ENH: Adding lumpedMassWallTemperature BC and adding usage tutorial in buoyantPimpleFoam/hotRoom

src/TurbulenceModels/compressible/Make/files

@@ -12,6 +12,7 @@ $(BCs)/externalWallHeatFluxTemperature/externalWallHeatFluxTemperatureFvPatchSca
 $(BCs)/wallHeatTransfer/wallHeatTransferFvPatchScalarField.C
 $(BCs)/convectiveHeatTransfer/convectiveHeatTransferFvPatchScalarField.C
 $(BCs)/fixedIncidentRadiation/fixedIncidentRadiationFvPatchScalarField.C
+$(BCs)/lumpedMassWallTemperature/lumpedMassWallTemperatureFvPatchScalarField.C
 
 turbulentFluidThermoModels/derivedFvPatchFields/wallFunctions/alphatWallFunctions/alphatWallFunction/alphatWallFunctionFvPatchScalarField.C
 turbulentFluidThermoModels/derivedFvPatchFields/wallFunctions/alphatWallFunctions/alphatJayatillekeWallFunction/alphatJayatillekeWallFunctionFvPatchScalarField.C

src/TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/lumpedMassWallTemperature/lumpedMassWallTemperatureFvPatchScalarField.C

@@ -0,0 +1,210 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2016 OpenCFD Ltd.
+     \\/     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 "lumpedMassWallTemperatureFvPatchScalarField.H"
+#include "addToRunTimeSelectionTable.H"
+#include "fvPatchFieldMapper.H"
+#include "volFields.H"
+#include "mappedPatchBase.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::lumpedMassWallTemperatureFvPatchScalarField::
+lumpedMassWallTemperatureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    mixedFvPatchScalarField(p, iF),
+    temperatureCoupledBase(patch(), "undefined", "undefined", "undefined-K"),
+    Cp_(0.0),
+    mass_(0.0),
+    curTimeIndex_(-1)
+{
+    refValue() = 0.0;
+    refGrad() = 0.0;
+    valueFraction() = 1.0;
+}
+
+
+Foam::lumpedMassWallTemperatureFvPatchScalarField::
+lumpedMassWallTemperatureFvPatchScalarField
+(
+    const lumpedMassWallTemperatureFvPatchScalarField& ptf,
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    mixedFvPatchScalarField(ptf, p, iF, mapper),
+    temperatureCoupledBase(patch(), ptf),
+    Cp_(ptf.Cp_),
+    mass_(ptf.mass_),
+    curTimeIndex_(-1)
+{}
+
+
+Foam::lumpedMassWallTemperatureFvPatchScalarField::
+lumpedMassWallTemperatureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    mixedFvPatchScalarField(p, iF),
+    temperatureCoupledBase(patch(), dict),
+    Cp_(readScalar(dict.lookup("Cp"))),
+    mass_(readScalar(dict.lookup("mass"))),
+    curTimeIndex_(-1)
+{
+    refGrad() = 0.0;
+    valueFraction() = 1.0;
+    refValue() = scalarField("value", dict, p.size());
+
+    fvPatchScalarField::operator=(scalarField("value", dict, p.size()));
+}
+
+
+Foam::lumpedMassWallTemperatureFvPatchScalarField::
+lumpedMassWallTemperatureFvPatchScalarField
+(
+    const lumpedMassWallTemperatureFvPatchScalarField& tppsf
+)
+:
+    mixedFvPatchScalarField(tppsf),
+    temperatureCoupledBase(tppsf),
+    Cp_(tppsf.Cp_),
+    mass_(tppsf.mass_),
+    curTimeIndex_(-1)
+{}
+
+
+Foam::lumpedMassWallTemperatureFvPatchScalarField::
+lumpedMassWallTemperatureFvPatchScalarField
+(
+    const lumpedMassWallTemperatureFvPatchScalarField& tppsf,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    mixedFvPatchScalarField(tppsf, iF),
+    temperatureCoupledBase(patch(), tppsf),
+    Cp_(tppsf.Cp_),
+    mass_(tppsf.mass_),
+    curTimeIndex_(-1)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::lumpedMassWallTemperatureFvPatchScalarField::updateCoeffs()
+{
+    if (updated() || (curTimeIndex_ == this->db().time().timeIndex()))
+    {
+        return;
+    }
+
+    // Calculate heat flux in or out the wall
+    scalarField& Tp(*this);
+    const scalarField& magSf = patch().magSf();
+
+    const scalar deltaT(db().time().deltaTValue());
+
+    tmp<scalarField> tkappa(kappa(Tp));
+
+    const scalarField q(tkappa.ref()*snGrad());
+
+    // Total heat in or out of the wall
+    const scalar Q = gSum(q*magSf);
+
+    Tp += -(Q/mass_/Cp_)*deltaT;
+
+    refGrad() = 0.0;
+    refValue() = Tp;
+    valueFraction() = 1.0;
+
+    mixedFvPatchScalarField::updateCoeffs();
+
+    if (debug)
+    {
+        scalar qin(0);
+        scalar qout(0);
+
+        forAll(q, facei)
+        {
+            if (q[facei] > 0.0) //out the wall
+            {
+                qout += q[facei]*magSf[facei];
+            }
+            else if (q[facei] < 0.0) //into the wall
+            {
+                qin += q[facei]*magSf[facei];
+            }
+        }
+
+        Info<< patch().boundaryMesh().mesh().name() << ':'
+            << patch().name() << ':'
+            << this->internalField().name() << " :"
+            << " heat transfer rate:" << Q
+            << " wall temperature "
+            << " min:" << gMin(*this)
+            << " max:" << gMax(*this)
+            << " avg:" << gAverage(*this)
+            << " Qin [W]:" << qin
+            << " Qout [W]:" << qout
+            << endl;
+    }
+
+    curTimeIndex_ = this->db().time().timeIndex();
+}
+
+
+void Foam::lumpedMassWallTemperatureFvPatchScalarField::write
+(
+    Ostream& os
+) const
+{
+    mixedFvPatchScalarField::write(os);
+    temperatureCoupledBase::write(os);
+
+    os.writeKeyword("Cp")<< Cp_ << token::END_STATEMENT << nl;
+    os.writeKeyword("mass")<< mass_
+        << token::END_STATEMENT << nl;
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchScalarField,
+        lumpedMassWallTemperatureFvPatchScalarField
+    );
+}
+
+// ************************************************************************* //

src/TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/lumpedMassWallTemperature/lumpedMassWallTemperatureFvPatchScalarField.H

@@ -0,0 +1,188 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2016 OpenCFD Ltd.
+     \\/     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::lumpedMassWallTemperatureFvPatchScalarField
+
+Group
+    grpThermoBoundaryConditions grpWallBoundaryConditions
+
+Description
+    Employs a lumped mass model for temperature.
+
+    It considers a single temperature value for the whole patch and evaluates
+    the temperature evolution using the net heat flux into the patch.
+
+Usage
+    \table
+        Property     | Description                 | Required | Default value
+        kappa        | thermal conductivity option | yes      |
+        Cp           | Heat capacity [J/Kg K]]     | yes      |
+        mass         | Total mass [Kg]             | yes      |
+    \endtable
+
+    Example of the boundary condition specification:
+    \verbatim
+    myPatch
+    {
+        type            lumpedMassWallTemperature;
+        kappaMethod     fluidThermo;
+        kappaName       none;
+        mass            1000;
+        Cp              4100;
+        value           uniform 300.0;
+    }
+    \endverbatim
+
+SourceFiles
+    lumpedMassWallTemperatureFvPatchScalarField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef lumpedMassWallTemperatureFvPatchScalarField_H
+#define lumpedMassWallTemperatureFvPatchScalarField_H
+
+#include "mixedFvPatchFields.H"
+#include "temperatureCoupledBase.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+         Class lumpedMassWallTemperatureFvPatchScalarField Declaration
+\*---------------------------------------------------------------------------*/
+
+class lumpedMassWallTemperatureFvPatchScalarField
+:
+    public mixedFvPatchScalarField,
+    public temperatureCoupledBase
+{
+private:
+
+    // Private data
+
+        //- Specifc heat capacity [J/kg/K]
+        scalar Cp_;
+
+        //- Mass / [kg]
+        scalar mass_;
+
+        //- Current time index (used for updating)
+        label curTimeIndex_;
+
+
+public:
+
+    //- Runtime type information
+    TypeName("lumpedMassWallTemperature");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        lumpedMassWallTemperatureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        lumpedMassWallTemperatureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given
+        // lumpedMassWallTemperatureFvPatchScalarField
+        // onto a new patch
+        lumpedMassWallTemperatureFvPatchScalarField
+        (
+            const lumpedMassWallTemperatureFvPatchScalarField&,
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Construct as copy
+        lumpedMassWallTemperatureFvPatchScalarField
+        (
+            const lumpedMassWallTemperatureFvPatchScalarField&
+        );
+
+        //- Construct and return a clone
+        virtual tmp<fvPatchScalarField> clone() const
+        {
+            return tmp<fvPatchScalarField>
+            (
+                new lumpedMassWallTemperatureFvPatchScalarField(*this)
+            );
+        }
+
+        //- Construct as copy setting internal field reference
+        lumpedMassWallTemperatureFvPatchScalarField
+        (
+            const lumpedMassWallTemperatureFvPatchScalarField&,
+            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 lumpedMassWallTemperatureFvPatchScalarField(*this, iF)
+            );
+        }
+
+
+    // Member functions
+
+        // Evaluation functions
+
+            //- Update the coefficients associated with the patch field
+            virtual void updateCoeffs();
+
+
+        // I-O
+
+            //- Write
+            void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //

tutorials/heatTransfer/buoyantPimpleFoam/hotRoom/0/T

@@ -28,8 +28,12 @@ boundaryField
 
     ceiling
     {
-        type            fixedValue;
+        type            lumpedMassWallTemperature;
-        value           uniform 300;
+        kappaMethod     fluidThermo;
+        kappaName       none;
+        mass            1000;
+        Cp              4100;
+        value           uniform 300.0;
     }
 
     fixedWalls

tutorials/heatTransfer/buoyantPimpleFoam/hotRoom/0/T.orig

@@ -28,8 +28,12 @@ boundaryField
 
     ceiling
     {
-        type            fixedValue;
+        type            lumpedMassWallTemperature;
-        value           uniform 300;
+        kappaMethod     fluidThermo;
+        kappaName       none;
+        mass            1000;
+        Cp              4100;
+        value           uniform 300.0;
     }
 
     fixedWalls