/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2016-2018 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/>.

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

#include "myWallHeatTransferCoeff.H"
#include "turbulentFluidThermoModel.H"
#include "solidThermo.H"
#include "surfaceInterpolate.H"
#include "fvcSnGrad.H"
#include "wallPolyPatch.H"
#include "addToRunTimeSelectionTable.H"

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

namespace Foam
{
namespace functionObjects
{
    defineTypeNameAndDebug(myWallHeatTransferCoeff, 0);
    addToRunTimeSelectionTable(functionObject, myWallHeatTransferCoeff, dictionary);
}
}

// * * * * * * * * * * * * * Protected Member Functions  * * * * * * * * * * //

void Foam::functionObjects::myWallHeatTransferCoeff::writeFileHeader(const label i)
{
    // Add headers to output data
    writeHeader(file(), "Wall HTC");
    writeCommented(file(), "Time");
    writeTabbed(file(), "patch");
    writeTabbed(file(), "min");
    writeTabbed(file(), "max");
    writeTabbed(file(), "integral");
    file() << endl;
}


Foam::tmp<Foam::volScalarField>
Foam::functionObjects::myWallHeatTransferCoeff::calcMyWallHeatTransferCoeff
(
    const volScalarField& alpha,
    const volScalarField& he,
    const volScalarField& T,
    scalar Tref
)
{
    tmp<volScalarField> tmyWallHeatTransferCoeff
    (
        volScalarField::New
        (
            type(),
            mesh_,
            dimensionedScalar(dimMass/(pow3(dimTime)*dimTemperature), 0)
        )
    );

    volScalarField::Boundary& myWallHeatTransferCoeffBf =
        tmyWallHeatTransferCoeff.ref().boundaryFieldRef();

    const volScalarField::Boundary& heBf =
        he.boundaryField();

    const volScalarField::Boundary& alphaBf =
        alpha.boundaryField();

    const volScalarField::Boundary& TBf =
        T.boundaryField();

    forAll(myWallHeatTransferCoeffBf, patchi)
    {
        if (!myWallHeatTransferCoeffBf[patchi].coupled())
        {
            myWallHeatTransferCoeffBf[patchi] = alphaBf[patchi]*heBf[patchi].snGrad()/(TBf[patchi]-Tref+ROOTVSMALL);
        }
    }

    if (foundObject<volScalarField>("qr"))
    {
        const volScalarField& qr = lookupObject<volScalarField>("qr");

        const volScalarField::Boundary& radHeatFluxBf =
            qr.boundaryField();

        forAll(myWallHeatTransferCoeffBf, patchi)
        {
            if (!myWallHeatTransferCoeffBf[patchi].coupled())
            {
                myWallHeatTransferCoeffBf[patchi]= (alphaBf[patchi]*heBf[patchi].snGrad()-radHeatFluxBf[patchi])/(TBf[patchi]-Tref+ROOTVSMALL);
            }
        }
    }

    return tmyWallHeatTransferCoeff;
}


// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::functionObjects::myWallHeatTransferCoeff::myWallHeatTransferCoeff
(
    const word& name,
    const Time& runTime,
    const dictionary& dict
)
:
    fvMeshFunctionObject(name, runTime, dict),
    logFiles(obr_, name),
    writeLocalObjects(obr_, log),
    patchSet_()
{
    read(dict);
    resetName(typeName);
    resetLocalObjectName(typeName);
}


// * * * * * * * * * * * * * * * * Destructor  * * * * * * * * * * * * * * * //

Foam::functionObjects::myWallHeatTransferCoeff::~myWallHeatTransferCoeff()
{}


// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //

bool Foam::functionObjects::myWallHeatTransferCoeff::read(const dictionary& dict)
{
    fvMeshFunctionObject::read(dict);
    writeLocalObjects::read(dict);

    Tref = dict.lookupOrDefault<scalar>("Tref", 0);

    const polyBoundaryMesh& pbm = mesh_.boundaryMesh();

    patchSet_ =
        mesh_.boundaryMesh().patchSet
        (
            wordReList(dict.lookupOrDefault("patches", wordReList()))
        );

    Info<< type() << " " << name() << ":" << nl;

    if (patchSet_.empty())
    {
        forAll(pbm, patchi)
        {
            if (isA<wallPolyPatch>(pbm[patchi]))
            {
                patchSet_.insert(patchi);
            }
        }

        Info<< "    processing all wall patches" << nl << endl;
    }
    else
    {
        Info<< "    processing wall patches: " << nl;
        labelHashSet filteredPatchSet;
        forAllConstIter(labelHashSet, patchSet_, iter)
        {
            label patchi = iter.key();
            if (isA<wallPolyPatch>(pbm[patchi]))
            {
                filteredPatchSet.insert(patchi);
                Info<< "        " << pbm[patchi].name() << endl;
            }
            else
            {
                WarningInFunction
                    << "Requested wall HTC on non-wall boundary "
                    << "type patch: " << pbm[patchi].name() << endl;
            }
        }

        Info<< endl;

        patchSet_ = filteredPatchSet;
    }

    return true;
}


bool Foam::functionObjects::myWallHeatTransferCoeff::execute()
{
    word name(type());

    if
    (
        foundObject<compressible::turbulenceModel>
        (
            turbulenceModel::propertiesName
        )
    )
    {
        const compressible::turbulenceModel& turbModel =
            lookupObject<compressible::turbulenceModel>
            (
                turbulenceModel::propertiesName
            );

        return store
        (
            name,
            calcMyWallHeatTransferCoeff(turbModel.alphaEff(), turbModel.transport().he(), turbModel.transport().T(), Tref)
        );
    }
    else if (foundObject<solidThermo>(solidThermo::dictName))
    {
        const solidThermo& thermo =
            lookupObject<solidThermo>(solidThermo::dictName);

        return store(name, calcMyWallHeatTransferCoeff(thermo.alpha(), thermo.he(), thermo.T(), Tref));
    }
    else
    {
        FatalErrorInFunction
            << "Unable to find compressible turbulence model in the "
            << "database" << exit(FatalError);
    }

    return true;
}


bool Foam::functionObjects::myWallHeatTransferCoeff::write()
{
    Log << type() << " " << name() << " write:" << nl;

    writeLocalObjects::write();

    logFiles::write();

    const volScalarField& myWallHeatTransferCoeff =
        obr_.lookupObject<volScalarField>(type());

    const fvPatchList& patches = mesh_.boundary();

    const surfaceScalarField::Boundary& magSf =
        mesh_.magSf().boundaryField();

    forAllConstIter(labelHashSet, patchSet_, iter)
    {
        label patchi = iter.key();
        const fvPatch& pp = patches[patchi];

        const scalarField& hfp = myWallHeatTransferCoeff.boundaryField()[patchi];

        const scalar minHfp = gMin(hfp);
        const scalar maxHfp = gMax(hfp);
        const scalar integralHfp = gSum(magSf[patchi]*hfp);

        if (Pstream::master())
        {
            file()
                << mesh_.time().value()
                << tab << pp.name()
                << tab << minHfp
                << tab << maxHfp
                << tab << integralHfp
                << endl;
        }

        Log << "    min/max/integ(" << pp.name() << ") = "
            << minHfp << ", " << maxHfp << ", " << integralHfp << endl;
    }

    Log << endl;

    return true;
}


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

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2016-2019 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::functionObjects::myWallHeatTransferCoeff

Description
    Calculates and write the HTC based on a fixed reference temperature

    \f[
            h = \frac{q}{T_{ref} - T_W}
    \f]

    at wall patches as the volScalarField field 'myWallHeatTransferCoeff'.

    All wall patches are included by default; to restrict the calculation to
    certain patches, use the optional 'patches' entry.

    Example of function object specification:
    \verbatim
    myWallHeatTransferCoeff1
    {
        type        myWallHeatTransferCoeff;
        libs        ("libfieldFunctionObjects.so");
        ...
        Tref        293;
        region      fluid;
        patches     (".*Wall");
    }
    \endverbatim

Usage
    \table
        Property | Description                        | Required   | Default value
        type     | type name: myWallHeatTransferCoeff | yes        |
        Tref     | reference temperature              | no         | 0
        patches  | list of patches to process         | no         | all wall patches
        region   | region to be evaluated             | no         | default region
    \endtable

Note
    Writing field 'myWallHeatTransferCoeff' is done by default, but it can be overridden by
    defining an empty \c objects list. For details see writeLocalObjects.

See also
    Foam::functionObject
    Foam::functionObjects::fvMeshFunctionObject
    Foam::functionObjects::logFiles
    Foam::functionObjects::writeLocalObjects
    Foam::functionObjects::timeControl

SourceFiles
    myWallHeatTransferCoeff.C

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

#ifndef functionObjects_myWallHeatTransferCoeff_H
#define functionObjects_myWallHeatTransferCoeff_H

#include "fvMeshFunctionObject.H"
#include "logFiles.H"
#include "writeLocalObjects.H"
#include "HashSet.H"
#include "volFieldsFwd.H"

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

namespace Foam
{
namespace functionObjects
{

/*---------------------------------------------------------------------------*\
                       Class myWallHeatTransferCoeff Declaration
\*---------------------------------------------------------------------------*/

class myWallHeatTransferCoeff
:
    public fvMeshFunctionObject,
    public logFiles,
    public writeLocalObjects
{
    // Private Data

    //- Optional Tref (default is 0)
    scalar Tref;

protected:

    // Protected data

        //- Optional list of patches to process
        labelHashSet patchSet_;


    // Protected Member Functions

        //- File header information
        virtual void writeFileHeader(const label i);

        //- Calculate the HTC
        tmp<volScalarField> calcMyWallHeatTransferCoeff
        (
            const volScalarField& alpha,
            const volScalarField& he,
            const volScalarField& T,
            scalar Tref
        );


public:

    //- Runtime type information
    TypeName("myWallHeatTransferCoeff");


    // Constructors

        //- Construct from Time and dictionary
        myWallHeatTransferCoeff
        (
            const word& name,
            const Time& runTime,
            const dictionary&
        );

        //- Disallow default bitwise copy construction
        myWallHeatTransferCoeff(const myWallHeatTransferCoeff&) = delete;


    //- Destructor
    virtual ~myWallHeatTransferCoeff();


    // Member Functions

        //- Read the myWallHeatTransferCoeff data
        virtual bool read(const dictionary&);

        //- Calculate the wall HTC
        virtual bool execute();

        //- Write the wall HTC
        virtual bool write();


    // Member Operators

        //- Disallow default bitwise assignment
        void operator=(const myWallHeatTransferCoeff&) = delete;
};


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

} // End namespace functionObjects
} // End namespace Foam

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

#endif

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