convectiveHeatTransferFvPatchScalarField.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::compressible::convectiveHeatTransferFvPatchScalarField
 
Description
    This boundary condition provides a convective heat transfer coefficient
    condition
 
    if Re > 500000
    \f[
        htc_p = \frac{0.664 Re^{0.5} Pr^{0.333} \kappa_p}{L}
    \f]
    else
    \f[
        htc_p = \frac{0.037 Re^{0.8} Pr^{0.333} \kappa_p}{L}
    \f]
 
    where
 
    \vartable
        htc_p   | patch convective heat transfer coefficient
        Re      | Reynolds number
        Pr      | Prandtl number
        \kappa_p | thermal conductivity
        L       | length scale
    \endvartable
 
Usage
    \table
        Property     | Description             | Required    | Default value
        L            | Length scale [m]        | yes |
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            convectiveHeatTransfer;
        L               0.1;
    }
    \endverbatim
 
See also
    Foam::fixedValueFvPatchField
 
SourceFiles
    convectiveHeatTransferFvPatchScalarField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef convectiveHeatTransferFvPatchScalarField_H
#define convectiveHeatTransferFvPatchScalarField_H
 
#include "fixedValueFvPatchFields.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
namespace compressible
{
 
/*---------------------------------------------------------------------------*\
          Class convectiveHeatTransferFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
 
class convectiveHeatTransferFvPatchScalarField
:
    public fixedValueFvPatchScalarField
{
protected:
 
    // Protected data
 
        //- L Length scale [m]
        const scalar L_;
 
 
public:
 
    //- Runtime type information
    TypeName("convectiveHeatTransfer");
 
 
    // Constructors
 
        //- Construct from patch, internal field and dictionary
        convectiveHeatTransferFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given
        //  convectiveHeatTransferFvPatchScalarField
        //  onto a new patch
        convectiveHeatTransferFvPatchScalarField
        (
            const convectiveHeatTransferFvPatchScalarField&,
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const fvPatchFieldMapper&
        );
 
        //- Disallow copy without setting internal field reference
        convectiveHeatTransferFvPatchScalarField
        (
            const convectiveHeatTransferFvPatchScalarField&
        ) = delete;
 
        //- Copy constructor setting internal field reference
        convectiveHeatTransferFvPatchScalarField
        (
            const convectiveHeatTransferFvPatchScalarField&,
            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 convectiveHeatTransferFvPatchScalarField(*this, iF)
            );
        }
 
 
    // Member Functions
 
        // Evaluation functions
 
            //- Update the coefficients associated with the patch field
            virtual void updateCoeffs();
 
 
        // I-O
 
            //- Write
            virtual void write(Ostream&) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace compressible
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //