freestreamPressureFvPatchScalarField.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::freestreamPressureFvPatchScalarField
 
Description
    This boundary condition provides a free-stream condition for pressure.
 
    It is an outlet-inlet condition that uses the velocity orientation to
    continuously blend between zero gradient for normal inlet and fixed value
    for normal outlet flow.
 
Usage
    \table
        Property        | Description                | Required | Default value
        U               | velocity field name        | no       | U
        freestreamValue | freestream pressure        | yes      |
        supersonic      | Switch for supersonic flow | no       | false
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            freestreamPressure;
        freestreamValue uniform 1e5;
    }
    \endverbatim
 
    Note:
        This condition is designed to operate with a freestreamVelocity
        condition
 
See also
    Foam::mixedFvPatchField
    Foam::freestreamFvPatchField
 
SourceFiles
    freestreamPressureFvPatchScalarField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef freestreamPressureFvPatchScalarField_H
#define freestreamPressureFvPatchScalarField_H
 
#include "fvPatchFields.H"
#include "mixedFvPatchFields.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
            Class freestreamPressureFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
 
class freestreamPressureFvPatchScalarField
:
    public mixedFvPatchScalarField
{
    // Private Data
 
        //- Name of the velocity field
        word UName_;
 
        //- Set true for supersonic freestream
        Switch supersonic_;
 
 
public:
 
    //- Runtime type information
    TypeName("freestreamPressure");
 
 
    // Constructors
 
        //- Construct from patch, internal field and dictionary
        freestreamPressureFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given freestreamPressureFvPatchScalarField onto
        //  a new patch
        freestreamPressureFvPatchScalarField
        (
            const freestreamPressureFvPatchScalarField&,
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const fieldMapper&
        );
 
        //- Disallow copy without setting internal field reference
        freestreamPressureFvPatchScalarField
        (
            const freestreamPressureFvPatchScalarField&
        ) = delete;
 
        //- Copy constructor setting internal field reference
        freestreamPressureFvPatchScalarField
        (
            const freestreamPressureFvPatchScalarField&,
            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 freestreamPressureFvPatchScalarField(*this, iF)
            );
        }
 
 
    // Member Functions
 
            const scalarField& freestreamValue() const
            {
                return refValue();
            }
 
            scalarField& freestreamValue()
            {
                return refValue();
            }
 
 
        // Evaluation functions
 
            //- Update the coefficients associated with the patch field
            virtual void updateCoeffs();
 
 
        //- Write
        virtual void write(Ostream&) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //