fvOptions: Added vertical damping

This fvOption applies an explicit damping force to components of the
vector field in the direction of gravity. Its intended purpose is to
damp the vertical motions of an interface in the region approaching an
outlet so that no reflections are generated. The level of damping is
specified by a coefficient, lambda, given in units of 1/s.

It can be enabled for a cellZone named "nearOutlet", by adding the
following entry to constant/fvOptions:

    verticalDamping1
    {
        type            verticalDamping;

        selectionMode   cellZone;
        cellZone        nearOutlet;

        lambda          [0 0 -1 0 0 0 0] 1;

        timeStart       0;
        duration        1e6;
    }

This work was supported by Jan Kaufmann and Jan Oberhagemann at DNV GL.

src/fvOptions/Make/files

@@ -37,6 +37,7 @@ $(derivedSources)/buoyancyForce/buoyancyForce.C
 $(derivedSources)/buoyancyForce/buoyancyForceIO.C
 $(derivedSources)/buoyancyEnergy/buoyancyEnergy.C
 $(derivedSources)/buoyancyEnergy/buoyancyEnergyIO.C
+$(derivedSources)/verticalDamping/verticalDamping.C
 
 interRegion = sources/interRegion
 $(interRegion)/interRegionHeatTransfer/interRegionHeatTransferModel/interRegionHeatTransferModel.C

src/fvOptions/sources/derived/verticalDamping/verticalDamping.C

@@ -0,0 +1,153 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2017 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 "verticalDamping.H"
+#include "fvMesh.H"
+#include "fvMatrix.H"
+#include "geometricOneField.H"
+#include "meshTools.H"
+#include "uniformDimensionedFields.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace fv
+{
+    defineTypeNameAndDebug(verticalDamping, 0);
+    addToRunTimeSelectionTable(option, verticalDamping, dictionary);
+}
+}
+
+
+// * * * * * * * * * * * * * Private Member Functions  * * * * * * * * * * * //
+
+void Foam::fv::verticalDamping::addSup
+(
+    const volVectorField& alphaRhoU,
+    fvMatrix<vector>& eqn,
+    const label fieldi
+)
+{
+    const uniformDimensionedVectorField& g =
+        mesh_.lookupObject<uniformDimensionedVectorField>("g");
+
+    const dimensionedSymmTensor lgg(lambda_*sqr(g)/magSqr(g));
+
+    const DimensionedField<scalar, volMesh>& V = mesh_.V();
+
+    // Check dimensions
+    eqn.dimensions()
+      - V.dimensions()*(lgg.dimensions() & alphaRhoU.dimensions());
+
+    forAll(cells_, i)
+    {
+        const label c = cells_[i];
+        vector f = V[c]*(lgg.value() & alphaRhoU[c]);
+        meshTools::constrainDirection(mesh_, mesh_.solutionD(), f);
+        eqn.source()[c] += f;
+    }
+}
+
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::fv::verticalDamping::verticalDamping
+(
+    const word& name,
+    const word& modelType,
+    const dictionary& dict,
+    const fvMesh& mesh
+)
+:
+    cellSetOption(name, modelType, dict, mesh),
+    lambda_("lambda", dimless/dimTime, coeffs_.lookup("lambda"))
+{
+    read(dict);
+}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::fv::verticalDamping::addSup
+(
+    fvMatrix<vector>& eqn,
+    const label fieldi
+)
+{
+    addSup(eqn.psi(), eqn, fieldi);
+}
+
+
+void Foam::fv::verticalDamping::addSup
+(
+    const volScalarField& rho,
+    fvMatrix<vector>& eqn,
+    const label fieldi
+)
+{
+    addSup(rho*eqn.psi(), eqn, fieldi);
+}
+
+
+void Foam::fv::verticalDamping::addSup
+(
+    const volScalarField& alpha,
+    const volScalarField& rho,
+    fvMatrix<vector>& eqn,
+    const label fieldi
+)
+{
+    addSup(alpha*rho*eqn.psi(), eqn, fieldi);
+}
+
+
+bool Foam::fv::verticalDamping::read(const dictionary& dict)
+{
+    if (cellSetOption::read(dict))
+    {
+        lambda_ =
+            dimensionedScalar
+            (
+                lambda_.name(),
+                lambda_.dimensions(),
+                coeffs_.lookup(lambda_.name())
+            );
+
+        fieldNames_ = wordList(1, coeffs_.lookupOrDefault<word>("U", "U"));
+
+        applied_.setSize(1, false);
+
+        return true;
+    }
+    else
+    {
+        return false;
+    }
+}
+
+
+// ************************************************************************* //

src/fvOptions/sources/derived/verticalDamping/verticalDamping.H

@@ -0,0 +1,162 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2017 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::fv::verticalDamping
+
+Description
+    This fvOption applies an explicit damping force to components of the vector
+    field in the direction of gravity. Its intended purpose is to damp the
+    vertical motions of an interface in the region approaching an outlet so that
+    no reflections are generated.
+
+Usage
+    Example usage:
+    \verbatim
+    verticalDamping1
+    {
+        type            verticalDamping;
+
+        selectionMode   cellZone;
+        cellZone        nearOutlet;
+
+        lambda          [0 0 -1 0 0 0 0] 1; // Damping coefficient
+
+        timeStart       0;
+        duration        1e6;
+    }
+    \endverbatim
+
+SourceFiles
+    verticalDamping.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef verticalDamping_H
+#define verticalDamping_H
+
+#include "cellSetOption.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace fv
+{
+
+/*---------------------------------------------------------------------------*\
+                   Class verticalDamping Declaration
+\*---------------------------------------------------------------------------*/
+
+class verticalDamping
+:
+    public cellSetOption
+{
+private:
+
+    // Private data
+
+        //- Damping coefficient [1/s]
+        dimensionedScalar lambda_;
+
+
+    // Private Member Functions
+
+        //- Source term to momentum equation
+        void addSup
+        (
+            const volVectorField& alphaRhoU,
+            fvMatrix<vector>& eqn,
+            const label fieldi
+        );
+
+
+public:
+
+    //- Runtime type information
+    TypeName("verticalDamping");
+
+
+    // Constructors
+
+        //- Construct from components
+        verticalDamping
+        (
+            const word& name,
+            const word& modelType,
+            const dictionary& dict,
+            const fvMesh& mesh
+        );
+
+
+    //- Destructor
+    virtual ~verticalDamping()
+    {}
+
+
+    // Member Functions
+
+         // Add explicit and implicit contributions
+
+            //- Source term to momentum equation
+            virtual void addSup
+            (
+                fvMatrix<vector>& eqn,
+                const label fieldi
+            );
+
+            //- Source term to compressible momentum equation
+            virtual void addSup
+            (
+                const volScalarField& rho,
+                fvMatrix<vector>& eqn,
+                const label fieldi
+            );
+
+            //- Source term to phase momentum equation
+            virtual void addSup
+            (
+                const volScalarField& alpha,
+                const volScalarField& rho,
+                fvMatrix<vector>& eqn,
+                const label fieldi
+            );
+
+
+        // IO
+
+            //- Read dictionary
+            virtual bool read(const dictionary& dict);
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace fv
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //