VoF solvers: New interfaceCompressionFvPatchScalarField BC and additi…

…onal shear compression

Provides the additional compression necessary to ensure interface integrity
adjacent to a boundary at a low angle of incidence to the interface.  This is
particularly important when simulating planing hulls.

applications/solvers/multiphase/VoF/alphaEqn.H

@@ -65,6 +65,14 @@
         phic += (mixture.cAlpha()*icAlpha)*fvc::interpolate(mag(U));
     }
 
+    // Add the optional shear compression contribution
+    if (scAlpha > 0)
+    {
+        phic +=
+            scAlpha*mag(mesh.delta() & fvc::interpolate(symm(fvc::grad(U))));
+    }
+
+
     surfaceScalarField::Boundary& phicBf =
         phic.boundaryFieldRef();
 

src/finiteVolume/Make/files

@@ -205,6 +205,7 @@ $(derivedFvPatchFields)/prghTotalPressure/prghTotalPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/prghTotalHydrostaticPressure/prghTotalHydrostaticPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/fixedProfile/fixedProfileFvPatchFields.C
 $(derivedFvPatchFields)/plenumPressure/plenumPressureFvPatchScalarField.C
+$(derivedFvPatchFields)/interfaceCompression/interfaceCompressionFvPatchScalarField.C
 
 fvsPatchFields = fields/fvsPatchFields
 $(fvsPatchFields)/fvsPatchField/fvsPatchFields.C

src/finiteVolume/cfdTools/general/include/alphaControls.H

@@ -19,3 +19,9 @@ scalar icAlpha
 (
     alphaControls.lookupOrDefault<scalar>("icAlpha", 0)
 );
+
+// Shear compression coefficient
+scalar scAlpha
+(
+    alphaControls.lookupOrDefault<scalar>("scAlpha", 0)
+);

src/finiteVolume/fields/fvPatchFields/derived/interfaceCompression/interfaceCompressionFvPatchScalarField.C

@@ -0,0 +1,127 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  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 "interfaceCompressionFvPatchScalarField.H"
+#include "addToRunTimeSelectionTable.H"
+#include "fvPatchFieldMapper.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::interfaceCompressionFvPatchScalarField::
+interfaceCompressionFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    fixedValueFvPatchScalarField(p, iF)
+{}
+
+
+Foam::interfaceCompressionFvPatchScalarField::
+interfaceCompressionFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    fixedValueFvPatchScalarField(p, iF)
+{
+    evaluate();
+}
+
+
+Foam::interfaceCompressionFvPatchScalarField::
+interfaceCompressionFvPatchScalarField
+(
+    const interfaceCompressionFvPatchScalarField& ptf,
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    fixedValueFvPatchScalarField(ptf, p, iF, mapper)
+{}
+
+
+Foam::interfaceCompressionFvPatchScalarField::
+interfaceCompressionFvPatchScalarField
+(
+    const interfaceCompressionFvPatchScalarField& ptf
+)
+:
+    fixedValueFvPatchScalarField(ptf)
+{}
+
+
+Foam::interfaceCompressionFvPatchScalarField::
+interfaceCompressionFvPatchScalarField
+(
+    const interfaceCompressionFvPatchScalarField& ptf,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    fixedValueFvPatchScalarField(ptf, iF)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::interfaceCompressionFvPatchScalarField::updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    operator==(pos(this->patchInternalField() - 0.5));
+
+    fixedValueFvPatchScalarField::updateCoeffs();
+}
+
+
+void Foam::interfaceCompressionFvPatchScalarField::write
+(
+    Ostream& os
+) const
+{
+    fvPatchScalarField::write(os);
+    writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchScalarField,
+        interfaceCompressionFvPatchScalarField
+    );
+}
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/interfaceCompression/interfaceCompressionFvPatchScalarField.H

@@ -0,0 +1,155 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  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::interfaceCompressionFvPatchScalarField
+
+Group
+    grpGenericBoundaryConditions
+
+Description
+    Applies interface-compression to the phase-fraction distribution at the
+    patch by setting the phase-fraction to 0 if it is below 0.5, otherwise
+    to 1.
+
+    This approach is useful to avoid unphysical "bleed" of the lighter phase
+    along the surface in regions of high shear adjacent to the surface which
+    is at a shallow angle to the interface.
+
+See also
+    Foam::fixedValueFvPatchScalarField
+
+SourceFiles
+    interfaceCompressionFvPatchScalarField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef interfaceCompressionFvPatchScalarField_H
+#define interfaceCompressionFvPatchScalarField_H
+
+#include "fixedValueFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+         Class interfaceCompressionFvPatchScalarField Declaration
+\*---------------------------------------------------------------------------*/
+
+class interfaceCompressionFvPatchScalarField
+:
+    public fixedValueFvPatchScalarField
+{
+
+public:
+
+    //- Runtime type information
+    TypeName("interfaceCompression");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        interfaceCompressionFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        interfaceCompressionFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given
+        //  interfaceCompressionFvPatchScalarField onto a new patch
+        interfaceCompressionFvPatchScalarField
+        (
+            const interfaceCompressionFvPatchScalarField&,
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Construct as copy
+        interfaceCompressionFvPatchScalarField
+        (
+            const interfaceCompressionFvPatchScalarField&
+        );
+
+        //- Construct and return a clone
+        virtual tmp<fvPatchScalarField> clone() const
+        {
+            return tmp<fvPatchScalarField >
+            (
+                new interfaceCompressionFvPatchScalarField(*this)
+            );
+        }
+
+        //- Construct as copy setting internal field reference
+        interfaceCompressionFvPatchScalarField
+        (
+            const interfaceCompressionFvPatchScalarField&,
+            const DimensionedField<scalar, volMesh>&
+        );
+
+        //- Construct and return a clone setting internal field reference
+        virtual tmp<fvPatchScalarField> clone
+        (
+            const DimensionedField<scalar, volMesh>& iF
+        ) const
+        {
+            return tmp<fvPatchScalarField>
+            (
+                new interfaceCompressionFvPatchScalarField(*this, iF)
+            );
+        }
+
+
+    // Member functions
+
+        // Evaluation functions
+
+            //- Update the coefficients associated with the patch field
+            virtual void updateCoeffs();
+
+
+        //- Write
+        virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //