tabulatedNTUHeatTransfer.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2015 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::fv::tabulatedNTUHeatTransfer
 
Description
    Tabulated heat transfer model.
 
    The heat flux is calculated based on the Number of Thermal Units (NTU).
    A 2-D table of NTU as functions of the primary and secondary mass flow
    rates is required.
 
    The exchanger geometry can be specified using either:
    - \c calculated:
        - inlet area of each region and core volume determined by interrogating
          mesh patches, and mesh-to-mesh interpolation volume
        - calculated core volume canbe partially blocked by specifying a
          \c coreBlockageRatio [0-1] entry
    - \c user:
        - inlet area of each region privided by the user
        - core volume automatically calculated by the mesh-to-mesh
          interpolation volume if not provided by user
 
    Heat transfer coefficient calculated by:
 
    \f[
        htc = C_{min} \frac{NTU}{V_{core}}
    \f]
 
    Where \f$ C_{min} \f$ is given by:
 
    \f[
        C_{min} = min \left(Cp_1 \dot{m}_1, Cp_2 \dot{m}_2 \right)
    \f]
 
    \heading Example usage
 
    \verbatim
    coolerToAir
    {
        type            tabulatedNTUHeatTransfer;
        active          yes;
 
        tabulatedNTUHeatTransferCoeffs
        {
            interpolationMethod cellVolumeWeight;
            nbrRegionName   air;
            master          true;
 
            fieldNames      (h);
            outOfBounds     clamp;
            fileName        "ntuTable";
            nbrModelName    airToCooler;
            semiImplicit    no;
 
 
            geometryMode    user;
            Ain             0.01728;
            AinNbr          0.3456;
            Vcore           0.01244;  // Optional
    
            // geometryMode    calculated;
            // inletPatch      inlet_HWK;
            // inletPatchNbr   inlet_air;
            // inletBlockageRatio 0.10;
            // inletBlockageRatioNbr 0.04;
            // coreBlockageRatio 0;
        }
    }
 
SourceFiles
    tabulatedNTUHeatTransfer.C
 
SeeAlso
    interRegionHeatTransferModel.H
 
\*---------------------------------------------------------------------------*/
 
#ifndef tabulatedNTUHeatTransfer_H
#define tabulatedNTUHeatTransfer_H
 
#include "interRegionHeatTransferModel.H"
#include "autoPtr.H"
#include "interpolation2DTable.H"
#include "NamedEnum.H"
#include "basicThermo.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
namespace fv
{
 
/*---------------------------------------------------------------------------*\
                  Class tabulatedNTUHeatTransfer Declaration
\*---------------------------------------------------------------------------*/
 
class tabulatedNTUHeatTransfer
:
    public interRegionHeatTransferModel
{
public:
 
    // Public enumerations
 
        enum geometryModeType
        {
            gmCalculated,
            gmUser
        };
 
        static const NamedEnum<geometryModeType, 2> geometryModelNames_;
 
 
private:
 
    // Private data
 
        //- Name of velocity field; default = U
        word UName_;
 
        //- Name of neighbour velocity field; default = U
        word UNbrName_;
 
        //- Name of density field; default = rho
        word rhoName_;
 
        //- Name of neighbour density field; default = rho
        word rhoNbrName_;
 
        //- Pointer to 2-D look-up table of NTU f(mDot1, mDot2)
        autoPtr<interpolation2DTable<scalar> > ntuTable_;
 
        //- Geometry input mode
        geometryModeType geometryMode_;
 
        //- Inlet area [m2]
        scalar Ain_;
 
        //- Neighbour region inlet area [m2]
        scalar AinNbr_;
 
        //- Heat exchanger core volume
        scalar Vcore_;
 
 
    // Private Member functions
 
        //- NTU table helper
        const interpolation2DTable<Foam::scalar>& ntuTable();
 
        //- Thermophysical properties helper
        const basicThermo& thermo(const fvMesh& mesh) const;
 
        //- Initialise geometry
        void initialiseGeometry();
 
 
public:
 
    //- Runtime type information
    TypeName("tabulatedNTUHeatTransfer");
 
 
    // Constructors
 
        //- Construct from dictionary
        tabulatedNTUHeatTransfer
        (
            const word& name,
            const word& modelType,
            const dictionary& dict,
            const fvMesh& mesh
        );
 
 
    //- Destructor
    virtual ~tabulatedNTUHeatTransfer();
 
 
    // Public Functions
 
        //- Calculate the heat transfer coefficient
        virtual void calculateHtc();
 
 
        // I-O
 
            //- Read dictionary
            virtual bool read(const dictionary& dict);
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace fv
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //