movingMappedWallVelocity: New velocity boundary condition

This boundary condition provides a no-slip velocity condition for mapped
walls. The wall velocity is taken to be the mesh velocity of the
neighbouring region.

This will typically be used in CHT simulations in order to apply the
mesh motion of a solid region to the boundary of the adjacent fluid
region.

Example of the boundary condition specification:

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

src/finiteVolume/Make/files

@@ -199,6 +199,7 @@ $(derivedFvPatchFields)/matchedFlowRateOutletVelocity/matchedFlowRateOutletVeloc
 $(derivedFvPatchFields)/noSlip/noSlipFvPatchVectorField.C
 $(derivedFvPatchFields)/movingWallVelocity/movingWallVelocityFvPatchVectorField.C
 $(derivedFvPatchFields)/movingWallSlipVelocity/movingWallSlipVelocityFvPatchVectorField.C
+$(derivedFvPatchFields)/movingMappedWallVelocity/movingMappedWallVelocityFvPatchVectorField.C
 $(derivedFvPatchFields)/outletInlet/outletInletFvPatchFields.C
 $(derivedFvPatchFields)/outletMappedUniformInlet/outletMappedUniformInletFvPatchFields.C
 $(derivedFvPatchFields)/fixedMeanOutletInlet/fixedMeanOutletInletFvPatchFields.C

src/finiteVolume/fields/fvPatchFields/derived/movingMappedWallVelocity/movingMappedWallVelocityFvPatchVectorField.C

@@ -0,0 +1,157 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Copyright (C) 2011-2024 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 "movingMappedWallVelocityFvPatchVectorField.H"
+#include "volFields.H"
+#include "surfaceFields.H"
+#include "fvcMeshPhi.H"
+#include "mappedFvPatchBaseBase.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::movingMappedWallVelocityFvPatchVectorField::
+movingMappedWallVelocityFvPatchVectorField
+(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    fixedValueFvPatchVectorField(p, iF, dict)
+{}
+
+
+Foam::movingMappedWallVelocityFvPatchVectorField::
+movingMappedWallVelocityFvPatchVectorField
+(
+    const movingMappedWallVelocityFvPatchVectorField& ptf,
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const fieldMapper& mapper
+)
+:
+    fixedValueFvPatchVectorField(ptf, p, iF, mapper, false)
+{
+    mapper(*this, ptf, vector::zero);
+}
+
+
+Foam::movingMappedWallVelocityFvPatchVectorField::
+movingMappedWallVelocityFvPatchVectorField
+(
+    const movingMappedWallVelocityFvPatchVectorField& mwvpvf,
+    const DimensionedField<vector, volMesh>& iF
+)
+:
+    fixedValueFvPatchVectorField(mwvpvf, iF)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::movingMappedWallVelocityFvPatchVectorField::map
+(
+    const fvPatchVectorField& ptf,
+    const fieldMapper& mapper
+)
+{
+    mapper(*this, ptf, vector::zero);
+}
+
+
+void Foam::movingMappedWallVelocityFvPatchVectorField::updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    const fvPatch& fvp = patch();
+
+    const mappedFvPatchBaseBase& mapper =
+        mappedFvPatchBaseBase::getMap(patch());
+    const fvMesh& nbrMesh = mapper.nbrMesh();
+    const fvPatch& nbrFvp = mapper.nbrFvPatch();
+
+    if (nbrMesh.moving())
+    {
+        // Calculate the normal velocity on this mesh from the mesh flux
+        const volVectorField& U =
+            static_cast<const volVectorField&>(internalField());
+        tmp<scalarField> Un =
+            U.mesh().moving()
+          ? fvc::meshPhi(U, fvp.index())/(fvp.magSf() + vSmall)
+          : tmp<scalarField>(new scalarField(fvp.size(), Zero));
+
+        // Calculate and map the mesh velocity from the neighbour
+        vectorField nbrCf0(nbrFvp.size());
+        forAll(nbrCf0, nbrPatchFacei)
+        {
+            nbrCf0[nbrPatchFacei] =
+                nbrMesh.faces()
+                [
+                    nbrMesh.polyFacesBf()[nbrFvp.index()][nbrPatchFacei]
+                ].centre(nbrMesh.oldPoints());
+        }
+        const vectorField nbrUp
+        (
+            (nbrFvp.Cf() - nbrCf0)/db().time().deltaTValue()
+        );
+        const vectorField Up(mapper.fromNeighbour(nbrUp));
+
+        // Set the velocity equal to the normal component from this mesh plus
+        // the tangential component from the neighbouring mesh. That way the
+        // flux is exactly preserved but the neighbour can impart shear. The
+        // normal components should be the same anyway, otherwise the mapped
+        // patches are moving apart. Using the normal component from this mesh
+        // just prevents mapping inaccuracies from affecting the flux.
+        const vectorField n(fvp.nf());
+        vectorField::operator=(Up + n*(Un - (n & Up)));
+    }
+
+    fixedValueFvPatchVectorField::updateCoeffs();
+}
+
+
+void Foam::movingMappedWallVelocityFvPatchVectorField::write(Ostream& os) const
+{
+    fvPatchVectorField::write(os);
+    writeEntry(os, "value", *this);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchVectorField,
+        movingMappedWallVelocityFvPatchVectorField
+    );
+}
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/movingMappedWallVelocity/movingMappedWallVelocityFvPatchVectorField.H

@@ -0,0 +1,152 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Copyright (C) 2011-2023 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::movingMappedWallVelocityFvPatchVectorField
+
+Description
+    This boundary condition provides a no-slip velocity condition for mapped
+    walls. The wall velocity is taken to be the mesh velocity of the
+    neighbouring region.
+
+    This will typically be used in CHT simulations in order to apply the
+    mesh motion of a solid region to the boundary of the adjacent fluid
+    region.
+
+Usage
+    Example of the boundary condition specification:
+    \verbatim
+    <patchName>
+    {
+        type            movingMappedWallVelocity;
+        value           uniform (0 0 0);    // Initial value
+    }
+    \endverbatim
+
+See also
+    Foam::fixedValueFvPatchVectorField
+
+SourceFiles
+    movingMappedWallVelocityFvPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef movingMappedWallVelocityFvPatchVectorField_H
+#define movingMappedWallVelocityFvPatchVectorField_H
+
+#include "fixedValueFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+            Class movingMappedWallVelocityFvPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class movingMappedWallVelocityFvPatchVectorField
+:
+    public fixedValueFvPatchVectorField
+{
+
+public:
+
+    //- Runtime type information
+    TypeName("movingMappedWallVelocity");
+
+
+    // Constructors
+
+        //- Construct from patch, internal field and dictionary
+        movingMappedWallVelocityFvPatchVectorField
+        (
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given
+        //  movingMappedWallVelocityFvPatchVectorField onto a new patch
+        movingMappedWallVelocityFvPatchVectorField
+        (
+            const movingMappedWallVelocityFvPatchVectorField&,
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&,
+            const fieldMapper&
+        );
+
+        //- Disallow copy without setting internal field reference
+        movingMappedWallVelocityFvPatchVectorField
+        (
+            const movingMappedWallVelocityFvPatchVectorField&
+        ) = delete;
+
+        //- Copy constructor setting internal field reference
+        movingMappedWallVelocityFvPatchVectorField
+        (
+            const movingMappedWallVelocityFvPatchVectorField&,
+            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 movingMappedWallVelocityFvPatchVectorField(*this, iF)
+            );
+        }
+
+
+    // Member Functions
+
+        // Mapping functions
+
+            //- Map the given fvPatchField onto this fvPatchField
+            virtual void map(const fvPatchVectorField&, const fieldMapper&);
+
+
+        // Evaluation functions
+
+            //- Update the coefficients associated with the patch field
+            virtual void updateCoeffs();
+
+
+        //- Write
+        virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //