supersonicFreestreamFvPatchVectorField.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) 2011-2022 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::supersonicFreestreamFvPatchVectorField

Description
    This boundary condition provides a supersonic free-stream condition.

    - supersonic outflow is vented according to ???
    - supersonic inflow is assumed to occur according to the Prandtl-Meyer
      expansion process.
    - subsonic outflow is applied via a zero-gradient condition from inside
      the domain.

Usage
    \table
        Property     | Description             | Required    | Default value
        T            | Temperature field name  | no          | T
        p            | Pressure field name     | no          | p
        psi          | Compressibility field name | no       | thermo:psi
        UInf         | free-stream velocity    | yes         |
        pInf         | free-stream pressure    | yes         |
        TInf         | free-stream temperature | yes         |
        gamma        | heat capacity ratio (cp/Cv) | yes     |
    \endtable

    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            supersonicFreestream;
        UInf            500;
        pInf            1e4;
        TInf            265;
        gamma           1.4;
    }
    \endverbatim

    Note:
        This boundary condition is ill-posed if the free-stream flow is normal
        to the boundary.

SourceFiles
    supersonicFreestreamFvPatchVectorField.C

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

#ifndef supersonicFreestreamFvPatchVectorField_H
#define supersonicFreestreamFvPatchVectorField_H

#include "fvPatchFields.H"
#include "mixedFvPatchFields.H"

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

namespace Foam
{

/*---------------------------------------------------------------------------*\
           Class supersonicFreestreamFvPatchVectorField Declaration
\*---------------------------------------------------------------------------*/

class supersonicFreestreamFvPatchVectorField
:
    public mixedFvPatchVectorField
{
    // Private Data

        //- Name of temperature field, default = "T"
        word TName_;

        //- Name of pressure field, default = "p"
        word pName_;

        //- Name of compressibility field field, default = "thermo:psi"
        word psiName_;

        //- Velocity of the free stream
        vector UInf_;

        //- Pressure of the free stream
        scalar pInf_;

        //- Temperature of the free stream
        scalar TInf_;

        //- Heat capacity ratio
        scalar gamma_;


public:

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


    // Constructors

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

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

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

        //- Disallow copy without setting internal field reference
        supersonicFreestreamFvPatchVectorField
        (
            const supersonicFreestreamFvPatchVectorField&
        ) = delete;

        //- Copy constructor setting internal field reference
        supersonicFreestreamFvPatchVectorField
        (
            const supersonicFreestreamFvPatchVectorField&,
            const DimensionedField<vector, volMesh>&
        );

        //- Construct and return a clone setting internal field reference
        virtual tmp<fvPatchVectorField> clone
        (
            const DimensionedField<vector, volMesh>& iF
        ) const
        {
            return tmp<fvPatchVectorField>
            (
                new supersonicFreestreamFvPatchVectorField(*this, iF)
            );
        }


    // Member Functions

        // Access

            //- Return the velocity at infinity
            const vector& UInf() const
            {
                return UInf_;
            }

            //- Return reference to the velocity at infinity to allow adjustment
            vector& UInf()
            {
                return UInf_;
            }

            //- Return the pressure at infinity
            scalar pInf() const
            {
                return pInf_;
            }

            //- Return reference to the pressure at infinity to allow adjustment
            scalar& pInf()
            {
                return pInf_;
            }

            //- Return the temperature at infinity
            scalar TInf() const
            {
                return TInf_;
            }

            //- Return reference to the temperature at infinity
            //  to allow adjustment
            scalar& TInf()
            {
                return TInf_;
            }


        // Evaluation functions

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


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


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

} // End namespace Foam

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

#endif

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