interRegionHeatTransfer.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2011-2023 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::interRegionHeatTransfer
 
Description
    Model for inter-region heat exchange. Requires specification of a model for
    the heat transfer coefficient (htc) and the area per unit volume (Av).
    These are then used to apply the following source to the energy equation:
 
    \f[
        -htc*Av*(T_{nbr,mapped} - T)
    \f]
 
    If the semiImplicit option is set, then this becomes:
 
    \f[
        -htc*Av*(T_{nbr,mapped} - T) + htc*Av/Cp*h - Sp(htc*Av/Cp, h);
    \f]
 
Usage
    Example usage:
    \verbatim
    interRegionHeatTransfer
    {
        type            interRegionHeatTransfer;
 
        nbrRegion       other;
 
        interpolationMethod intersection;
        master          true;
 
        semiImplicit    no;
 
        Av              200;
 
        heatTransferCoefficientModel constant;
 
        htc             10;
    }
    \endverbatim
 
See also
    Foam::fv::heatTransferCoefficientModel
 
SourceFiles
    interRegionHeatTransfer.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef interRegionHeatTransfer_H
#define interRegionHeatTransfer_H
 
#include "interRegionModel.H"
#include "heatTransferCoefficientModel.H"
#include "heatTransferAv.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
namespace fv
{
 
/*---------------------------------------------------------------------------*\
                Class interRegionHeatTransfer Declaration
\*---------------------------------------------------------------------------*/
 
class interRegionHeatTransfer
:
    public interRegionModel
{
    // Private data
 
        //- Flag to activate semi-implicit coupling
        bool semiImplicit_;
 
        //- Name of temperature field; default = "T"
        word TName_;
 
        //- Name of neighbour temperature field; default = "T"
        word TNbrName_;
 
        //- The heat transfer area per unit volume
        autoPtr<heatTransferAv> heatTransferAv_;
 
        //- The heat transfer model
        autoPtr<heatTransferCoefficientModel> heatTransferCoefficientModel_;
 
 
    // Private member functions
 
        //- Non-virtual read
        void readCoeffs();
 
        //- Get the neighbour heat transfer
        const interRegionHeatTransfer& nbrHeatTransfer() const;
 
 
public:
 
    //- Runtime type information
    TypeName("interRegionHeatTransfer");
 
 
    // Constructors
 
        //- Construct from dictionary
        interRegionHeatTransfer
        (
            const word& name,
            const word& modelType,
            const fvMesh& mesh,
            const dictionary& dict
        );
 
 
    //- Destructor
    virtual ~interRegionHeatTransfer();
 
 
    // Member Functions
 
        // Access
 
            //- Return the heat transfer coefficient
            inline const volScalarField& htc() const;
 
 
        // Checks
 
            //- Return the list of fields for which the fvModel adds source term
            //  to the transport equation
            virtual wordList addSupFields() const;
 
 
        // Sources
 
            //- Source term to energy equation
            virtual void addSup
            (
                fvMatrix<scalar>& eqn,
                const word& fieldName
            ) const;
 
            //- Source term to compressible energy equation
            virtual void addSup
            (
                const volScalarField& rho,
                fvMatrix<scalar>& eqn,
                const word& fieldName
            ) const;
 
 
        // Correction
 
            //- Correct the model
            virtual void correct();
 
 
        // Mesh changes
 
            //- Update for mesh motion
            virtual bool movePoints();
 
            //- Update topology using the given map
            virtual void topoChange(const polyTopoChangeMap&);
 
            //- Update from another mesh using the given map
            virtual void mapMesh(const polyMeshMap&);
 
            //- Redistribute or update using the given distribution map
            virtual void distribute(const polyDistributionMap&);
 
 
        // IO
 
            //- Read dictionary
            virtual bool read(const dictionary& dict);
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace fv
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //