel.C
 $(SRF)/SRFModel/SRFModel/SRFModelNew.C
 $(SRF)/SRFModel/rpm/rpm.C
 $(SRF)/derivedFvPatchFields/SRFVelocityFvPatchVectorField/SRFVelocityFvPatchVectorField.C
+$(SRF)/derivedFvPatchFields/SRFWallVelocityFvPatchVectorField/SRFWallVelocityFvPatchVectorField.C
 $(SRF)/derivedFvPatchFields/SRFFreestreamVelocityFvPatchVectorField/SRFFreestreamVelocityFvPatchVectorField.C
 
 fvOptions = $(general)/fvOptions

src/finiteVolume/cfdTools/general/SRF/derivedFvPatchFields/SRFWallVelocityFvPatchVectorField/SRFWallVelocityFvPatchVectorField.C

+/*---------------------------------------------------------------------------* \
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2016 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 "SRFWallVelocityFvPatchVectorField.H"
+#include "addToRunTimeSelectionTable.H"
+#include "volFields.H"
+
+#include "SRFModel.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::SRFWallVelocityFvPatchVectorField::SRFWallVelocityFvPatchVectorField
+(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF
+)
+:
+    fixedValueFvPatchVectorField(p, iF)
+{}
+
+
+Foam::SRFWallVelocityFvPatchVectorField::SRFWallVelocityFvPatchVectorField
+(
+    const SRFWallVelocityFvPatchVectorField& ptf,
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    fixedValueFvPatchVectorField(ptf, p, iF, mapper)
+{}
+
+
+Foam::SRFWallVelocityFvPatchVectorField::SRFWallVelocityFvPatchVectorField
+(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    fixedValueFvPatchVectorField(p, iF)
+{
+    fvPatchVectorField::operator=(vectorField("value", dict, p.size()));
+}
+
+
+Foam::SRFWallVelocityFvPatchVectorField::SRFWallVelocityFvPatchVectorField
+(
+    const SRFWallVelocityFvPatchVectorField& srfvpvf
+)
+:
+    fixedValueFvPatchVectorField(srfvpvf)
+{}
+
+
+Foam::SRFWallVelocityFvPatchVectorField::SRFWallVelocityFvPatchVectorField
+(
+    const SRFWallVelocityFvPatchVectorField& srfvpvf,
+    const DimensionedField<vector, volMesh>& iF
+)
+:
+    fixedValueFvPatchVectorField(srfvpvf, iF)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::SRFWallVelocityFvPatchVectorField::autoMap
+(
+    const fvPatchFieldMapper& m
+)
+{
+    vectorField::autoMap(m);
+}
+
+
+void Foam::SRFWallVelocityFvPatchVectorField::rmap
+(
+    const fvPatchVectorField& ptf,
+    const labelList& addr
+)
+{
+    fixedValueFvPatchVectorField::rmap(ptf, addr);
+}
+
+
+void Foam::SRFWallVelocityFvPatchVectorField::updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    // Get reference to the SRF model
+    const SRF::SRFModel& srf =
+        db().lookupObject<SRF::SRFModel>("SRFProperties");
+
+    // Determine patch velocity due to SRF
+    const vectorField Up(-srf.velocity(patch().Cf()));
+
+    // Remove the component of Up normal to the wall
+    // just in case it is not exactly circular
+    const vectorField n(patch().nf());
+    vectorField::operator=(Up - n*(n & Up));
+
+    fixedValueFvPatchVectorField::updateCoeffs();
+}
+
+
+void Foam::SRFWallVelocityFvPatchVectorField::write(Ostream& os) const
+{
+    fvPatchVectorField::write(os);
+    writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchVectorField,
+        SRFWallVelocityFvPatchVectorField
+    );
+}
+
+// ************************************************************************* //

src/finiteVolume/cfdTools/general/SRF/derivedFvPatchFields/SRFWallVelocityFvPatchVectorField/SRFWallVelocityFvPatchVectorField.H

+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2016 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::SRFWallVelocityFvPatchVectorField
+
+Group
+    grpWallBoundaryConditions
+
+Description
+    Wall-velocity condition to be used in conjunction with the single rotating
+    frame (SRF) model (see: FOAM::SRFModel)
+
+    The condition applies the appropriate rotation transformation in time and
+    space to determine the local SRF velocity of the wall.
+
+        \f[
+            U_p = - U_{p,srf}
+        \f]
+
+    where
+    \vartable
+        U_p     = patch velocity [m/s]
+        U_{p,srf} = SRF velocity
+    \endvartable
+
+    The normal component of \f$ U_p \f$ is removed to ensure 0 wall-flux even
+    if the wall patch faces are irregular.
+
+    \heading Patch usage
+
+    Example of the boundary condition specification:
+    \verbatim
+    myPatch
+    {
+        type            SRFWallVelocity;
+        value           uniform (0 0 0);    // Initial value
+    }
+    \endverbatim
+
+SeeAlso
+    Foam::SRFModel
+    Foam::SRFVelocityFvPatchVectorField
+    Foam::fixedValueFvPatchField
+
+SourceFiles
+    SRFWallVelocityFvPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef SRFWallVelocityFvPatchVectorField_H
+#define SRFWallVelocityFvPatchVectorField_H
+
+#include "fvPatchFields.H"
+#include "fixedValueFvPatchFields.H"
+#include "Switch.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+               Class SRFWallVelocityFvPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class SRFWallVelocityFvPatchVectorField
+:
+    public fixedValueFvPatchVectorField
+{
+
+public:
+
+    //- Runtime type information
+    TypeName("SRFWallVelocity");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        SRFWallVelocityFvPatchVectorField
+        (
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        SRFWallVelocityFvPatchVectorField
+        (
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given SRFWallVelocityFvPatchVectorField
+        //  onto a new patch
+        SRFWallVelocityFvPatchVectorField
+        (
+            const SRFWallVelocityFvPatchVectorField&,
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Construct as copy
+        SRFWallVelocityFvPatchVectorField
+        (
+            const SRFWallVelocityFvPatchVectorField&
+        );
+
+        //- Construct and return a clone
+        virtual tmp<fvPatchVectorField> clone() const
+        {
+            return tmp<fvPatchVectorField>
+            (
+                new SRFWallVelocityFvPatchVectorField(*this)
+            );
+        }
+
+        //- Construct as copy setting internal field reference
+        SRFWallVelocityFvPatchVectorField
+        (
+            const SRFWallVelocityFvPatchVectorField&,
+            const DimensionedField<vector, volMesh>&
+        );
+
+        //- Construct and return a clone setting internal field reference
+        virtual tmp<fvPatchVectorField> clone
+        (
+            const DimensionedField<vector, volMesh>& iF
+        ) const
+        {
+            return tmp<fvPatchVectorField>
+            (
+                new SRFWallVelocityFvPatchVectorField(*this, iF)
+            );
+        }
+
+
+    // Member functions
+
+        // 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 fvPatchVectorField&,
+                const labelList&
+            );
+
+
+        // Evaluation functions
+
+            //- Update the coefficients associated with the patch field
+            virtual void updateCoeffs();
+
+
+        // I-O
+
+            //- Write
+            virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //