movingWallSlipVelocity: Added boundary condition

This boundary condition specifies a slip velocity on moving walls. It
works similarly to movingWallVelocity, except that the tangential
velocity is not constrained. It can be specified as follows:

    <patchName>
    {
        type            movingWallSlipVelocity;
        value           uniform (0 0 0); // Initial value
    }

src/finiteVolume/Make/files

@@ -178,6 +178,7 @@ $(derivedFvPatchFields)/mappedVelocityFluxFixedValue/mappedVelocityFluxFixedValu
 $(derivedFvPatchFields)/matchedFlowRateOutletVelocity/matchedFlowRateOutletVelocityFvPatchVectorField.C
 $(derivedFvPatchFields)/noSlip/noSlipFvPatchVectorField.C
 $(derivedFvPatchFields)/movingWallVelocity/movingWallVelocityFvPatchVectorField.C
+$(derivedFvPatchFields)/movingWallSlipVelocity/movingWallSlipVelocityFvPatchVectorField.C
 $(derivedFvPatchFields)/outletInlet/outletInletFvPatchFields.C
 $(derivedFvPatchFields)/outletMappedUniformInlet/outletMappedUniformInletFvPatchFields.C
 $(derivedFvPatchFields)/fixedMeanOutletInlet/fixedMeanOutletInletFvPatchFields.C

src/finiteVolume/fields/fvPatchFields/derived/movingWallSlipVelocity/movingWallSlipVelocityFvPatchVectorField.C

@@ -0,0 +1,149 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Copyright (C) 2021 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 "movingWallSlipVelocityFvPatchVectorField.H"
+#include "volFields.H"
+#include "surfaceFields.H"
+#include "fvcMeshPhi.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::movingWallSlipVelocityFvPatchVectorField::
+movingWallSlipVelocityFvPatchVectorField
+(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF
+)
+:
+    directionMixedFvPatchVectorField(p, iF)
+{
+    refValue() = Zero;
+    refGrad() = Zero;
+    valueFraction() = Zero;
+}
+
+
+Foam::movingWallSlipVelocityFvPatchVectorField::
+movingWallSlipVelocityFvPatchVectorField
+(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    directionMixedFvPatchVectorField(p, iF)
+{
+    fvPatchVectorField::operator=(vectorField("value", dict, p.size()));
+
+    const vectorField n(p.nf());
+
+    refValue() = sqr(n) & *this;
+    refGrad() = Zero;
+    valueFraction() = sqr(n);
+}
+
+
+Foam::movingWallSlipVelocityFvPatchVectorField::
+movingWallSlipVelocityFvPatchVectorField
+(
+    const movingWallSlipVelocityFvPatchVectorField& ptf,
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    directionMixedFvPatchVectorField(ptf, p, iF, mapper)
+{}
+
+
+Foam::movingWallSlipVelocityFvPatchVectorField::
+movingWallSlipVelocityFvPatchVectorField
+(
+    const movingWallSlipVelocityFvPatchVectorField& mwvpvf,
+    const DimensionedField<vector, volMesh>& iF
+)
+:
+    directionMixedFvPatchVectorField(mwvpvf, iF)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::movingWallSlipVelocityFvPatchVectorField::updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    const fvMesh& mesh = internalField().mesh();
+
+    if (mesh.moving())
+    {
+        const fvPatch& p = patch();
+
+        const volVectorField& U =
+            static_cast<const volVectorField&>(internalField());
+
+        scalarField phip
+        (
+            p.patchField<surfaceScalarField, scalar>(fvc::meshPhi(U))
+        );
+
+        const vectorField n(p.nf());
+        const scalarField& magSf = p.magSf();
+
+        tmp<scalarField> Un = phip/(magSf + vSmall);
+
+        refValue() = n*Un;
+        refGrad() = Zero;
+        valueFraction() = sqr(n);
+    }
+
+    directionMixedFvPatchVectorField::updateCoeffs();
+    directionMixedFvPatchVectorField::evaluate();
+}
+
+
+void Foam::movingWallSlipVelocityFvPatchVectorField::write(Ostream& os) const
+{
+    fvPatchVectorField::write(os);
+    writeEntry(os, "value", *this);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchVectorField,
+        movingWallSlipVelocityFvPatchVectorField
+    );
+}
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/movingWallSlipVelocity/movingWallSlipVelocityFvPatchVectorField.H

@@ -0,0 +1,142 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Copyright (C) 2021 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::movingWallSlipVelocityFvPatchVectorField
+
+Description
+    This boundary condition provides a slip velocity condition for cases with
+    moving walls.
+
+Usage
+    Example of the boundary condition specification:
+    \verbatim
+    <patchName>
+    {
+        type            movingWallSlipVelocity;
+        value           uniform (0 0 0);    // Initial value
+    }
+    \endverbatim
+
+SourceFiles
+    movingWallSlipVelocityFvPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef movingWallSlipVelocityFvPatchVectorField_H
+#define movingWallSlipVelocityFvPatchVectorField_H
+
+#include "directionMixedFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+            Class movingWallSlipVelocityFvPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class movingWallSlipVelocityFvPatchVectorField
+:
+    public directionMixedFvPatchVectorField
+{
+
+public:
+
+    //- Runtime type information
+    TypeName("movingWallSlipVelocity");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        movingWallSlipVelocityFvPatchVectorField
+        (
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        movingWallSlipVelocityFvPatchVectorField
+        (
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given movingWallSlipVelocityFvPatchVectorField
+        //  onto a new patch
+        movingWallSlipVelocityFvPatchVectorField
+        (
+            const movingWallSlipVelocityFvPatchVectorField&,
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Disallow copy without setting internal field reference
+        movingWallSlipVelocityFvPatchVectorField
+        (
+            const movingWallSlipVelocityFvPatchVectorField&
+        ) = delete;
+
+        //- Copy constructor setting internal field reference
+        movingWallSlipVelocityFvPatchVectorField
+        (
+            const movingWallSlipVelocityFvPatchVectorField&,
+            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 movingWallSlipVelocityFvPatchVectorField(*this, iF)
+            );
+        }
+
+
+    // Member Functions
+
+        //- Update the coefficients associated with the patch field
+        virtual void updateCoeffs();
+
+        //- Write
+        virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //