/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | www.openfoam.com
     \\/     M anipulation  |
-------------------------------------------------------------------------------
    Copyright (C) 2011-2016 OpenFOAM Foundation
-------------------------------------------------------------------------------
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::totalPressureFvPatchScalarField

Group
    grpInletBoundaryConditions grpOutletBoundaryConditions

Description
    This boundary condition provides a total pressure condition.  Four
    variants are possible:

    1. incompressible subsonic:
        \f[
            p_p = p_0 - 0.5 |U|^2
        \f]
        where
        \vartable
            p_p     | incompressible pressure at patch [m2/s2]
            p_0     | incompressible total pressure [m2/s2]
            U       | velocity
        \endvartable

    2. compressible subsonic:
        \f[
            p_p = p_0 - 0.5 \rho |U|^2
        \f]
        where
        \vartable
            p_p     | pressure at patch [Pa]
            p_0     | total pressure [Pa]
            \rho    | density [kg/m3]
            U       | velocity
        \endvartable

    3. compressible transonic (\f$\gamma = 1\f$):
        \f[
            p_p = \frac{p_0}{1 + 0.5 \psi |U|^2}
        \f]
        where
        \vartable
            p_p     | pressure at patch [Pa]
            p_0     | total pressure [Pa]
            G       | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$
        \endvartable

    4. compressible supersonic (\f$\gamma > 1\f$):
        \f[
            p_p = \frac{p_0}{(1 + 0.5 \psi G |U|^2)^{\frac{1}{G}}}
        \f]
        where
        \vartable
            p_p     | pressure at patch [Pa]
            p_0     | total pressure [Pa]
            \gamma  | ratio of specific heats (Cp/Cv)
            \psi    | compressibility [m2/s2]
            G       | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$
        \endvartable

    The modes of operation are set by the dimensions of the pressure field
    to which this boundary condition is applied, the \c psi entry and the value
    of \c gamma:
    \table
        Mode                    | dimensions | psi   | gamma
        incompressible subsonic | p/rho      |       |
        compressible subsonic   | p          | none  |
        compressible transonic  | p          | psi   | 1
        compressible supersonic | p          | psi   | > 1
    \endtable


Usage
    \table
        Property     | Description                | Required | Default value
        U            | Velocity field name        | no       | U
        phi          | Flux field name            | no       | phi
        rho          | Density field name         | no       | rho
        psi          | Compressibility field name | no       | none
        gamma        | (Cp/Cv)                    | no       | 1
        p0           | Total pressure             | yes      |
    \endtable

    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            totalPressure;
        p0              uniform 1e5;
    }
    \endverbatim

See also
    Foam::fixedValueFvPatchField

SourceFiles
    totalPressureFvPatchScalarField.C

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

#ifndef totalPressureFvPatchScalarField_H
#define totalPressureFvPatchScalarField_H

#include "fixedValueFvPatchFields.H"

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

namespace Foam
{

/*---------------------------------------------------------------------------*\
              Class totalPressureFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/

class totalPressureFvPatchScalarField
:
    public fixedValueFvPatchScalarField
{
    // Private data

        //- Name of the velocity field
        word UName_;

        //- Name of the flux transporting the field
        word phiName_;

        //- Name of the density field used to normalise the mass flux
        //- if necessary
        word rhoName_;

        //- Name of the compressibility field used to calculate the wave speed
        word psiName_;

        //- Heat capacity ratio
        scalar gamma_;

        //- Total pressure
        scalarField p0_;


public:

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


    // Constructors

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

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

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

        //- Construct as copy
        totalPressureFvPatchScalarField
        (
            const totalPressureFvPatchScalarField&
        );

        //- Construct as copy setting internal field reference
        totalPressureFvPatchScalarField
        (
            const totalPressureFvPatchScalarField&,
            const DimensionedField<scalar, volMesh>&
        );

        //- Return a clone
        virtual tmp<fvPatchField<scalar>> clone() const
        {
            return fvPatchField<scalar>::Clone(*this);
        }

        //- Clone with an internal field reference
        virtual tmp<fvPatchField<scalar>> clone
        (
            const DimensionedField<scalar, volMesh>& iF
        ) const
        {
            return fvPatchField<scalar>::Clone(*this, iF);
        }


    // Member functions

        // Access

            //- Return the name of the velocity field
            const word& UName() const
            {
                return UName_;
            }

            //- Return reference to the name of the velocity field
            //  to allow adjustment
            word& UName()
            {
                return UName_;
            }

            //- Return the name of the flux field
            const word& phiName() const
            {
                return phiName_;
            }

            //- Return reference to the name of the flux field
            //  to allow adjustment
            word& phiName()
            {
                return phiName_;
            }

            //- Return the name of the density field
            const word& rhoName() const
            {
                return rhoName_;
            }

            //- Return reference to the name of the density field
            //  to allow adjustment
            word& rhoName()
            {
                return rhoName_;
            }

            //- Return the name of the compressibility field
            const word& psiName() const
            {
                return psiName_;
            }

            //- Return reference to the name of the compressibility field
            //  to allow adjustment
            word& psiName()
            {
                return psiName_;
            }

            //- Return the heat capacity ratio
            scalar gamma() const
            {
                return gamma_;
            }

            //- Return reference to the heat capacity ratio to allow adjustment
            scalar& gamma()
            {
                return gamma_;
            }

            //- Return the total pressure
            const scalarField& p0() const
            {
                return p0_;
            }

            //- Return reference to the total pressure to allow adjustment
            scalarField& p0()
            {
                return p0_;
            }


        // Mapping functions

            //- Map (and resize as needed) from self given a mapping object
            virtual void autoMap
            (
                const fvPatchFieldMapper&
            );

            //- Reverse map the given fvPatchField onto this fvPatchField
            virtual void rmap
            (
                const fvPatchScalarField&,
                const labelList&
            );


        // Evaluation functions

            //- Inherit updateCoeffs from fixedValueFvPatchScalarField
            using fixedValueFvPatchScalarField::updateCoeffs;

            //- Update the coefficients associated with the patch field
            //  using the given patch total pressure and velocity fields
            virtual void updateCoeffs
            (
                const scalarField& p0p,
                const vectorField& Up
            );

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


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


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

} // End namespace Foam

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

#endif

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