ENH: Added new scalarFixedValue boundary condition

This condition applies a scalar multiplier to the value of another
boundary condition.

Usage
    Property     | Description             | Required    | Default value
    scale        | Time varing scale       | yes         |
    patch        | patchField providing the raw patch value | yes |

Example of the boundary condition specification to scale a reference
velocity of (15 0 0)  supplied as a fixedValue by a table of values
that ramps the scale from 0 to 1 over 1 second:

    <patchName>
    {
        type            scaledFixedValue;

        scale table
        (
            (    0   0)
            (  1.0 1.0)
            (100.0 1.0)
        );

        patch
        {
            type            fixedValue;
            value           uniform (15 0 0);
        }
    }

src/finiteVolume/Make/files

@@ -184,6 +184,7 @@ $(derivedFvPatchFields)/fixedNormalInletOutletVelocity/fixedNormalInletOutletVel
 $(derivedFvPatchFields)/rotatingPressureInletOutletVelocity/rotatingPressureInletOutletVelocityFvPatchVectorField.C
 $(derivedFvPatchFields)/rotatingTotalPressure/rotatingTotalPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/rotatingWallVelocity/rotatingWallVelocityFvPatchVectorField.C
+$(derivedFvPatchFields)/scaledFixedValue/scaledFixedValueFvPatchFields.C
 $(derivedFvPatchFields)/slip/slipFvPatchFields.C
 $(derivedFvPatchFields)/supersonicFreestream/supersonicFreestreamFvPatchVectorField.C
 $(derivedFvPatchFields)/surfaceNormalFixedValue/surfaceNormalFixedValueFvPatchVectorField.C

src/finiteVolume/fields/fvPatchFields/derived/scaledFixedValue/scaledFixedValueFvPatchField.C

@@ -0,0 +1,240 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | www.openfoam.com
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+    Copyright (C) 2019 OpenCFD Ltd.
+-------------------------------------------------------------------------------
+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 "scaledFixedValueFvPatchField.H"
+#include "addToRunTimeSelectionTable.H"
+#include "volFields.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+template<class Type>
+Foam::scaledFixedValueFvPatchField<Type>::scaledFixedValueFvPatchField
+(
+    const fvPatch& p,
+    const DimensionedField<Type, volMesh>& iF
+)
+:
+    fixedValueFvPatchField<Type>(p, iF),
+    scalePtr_(),
+    refValuePtr_(fvPatchField<Type>::New("refValue", p, iF))
+{}
+
+
+template<class Type>
+Foam::scaledFixedValueFvPatchField<Type>::scaledFixedValueFvPatchField
+(
+    const fvPatch& p,
+    const DimensionedField<Type, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    fixedValueFvPatchField<Type>(p, iF, dict, false),
+    scalePtr_(PatchFunction1<scalar>::New(p.patch(), "scale", dict)),
+    refValuePtr_(fvPatchField<Type>::New(p, iF, dict.subDict("refValue")))
+{
+    if (!isA<fixedValueFvPatchField<Type>>(refValuePtr_()))
+    {
+        FatalIOErrorInFunction(dict)
+            << typeName << " condition can only be applied to fixed value "
+            << "conditions"
+            << exit(FatalIOError);
+    }
+
+    const scalarField s(scalePtr_->value(this->db().time().timeOutputValue()));
+    this->operator==(s*refValuePtr_());
+}
+
+
+template<class Type>
+Foam::scaledFixedValueFvPatchField<Type>::scaledFixedValueFvPatchField
+(
+    const scaledFixedValueFvPatchField& ptf,
+    const fvPatch& p,
+    const DimensionedField<Type, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    fixedValueFvPatchField<Type>(ptf, p, iF, mapper),
+    scalePtr_(ptf.scalePtr_.clone(p.patch())),
+    refValuePtr_(fvPatchField<Type>::New(ptf.refValue(), p, iF, mapper))
+{}
+
+
+template<class Type>
+Foam::scaledFixedValueFvPatchField<Type>::scaledFixedValueFvPatchField
+(
+    const scaledFixedValueFvPatchField& spf
+)
+:
+    fixedValueFvPatchField<Type>(spf),
+    scalePtr_(spf.scalePtr_.clone(spf.patch().patch())),
+    refValuePtr_(spf.refValue().clone())
+{}
+
+
+template<class Type>
+Foam::scaledFixedValueFvPatchField<Type>::scaledFixedValueFvPatchField
+(
+    const scaledFixedValueFvPatchField& spf,
+    const DimensionedField<Type, volMesh>& iF
+)
+:
+    fixedValueFvPatchField<Type>(spf, iF),
+    scalePtr_(spf.scalePtr_.clone(spf.patch().patch())),
+    refValuePtr_(spf.refValue().clone())
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+template<class Type>
+void Foam::scaledFixedValueFvPatchField<Type>::autoMap
+(
+    const fvPatchFieldMapper& m
+)
+{
+    fixedValueFvPatchField<Type>::autoMap(m);
+    refValuePtr_->autoMap(m);
+
+    scalePtr_().autoMap(m);
+
+    if (scalePtr_().constant())
+    {
+        // If mapper is not dependent on time we're ok to evaluate
+        this->evaluate();
+    }
+}
+
+
+template<class Type>
+void Foam::scaledFixedValueFvPatchField<Type>::rmap
+(
+    const fvPatchField<Type>& ptf,
+    const labelList& addr
+)
+{
+    fixedValueFvPatchField<Type>::rmap(ptf, addr);
+
+    const scaledFixedValueFvPatchField& sptf =
+        refCast<const scaledFixedValueFvPatchField>(ptf);
+
+    refValuePtr_->rmap(sptf.refValue(), addr);
+
+    scalePtr_().rmap(sptf.scalePtr_(), addr);
+}
+
+
+template<class Type>
+void Foam::scaledFixedValueFvPatchField<Type>::updateCoeffs()
+{
+    if (this->updated())
+    {
+        return;
+    }
+
+    refValuePtr_->evaluate();
+
+    const scalarField s(scalePtr_->value(this->db().time().timeOutputValue()));
+
+    // Note: setting this field value using = operator (not ==)
+    Field<Type>::operator=(s*refValuePtr_());
+
+    fixedValueFvPatchField<Type>::updateCoeffs();
+}
+
+
+template<class Type>
+void Foam::scaledFixedValueFvPatchField<Type>::write(Ostream& os) const
+{
+    fvPatchField<Type>::write(os);
+
+    scalePtr_->writeData(os);
+
+    os.beginBlock("refValue");
+    refValuePtr_->write(os);
+    os.endBlock();
+}
+
+
+template<class Type>
+void Foam::scaledFixedValueFvPatchField<Type>::operator==
+(
+    const fvPatchField<Type>& ptf
+)
+{
+    const scalarField s(scalePtr_->value(this->db().time().timeOutputValue()));
+
+    forAll(s, facei)
+    {
+        const scalar si = s[facei];
+        if (mag(si) > ROOTVSMALL)
+        {
+            refValuePtr_->operator[](facei) = ptf[facei]/si;
+        }
+    }
+
+    Field<Type>::operator=(ptf);
+}
+
+
+template<class Type>
+void Foam::scaledFixedValueFvPatchField<Type>::operator==(const Field<Type>& tf)
+{
+    const scalarField s(scalePtr_->value(this->db().time().timeOutputValue()));
+
+    forAll(s, facei)
+    {
+        const scalar si = s[facei];
+        if (mag(si) > ROOTVSMALL)
+        {
+            refValuePtr_->operator[](facei) = tf[facei]/si;
+        }
+    }
+
+    Field<Type>::operator=(tf);
+}
+
+
+template<class Type>
+void Foam::scaledFixedValueFvPatchField<Type>::operator==(const Type& t)
+{
+    const scalarField s(scalePtr_->value(this->db().time().timeOutputValue()));
+
+    forAll(s, facei)
+    {
+        const scalar si = s[facei];
+        if (mag(si) > ROOTVSMALL)
+        {
+            refValuePtr_->operator[](facei) = t/si;
+        }
+    }
+
+    Field<Type>::operator=(t);
+}
+
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/scaledFixedValue/scaledFixedValueFvPatchField.H

@@ -0,0 +1,221 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | www.openfoam.com
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+    Copyright (C) 2019 OpenCFD Ltd.
+-------------------------------------------------------------------------------
+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::scaledFixedValueFvPatchField
+
+
+Description
+    This condition applies a scalar multiplier to the value of another
+    boundary condition.
+
+Usage
+    \table
+        Property     | Description             | Required    | Default value
+        scale        | Time varing scale       | yes         |
+        patch        | patchField providing the raw patch value | yes |
+    \endtable
+
+    Example of the boundary condition specification to scale a reference
+    velocity of (15 0 0)  supplied as a fixedValue by a table of values
+    that ramps the scale from 0 to 1 over 1 second:
+    \verbatim
+    <patchName>
+    {
+        type            scaledFixedValue;
+
+        scale table
+        (
+            (    0   0)
+            (  1.0 1.0)
+            (100.0 1.0)
+        );
+
+        patch
+        {
+            type            fixedValue;
+            value           uniform (15 0 0);
+        }
+    }
+    \endverbatim
+
+SourceFiles
+    scaledFixedValueFvPatchField.C
+
+SeeAlso
+    PatchFunction1.H
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef scaledFixedValueFvPatchField_H
+#define scaledFixedValueFvPatchField_H
+
+#include "fixedValueFvPatchField.H"
+#include "PatchFunction1.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+                Class scaledFixedValueFvPatchField Declaration
+\*---------------------------------------------------------------------------*/
+
+template<class Type>
+class scaledFixedValueFvPatchField
+:
+    public fixedValueFvPatchField<Type>
+{
+protected:
+
+    // Protected data
+
+        //- Scalar scale factor
+        autoPtr<PatchFunction1<scalar>> scalePtr_;
+
+        //- Condition to supply the reference value
+        tmp<fvPatchField<Type>> refValuePtr_;
+
+
+public:
+
+    //- Runtime type information
+    TypeName("scaledFixedValue");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        scaledFixedValueFvPatchField
+        (
+            const fvPatch&,
+            const DimensionedField<Type, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        scaledFixedValueFvPatchField
+        (
+            const fvPatch&,
+            const DimensionedField<Type, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given a scaledFixedValueFvPatchField onto
+        //- a new patch
+        scaledFixedValueFvPatchField
+        (
+            const scaledFixedValueFvPatchField&,
+            const fvPatch&,
+            const DimensionedField<Type, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Construct as copy
+        scaledFixedValueFvPatchField(const scaledFixedValueFvPatchField&);
+
+        //- Construct and return a clone
+        virtual tmp<fvPatchField<Type>> clone() const
+        {
+            return tmp<fvPatchField<Type>>
+            (
+                new scaledFixedValueFvPatchField(*this)
+            );
+        }
+
+        //- Construct as copy setting internal field reference
+        scaledFixedValueFvPatchField
+        (
+            const scaledFixedValueFvPatchField&,
+            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 scaledFixedValueFvPatchField(*this, iF)
+            );
+        }
+
+
+    // Member functions
+
+        // Access
+
+            //- Return the reference value condition
+            const fvPatchField<Type>& refValue() const
+            {
+                return refValuePtr_();
+            }
+
+
+        // Mapping functions
+
+            //- Map (and resize as needed) from self given a mapping object
+            virtual void autoMap(const fvPatchFieldMapper& m);
+
+            //- Reverse map the given fvPatchField onto this fvPatchField
+            virtual void rmap
+            (
+                const fvPatchField<Type>& ptf,
+                const labelList& addr
+            );
+
+
+        //- Update the coefficients associated with the patch field
+        virtual void updateCoeffs();
+
+        //- Write
+        virtual void write(Ostream&) const;
+
+
+        // Force an assignment irrespective of form of patch
+
+            virtual void operator==(const fvPatchField<Type>& ptf);
+            virtual void operator==(const Field<Type>& tf);
+            virtual void operator==(const Type& t);
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#ifdef NoRepository
+    #include "scaledFixedValueFvPatchField.C"
+#endif
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/scaledFixedValue/scaledFixedValueFvPatchFields.C

@@ -0,0 +1,44 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | www.openfoam.com
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+    Copyright (C) 2019 OpenCFD Ltd.
+-------------------------------------------------------------------------------
+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 "scaledFixedValueFvPatchFields.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
+
+makePatchFields(scaledFixedValue);
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/scaledFixedValue/scaledFixedValueFvPatchFields.H

@@ -0,0 +1,51 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | www.openfoam.com
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+    Copyright (C) 2019 OpenCFD Ltd.
+-------------------------------------------------------------------------------
+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 scaledFvPatchFields_H
+#define scaledFvPatchFields_H
+
+#include "scaledFixedValueFvPatchField.H"
+#include "fieldTypes.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+makePatchTypeFieldTypedefs(scaledFixedValue);
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/scaledFixedValue/scaledFixedValueFvPatchFieldsFwd.H

@@ -0,0 +1,52 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | www.openfoam.com
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+    Copyright (C) 2019 OpenCFD Ltd.
+-------------------------------------------------------------------------------
+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 scaledFvPatchFieldsFwd_H
+#define scaledFvPatchFieldsFwd_H
+
+#include "fieldTypes.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+template<class Type> class scaledFixedValueFvPatchField;
+
+makePatchTypeFieldTypedefs(scaledFixedValue);
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //