filmSurfaceVelocityFvPatchVectorField: New film surface boundary cond…

…ition

Class
    Foam::filmSurfaceVelocityFvPatchVectorField

Description
    Film surface velocity boundary condition

    Evaluates the surface velocity from the shear imposed by the neighbouring
    fluid velocity using a simple drag model based on the difference between the
    fluid and film velocities multiplied by the coefficient \c Cs.  This simple
    model is used in preference to the standard viscous shear stress model in
    order to provide some means to include the drag enhancing effect
    of surface ripples, rivulets etc. in the film surface.

Usage
    \table
        Property     | Description             | Required    | Default value
        Cs           | Fluid-film drag coefficient | yes |
    \endtable

    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            filmSurfaceVelocity;
        Cs              0.005;
    }
    \endverbatim

applications/solvers/modules/isothermalFilm/Make/files

@@ -19,6 +19,7 @@ patches/mappedFilmSurface/mappedFilmSurfaceFvPatch/mappedFilmSurfaceFvPatch.C
 derivedFvPatchFields/alphaOne/alphaOneFvPatchScalarField.C
 derivedFvPatchFields/filmContactAngle/filmContactAngleFvPatchScalarField.C
 derivedFvPatchFields/mappedFilmPressure/mappedFilmPressureFvPatchScalarField.C
+derivedFvPatchFields/filmSurfaceVelocity/filmSurfaceVelocityFvPatchVectorField.C
 
 filmGaussGrad/filmGaussGrads.C
 

applications/solvers/modules/isothermalFilm/derivedFvPatchFields/filmSurfaceVelocity/filmSurfaceVelocityFvPatchVectorField.C

@@ -0,0 +1,182 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Copyright (C) 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/>.
+
+\*---------------------------------------------------------------------------*/
+
+#include "filmSurfaceVelocityFvPatchVectorField.H"
+#include "momentumTransportModel.H"
+#include "mappedPatchBase.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::filmSurfaceVelocityFvPatchVectorField::
+filmSurfaceVelocityFvPatchVectorField
+(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF
+)
+:
+    mixedFvPatchField<vector>(p, iF),
+    Cs_(0)
+{
+    refValue() = Zero;
+    refGrad() = Zero;
+    valueFraction() = 0;
+}
+
+
+Foam::filmSurfaceVelocityFvPatchVectorField::
+filmSurfaceVelocityFvPatchVectorField
+(
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    mixedFvPatchField<vector>(p, iF, dict, false),
+    Cs_(dict.lookup<scalar>("Cs"))
+{
+    refValue() = Zero;
+    refGrad() = Zero;
+    valueFraction() = 0;
+
+    if (dict.found("value"))
+    {
+        fvPatchVectorField::operator=
+        (
+            vectorField("value", dict, p.size())
+        );
+    }
+    else
+    {
+        // If the value entry is not present initialise to zero-gradient
+        fvPatchVectorField::operator=(patchInternalField());
+    }
+}
+
+
+Foam::filmSurfaceVelocityFvPatchVectorField::
+filmSurfaceVelocityFvPatchVectorField
+(
+    const filmSurfaceVelocityFvPatchVectorField& ptf,
+    const fvPatch& p,
+    const DimensionedField<vector, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    mixedFvPatchField<vector>(ptf, p, iF, mapper),
+    Cs_(ptf.Cs_)
+{}
+
+
+Foam::filmSurfaceVelocityFvPatchVectorField::
+filmSurfaceVelocityFvPatchVectorField
+(
+    const filmSurfaceVelocityFvPatchVectorField& ptf,
+    const DimensionedField<vector, volMesh>& iF
+)
+:
+    mixedFvPatchField<vector>(ptf, iF),
+    Cs_(ptf.Cs_)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::filmSurfaceVelocityFvPatchVectorField::updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    // Since we're inside initEvaluate/evaluate there might be processor
+    // comms underway. Change the tag we use.
+    const int oldTag = UPstream::msgType();
+    UPstream::msgType() = oldTag + 1;
+
+    // Get the coupling information from the mappedPatchBase
+    const mappedPatchBase& mpp = mappedPatchBase::getMap(patch().patch());
+    const label patchiNbr = mpp.nbrPolyPatch().index();
+    const fvPatch& patchNbr =
+        refCast<const fvMesh>(mpp.nbrMesh()).boundary()[patchiNbr];
+
+    const vectorField UpNbr =
+        patchNbr.lookupPatchField<volVectorField, scalar>("U")
+       .patchInternalField();
+
+    // Set the reference value to the neighbouring fluid internal velocity
+    refValue() = mpp.distribute(UpNbr);
+
+    // Remove the normal component of the surface vel
+    const vectorField n(patch().nf());
+    refValue() -= n*(n & refValue());
+
+    // Lookup the momentum transport model
+    const momentumTransportModel& transportModel =
+        db().lookupType<momentumTransportModel>();
+
+    // Get the patch laminar viscosity
+    const tmp<scalarField> nuEff(transportModel.nuEff(patch().index()));
+
+    // Calculate the drag coefficient from the drag constant
+    // and the magnitude of the velocity difference
+    const scalarField Ds(Cs_*mag(refValue() - *this));
+
+    // Calculate the value-fraction from the balance between the
+    // external fluid drag and internal film stress
+    valueFraction() = Ds/(Ds + patch().deltaCoeffs()*nuEff);
+
+    mixedFvPatchField<vector>::updateCoeffs();
+
+    // Restore tag
+    UPstream::msgType() = oldTag;
+}
+
+
+void Foam::filmSurfaceVelocityFvPatchVectorField::write
+(
+    Ostream& os
+) const
+{
+    fvPatchField<vector>::write(os);
+
+    writeEntry(os, "Cs", Cs_);
+    writeEntry(os, "value", *this);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+   makePatchTypeField
+   (
+       fvPatchVectorField,
+       filmSurfaceVelocityFvPatchVectorField
+   );
+}
+
+
+// ************************************************************************* //

applications/solvers/modules/isothermalFilm/derivedFvPatchFields/filmSurfaceVelocity/filmSurfaceVelocityFvPatchVectorField.H

@@ -0,0 +1,165 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Copyright (C) 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::filmSurfaceVelocityFvPatchVectorField
+
+Description
+    Film surface velocity boundary condition
+
+    Evaluates the surface velocity from the shear imposed by the neighbouring
+    fluid velocity using a simple drag model based on the difference between the
+    fluid and film velocities multiplied by the coefficient \c Cs.  This simple
+    model is used in preference to the standard viscous shear stress model in
+    order to provide some means to include the drag enhancing effect
+    of surface ripples, rivulets etc. in the film surface.
+
+Usage
+    \table
+        Property     | Description             | Required    | Default value
+        Cs           | Fluid-film drag coefficient | yes |
+    \endtable
+
+    Example of the boundary condition specification:
+    \verbatim
+    <patchName>
+    {
+        type            filmSurfaceVelocity;
+        Cs              0.005;
+    }
+    \endverbatim
+
+See also
+    Foam::mixedFvPatchField
+
+SourceFiles
+    filmSurfaceVelocityFvPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef filmSurfaceVelocityFvPatchVectorField_H
+#define filmSurfaceVelocityFvPatchVectorField_H
+
+#include "mixedFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+/*---------------------------------------------------------------------------*\
+          Class filmSurfaceVelocityFvPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class filmSurfaceVelocityFvPatchVectorField
+:
+    public mixedFvPatchVectorField
+{
+    // Private Data
+
+        //- Fluid-film drag-coefficient
+        scalar Cs_;
+
+
+public:
+
+   //- Runtime type information
+   TypeName("filmSurfaceVelocity");
+
+
+   // Constructors
+
+        //- Construct from patch and internal field
+        filmSurfaceVelocityFvPatchVectorField
+        (
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        filmSurfaceVelocityFvPatchVectorField
+        (
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given
+        //  filmSurfaceVelocityFvPatchVectorField
+        //  onto a new patch
+        filmSurfaceVelocityFvPatchVectorField
+        (
+            const filmSurfaceVelocityFvPatchVectorField&,
+            const fvPatch&,
+            const DimensionedField<vector, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Disallow copy without setting internal field reference
+        filmSurfaceVelocityFvPatchVectorField
+        (
+            const filmSurfaceVelocityFvPatchVectorField&
+        ) = delete;
+
+        //- Copy constructor setting internal field reference
+        filmSurfaceVelocityFvPatchVectorField
+        (
+            const filmSurfaceVelocityFvPatchVectorField&,
+            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 filmSurfaceVelocityFvPatchVectorField
+                (
+                    *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
+
+// ************************************************************************* //

src/MomentumTransportModels/momentumTransportModels/derivedFvPatchFields/fixedShearStress/fixedShearStressFvPatchVectorField.C

@@ -2,7 +2,7 @@
   =========                 |
   \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
    \\    /   O peration     | Website:  https://openfoam.org
-    \\  /    A nd           | Copyright (C) 2011-2022 OpenFOAM Foundation
+    \\  /    A nd           | Copyright (C) 2011-2023 OpenFOAM Foundation
      \\/     M anipulation  |
 -------------------------------------------------------------------------------
 License
@@ -93,7 +93,7 @@ void Foam::fixedShearStressFvPatchVectorField::updateCoeffs()
     const momentumTransportModel& turbModel =
         db().lookupType<momentumTransportModel>(internalField().group());
 
-    scalarField nuEff(turbModel.nuEff(patch().index()));
+    const scalarField nuEff(turbModel.nuEff(patch().index()));
 
     const vectorField Uc(patchInternalField());