heatTransferCoeff.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | www.openfoam.com
     \\/     M anipulation  |
-------------------------------------------------------------------------------
    Copyright (C) 2017-2020 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::functionObjects::heatTransferCoeff
 
Group
    grpFieldFunctionObjects
 
Description
    Computes the heat transfer coefficient [W/(m2 K)]
    as a \c volScalarField for a given set of patches.
 
    Optionally, the Nusselt number (i.e. the ratio of convective
    to conductive heat transfer at a boundary in a fluid) can be output:
 
    \f[
        Nu = \frac{h L}{\kappa}
    \f]
 
    where
    \vartable
      Nu | Nusselt number
      h  | Convective heat transfer coefficient of the flow
      L  | Characteristic length that defines the scale of the physical system
      \kappa | Thermal conductivity of the fluid
    \endvartable
 
    Operands:
    \table
      Operand           | Type           | Location
      input             | -              | -
      output file       | -              | -
      output field      | volScalarField | $FOAM_CASE/<time>/<outField>
    \endtable
 
Usage
    Minimal example by using \c system/controlDict.functions:
    \verbatim
    heatTransferCoeff1
    {
        // Mandatory entries (unmodifiable)
        type        heatTransferCoeff;
        libs        (fieldFunctionObjects);
 
        // Mandatory (inherited) entries (runtime modifiable)
        field       <field>;
        patches     (<patch1> <patch2> ... <patchN>);
        htcModel    <htcModel>;
 
        // Optional entries (runtime modifable)
        qr          <qrName>;
        L           1.0;
        kappa       1.0;
 
        // Conditional mandatory and optional
        // entries based on selected <htcModel> (runtime modifiable)
        ...
 
        // Optional (inherited) entries
        ...
    }
    \endverbatim
 
    where the entries mean:
    \table
      Property    | Description                        | Type | Reqd | Dflt
      type        | Type name: heatTransferCoeff       | word | yes  | -
      libs        | Library name: fieldFunctionObjects | word | yes  | -
      field       | Name of the operand field          | word | yes  | -
      patches     | Names of operand patches        | wordRes | yes  | -
      htcModel    | Heat transfer coefficient model <!--
                -->                        - see below | word | yes  | -
      qr          | Name of radiative heat flux        | word | no   | qr
      L           | Characteristic length that defines <!--
                --> the scale of the physical system | scalar | no   | 1
      kappa       | Thermal conductivity of fluid    | scalar | no   | 1
    \endtable
 
    The inherited entries are elaborated in:
      - \link functionObject.H \endlink
      - \link fieldExpression.H \endlink
      - \link heatTransferCoeffModel.H \endlink
 
    Options for the \c htcModel entry:
    \verbatim
      ReynoldsAnalogy           | Reynold's analogy
      localReferenceTemperature | Local reference temperature
      fixedReferenceTemperature | Specified reference temperature
    \endverbatim
 
    Usage by the \c postProcess utility is not available.
 
See also
  - Foam::functionObject
  - Foam::functionObjects::fieldExpression
  - Foam::heatTransferCoeffModels::fixedReferenceTemperature
  - Foam::heatTransferCoeffModels::localReferenceTemperature
  - Foam::heatTransferCoeffModels::ReynoldsAnalogy
  - ExtendedCodeGuide::functionObjects::field::heatTransferCoeff
 
SourceFiles
    heatTransferCoeff.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef functionObjects_heatTransferCoeff_H
#define functionObjects_heatTransferCoeff_H
 
#include "fieldExpression.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
// Forward Declarations
class heatTransferCoeffModel;
 
namespace functionObjects
{
 
/*---------------------------------------------------------------------------*\
                      Class heatTransferCoeff Declaration
\*---------------------------------------------------------------------------*/
 
class heatTransferCoeff
:
    public fieldExpression
{
    // Private Data
 
        //- Characteristic length that defines the scale of the physical system
        scalar L_;
 
        //- Thermal conductivity of the fluid
        scalar kappa_;
 
        //- Heat transfer coefficient model
        autoPtr<heatTransferCoeffModel> htcModelPtr_;
 
 
protected:
 
        //- Calculate the heat transfer coefficient field and return true
        //- if successful
        virtual bool calc();
 
 
public:
 
    //- Runtime type information
    TypeName("heatTransferCoeff");
 
 
    // Constructors
 
        //- No default construct
        heatTransferCoeff() = delete;
 
        //- Construct for given objectRegistry and dictionary.
        //  Allow the possibility to load fields from files
        heatTransferCoeff
        (
            const word& name,
            const Time& runTime,
            const dictionary& dict
        );
 
        //- No copy construct
        heatTransferCoeff(const heatTransferCoeff&) = delete;
 
        //- No copy assignment
        void operator=(const heatTransferCoeff&) = delete;
 
 
    //- Destructor
    virtual ~heatTransferCoeff() = default;
 
 
    // Member Functions
 
        //- Read the heatTransferCoeff data
        virtual bool read(const dictionary& dict);
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace functionObjects
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //