/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2016 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::
        turbulentTemperatureCoupledBaffleMixedFvPatchScalarField

Description
    Mixed boundary condition for temperature, to be used for heat-transfer
    on back-to-back baffles. Optional thin thermal layer resistances can be
    specified through thicknessLayers and kappaLayers entries.

    The thermal conductivity, \c kappa, can either be retrieved from the
    mesh database using the \c lookup option, or from a \c solidThermo
    or \c fluidThermo thermophysical package.

    Specifies gradient and temperature such that the equations are the same
    on both sides:
      - refGradient = zero gradient
      - refValue = neighbour value
      - mixFraction = nbrKDelta / (nbrKDelta + myKDelta())

    where KDelta is heat-transfer coefficient K * deltaCoeffs

Usage
    \table
        Property     | Description             | Required    | Default value
        kappa        | thermal conductivity option | yes     |
        kappaName    | name of thermal conductivity field | no  |
        Tnbr         | name of the field    | no | T
        thicknessLayers | list of thicknesses per layer [m] | no |
        kappaLayers  | list of thermal conductivites per layer [W/m/K] | no |
    \endtable

    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        Tnbr            T;
        kappa           lookup;
        kappaName       kappa;
        thicknessLayers (0.1 0.2 0.3 0.4);
        kappaLayers     (1 2 3 4);
        value           uniform 300;
    }
    \endverbatim

    Needs to be on underlying mapped(Wall)FvPatch.

    Note:
      - \c kappa and \c kappaName are inherited from temperatureCoupledBase.


See also
    Foam::temperatureCoupledBase

SourceFiles
    turbulentTemperatureCoupledBaffleMixedFvPatchScalarField.C

\*---------------------------------------------------------------------------*/

#ifndef turbulentTemperatureCoupledBaffleMixedFvPatchScalarField_H
#define turbulentTemperatureCoupledBaffleMixedFvPatchScalarField_H

#include "mixedFvPatchFields.H"
#include "temperatureCoupledBase.H"
#include "scalarField.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

namespace Foam
{
namespace compressible
{

/*---------------------------------------------------------------------------*\
   Class turbulentTemperatureCoupledBaffleMixedFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/

class turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
:
    public mixedFvPatchScalarField,
    public temperatureCoupledBase
{
    // Private data

        //- Name of field on the neighbour region
        const word TnbrName_;

        //- Thickness of layers
        scalarList thicknessLayers_;

        //- Conductivity of layers
        scalarList kappaLayers_;

        //- Total contact resistance
        scalar contactRes_;


public:

    //- Runtime type information
    TypeName("compressible::turbulentTemperatureCoupledBaffleMixed");


    // Constructors

        //- Construct from patch and internal field
        turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&
        );

        //- Construct from patch, internal field and dictionary
        turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const dictionary&
        );

        //- Construct by mapping given
        //  turbulentTemperatureCoupledBaffleMixedFvPatchScalarField onto a
        //  new patch
        turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
        (
            const turbulentTemperatureCoupledBaffleMixedFvPatchScalarField&,
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const fvPatchFieldMapper&
        );

        //- Construct and return a clone
        virtual tmp<fvPatchScalarField> clone() const
        {
            return tmp<fvPatchScalarField>
            (
                new turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
                (
                    *this
                )
            );
        }

        //- Construct as copy setting internal field reference
        turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
        (
            const turbulentTemperatureCoupledBaffleMixedFvPatchScalarField&,
            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 turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
                (
                    *this,
                    iF
                )
            );
        }


    // Member functions

        //- Update the coefficients associated with the patch field
        virtual void updateCoeffs();

        //- Write
        virtual void write(Ostream&) const;
};


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

} // End namespace compressible
} // End namespace Foam

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

// ************************************************************************* //
