fixedMeanOutletInletFvPatchField: New outlet/inlet boundary condition which fixes the outlet mean

Description
    This boundary condition extrapolates field to the patch using the near-cell
    values and adjusts the distribution to match the specified, optionally
    time-varying, mean value.  This extrapolated field is applied as a
    fixedValue for outflow faces but zeroGradient is applied to inflow faces.

    This boundary condition can be applied to pressure when inletOutlet is
    applied to the velocity so that a zeroGradient condition is applied to the
    pressure at inflow faces where the velocity is specified to avoid an
    unphysical over-specification of the set of boundary conditions.

Usage
    \table
        Property     | Description             | Required    | Default value
        meanValue    | mean value Function1    | yes         |
        phi          | Flux field name         | no          | phi
    \endtable

    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            fixedMeanOutletInlet;
        meanValue       1.0;
    }
    \endverbatim

See also
    Foam::fixedMeanFvPatchField
    Foam::outletInletFvPatchField
    Foam::Function1Types

src/finiteVolume/Make/files

@@ -166,6 +166,7 @@ $(derivedFvPatchFields)/noSlip/noSlipFvPatchVectorField.C
 $(derivedFvPatchFields)/movingWallVelocity/movingWallVelocityFvPatchVectorField.C
 $(derivedFvPatchFields)/outletInlet/outletInletFvPatchFields.C
 $(derivedFvPatchFields)/outletMappedUniformInlet/outletMappedUniformInletFvPatchFields.C
+$(derivedFvPatchFields)/fixedMeanOutletInlet/fixedMeanOutletInletFvPatchFields.C
 $(derivedFvPatchFields)/partialSlip/partialSlipFvPatchFields.C
 $(derivedFvPatchFields)/phaseHydrostaticPressure/phaseHydrostaticPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/pressureDirectedInletOutletVelocity/pressureDirectedInletOutletVelocityFvPatchVectorField.C

src/finiteVolume/fields/fvPatchFields/derived/fixedMeanOutletInlet/fixedMeanOutletInletFvPatchField.C

@@ -0,0 +1,148 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2018 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 "fixedMeanOutletInletFvPatchField.H"
+#include "volFields.H"
+#include "surfaceFields.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+template<class Type>
+Foam::fixedMeanOutletInletFvPatchField<Type>::fixedMeanOutletInletFvPatchField
+(
+    const fvPatch& p,
+    const DimensionedField<Type, volMesh>& iF
+)
+:
+    outletInletFvPatchField<Type>(p, iF),
+    meanValue_()
+{}
+
+
+template<class Type>
+Foam::fixedMeanOutletInletFvPatchField<Type>::fixedMeanOutletInletFvPatchField
+(
+    const fvPatch& p,
+    const DimensionedField<Type, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    outletInletFvPatchField<Type>(p, iF),
+    meanValue_(Function1<Type>::New("meanValue", dict))
+{
+    this->phiName_ = dict.lookupOrDefault<word>("phi", "phi");
+
+    fvPatchField<Type>::operator=
+    (
+        Field<Type>("value", dict, p.size())
+    );
+
+    this->refValue() = *this;
+    this->refGrad() = Zero;
+    this->valueFraction() = 0.0;
+}
+
+
+template<class Type>
+Foam::fixedMeanOutletInletFvPatchField<Type>::fixedMeanOutletInletFvPatchField
+(
+    const fixedMeanOutletInletFvPatchField<Type>& ptf,
+    const fvPatch& p,
+    const DimensionedField<Type, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    outletInletFvPatchField<Type>(ptf, p, iF, mapper),
+    meanValue_(ptf.meanValue_, false)
+{}
+
+
+template<class Type>
+Foam::fixedMeanOutletInletFvPatchField<Type>::fixedMeanOutletInletFvPatchField
+(
+    const fixedMeanOutletInletFvPatchField<Type>& ptf
+)
+:
+    outletInletFvPatchField<Type>(ptf),
+    meanValue_(ptf.meanValue_, false)
+{}
+
+
+template<class Type>
+Foam::fixedMeanOutletInletFvPatchField<Type>::fixedMeanOutletInletFvPatchField
+(
+    const fixedMeanOutletInletFvPatchField<Type>& ptf,
+    const DimensionedField<Type, volMesh>& iF
+)
+:
+    outletInletFvPatchField<Type>(ptf, iF),
+    meanValue_(ptf.meanValue_, false)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+template<class Type>
+void Foam::fixedMeanOutletInletFvPatchField<Type>::updateCoeffs()
+{
+    if (this->updated())
+    {
+        return;
+    }
+
+    const scalar t = this->db().time().timeOutputValue();
+    Type meanValue = meanValue_->value(t);
+
+    Field<Type> newValues(this->patchInternalField());
+
+    Type meanValuePsi =
+        gSum(this->patch().magSf()*newValues)
+       /gSum(this->patch().magSf());
+
+    if (mag(meanValue) > small && mag(meanValuePsi)/mag(meanValue) > 0.5)
+    {
+        newValues *= mag(meanValue)/mag(meanValuePsi);
+    }
+    else
+    {
+        newValues += (meanValue - meanValuePsi);
+    }
+
+    this->refValue() = newValues;
+
+    outletInletFvPatchField<Type>::updateCoeffs();
+}
+
+
+template<class Type>
+void Foam::fixedMeanOutletInletFvPatchField<Type>::write(Ostream& os) const
+{
+    fvPatchField<Type>::write(os);
+    meanValue_->writeData(os);
+    this->writeEntry("value", os);
+}
+
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/fixedMeanOutletInlet/fixedMeanOutletInletFvPatchField.H

@@ -0,0 +1,185 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2018 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::fixedMeanOutletInletFvPatchField
+
+Group
+    grpInletBoundaryConditions
+
+Description
+    This boundary condition extrapolates field to the patch using the near-cell
+    values and adjusts the distribution to match the specified, optionally
+    time-varying, mean value.  This extrapolated field is applied as a
+    fixedValue for outflow faces but zeroGradient is applied to inflow faces.
+
+    This boundary condition can be applied to pressure when inletOutlet is
+    applied to the velocity so that a zeroGradient condition is applied to the
+    pressure at inflow faces where the velocity is specified to avoid an
+    unphysical over-specification of the set of boundary conditions.
+
+Usage
+    \table
+        Property     | Description             | Required    | Default value
+        meanValue    | mean value Function1    | yes         |
+        phi          | Flux field name         | no          | phi
+    \endtable
+
+    Example of the boundary condition specification:
+    \verbatim
+    <patchName>
+    {
+        type            fixedMeanOutletInlet;
+        meanValue       1.0;
+    }
+    \endverbatim
+
+See also
+    Foam::fixedMeanFvPatchField
+    Foam::outletInletFvPatchField
+    Foam::Function1Types
+
+SourceFiles
+    fixedMeanOutletInletFvPatchField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef fixedMeanOutletInletFvPatchField_H
+#define fixedMeanOutletInletFvPatchField_H
+
+#include "outletInletFvPatchFields.H"
+#include "Function1.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+                  Class fixedMeanOutletInletFvPatchField Declaration
+\*---------------------------------------------------------------------------*/
+
+template<class Type>
+class fixedMeanOutletInletFvPatchField
+:
+    public outletInletFvPatchField<Type>
+{
+    // Private data
+
+        //- MeanValue value the field is adjusted to maintain
+        autoPtr<Function1<Type>> meanValue_;
+
+
+public:
+
+    //- Runtime type information
+    TypeName("fixedMeanOutletInlet");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        fixedMeanOutletInletFvPatchField
+        (
+            const fvPatch&,
+            const DimensionedField<Type, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        fixedMeanOutletInletFvPatchField
+        (
+            const fvPatch&,
+            const DimensionedField<Type, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given fixedMeanOutletInletFvPatchField
+        //  onto a new patch
+        fixedMeanOutletInletFvPatchField
+        (
+            const fixedMeanOutletInletFvPatchField<Type>&,
+            const fvPatch&,
+            const DimensionedField<Type, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Construct as copy
+        fixedMeanOutletInletFvPatchField
+        (
+            const fixedMeanOutletInletFvPatchField<Type>&
+        );
+
+        //- Construct and return a clone
+        virtual tmp<fvPatchField<Type>> clone() const
+        {
+            return tmp<fvPatchField<Type>>
+            (
+                new fixedMeanOutletInletFvPatchField<Type>(*this)
+            );
+        }
+
+        //- Construct as copy setting internal field reference
+        fixedMeanOutletInletFvPatchField
+        (
+            const fixedMeanOutletInletFvPatchField<Type>&,
+            const DimensionedField<Type, volMesh>&
+        );
+
+        //- Construct and return a clone setting internal field reference
+        virtual tmp<fvPatchField<Type>> clone
+        (
+            const DimensionedField<Type, volMesh>& iF
+        ) const
+        {
+            return tmp<fvPatchField<Type>>
+            (
+                new fixedMeanOutletInletFvPatchField<Type>(*this, iF)
+            );
+        }
+
+
+    // Member functions
+
+        //- Update the coefficients associated with the patch field
+        virtual void updateCoeffs();
+
+        //- Write
+        virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#ifdef NoRepository
+    #include "fixedMeanOutletInletFvPatchField.C"
+#endif
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/fixedMeanOutletInlet/fixedMeanOutletInletFvPatchFields.C

@@ -0,0 +1,43 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2018 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 "fixedMeanOutletInletFvPatchFields.H"
+#include "volMesh.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
+
+makePatchFields(fixedMeanOutletInlet);
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/fixedMeanOutletInlet/fixedMeanOutletInletFvPatchFields.H

@@ -0,0 +1,49 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2018 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/>.
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef fixedMeanOutletInletFvPatchFields_H
+#define fixedMeanOutletInletFvPatchFields_H
+
+#include "fixedMeanOutletInletFvPatchField.H"
+#include "fieldTypes.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+makePatchTypeFieldTypedefs(fixedMeanOutletInlet);
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/fixedMeanOutletInlet/fixedMeanOutletInletFvPatchFieldsFwd.H

@@ -0,0 +1,50 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2018 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/>.
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef fixedMeanOutletInletFvPatchFieldsFwd_H
+#define fixedMeanOutletInletFvPatchFieldsFwd_H
+
+#include "fieldTypes.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+template<class Type> class fixedMeanOutletInletFvPatchField;
+
+makePatchTypeFieldTypedefs(fixedMeanOutletInlet);
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //