flowRateOutletVelocityFvPatchVectorField.H 6.8 KB
Newer Older
1 2 3 4
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
OpenFOAM bot's avatar
OpenFOAM bot committed
5
    \\  /    A nd           | www.openfoam.com
6
     \\/     M anipulation  |
OpenFOAM bot's avatar
OpenFOAM bot committed
7
-------------------------------------------------------------------------------
OpenFOAM bot's avatar
OpenFOAM bot committed
8
    Copyright (C) 2017 OpenFOAM Foundation
9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50
-------------------------------------------------------------------------------
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::flowRateOutletVelocityFvPatchVectorField

Group
    grpOutletBoundaryConditions

Description
    Velocity outlet boundary condition which corrects the extrapolated velocity
    to match the specified flow rate.

    For a mass-based flux:
    - the flow rate should be provided in kg/s
    - if \c rho is "none" the flow rate is in m^3/s
    - otherwise \c rho should correspond to the name of the density field
    - if the density field cannot be found in the database, the user must
      specify the outlet density using the \c rhoOutlet entry

    For a volumetric-based flux:
    - the flow rate is in m^3/s

Usage
    \table
        Property     | Description             | Required    | Default value
        massFlowRate | mass flow rate [kg/s]   | no          |
        volumetricFlowRate | volumetric flow rate [m^3/s]| no |
51 52
        rho          | density field name      | no          | rho
        rhoOutlet    | outlet density          | no          |
53 54 55 56 57 58 59 60 61 62 63 64 65 66 67 68 69 70 71 72 73 74 75 76 77 78 79 80 81 82 83 84 85 86 87 88 89 90 91 92 93 94 95 96 97 98 99 100 101 102 103 104 105 106 107 108 109 110 111 112 113 114 115 116 117 118 119 120 121 122 123 124 125 126 127 128 129 130 131 132 133 134 135 136 137 138 139 140 141 142 143 144 145 146 147 148 149 150 151 152 153 154 155 156 157 158 159 160 161 162 163 164 165 166 167 168 169 170 171 172 173 174 175 176 177 178 179 180 181 182 183 184 185 186 187 188 189 190 191 192 193 194 195 196 197 198 199 200 201 202 203 204 205 206 207 208 209 210 211 212 213 214 215 216 217 218 219 220 221 222 223
    \endtable

    Example of the boundary condition specification for a volumetric flow rate:
    \verbatim
    <patchName>
    {
        type                flowRateOutletVelocity;
        volumetricFlowRate  0.2;
        value               uniform (0 0 0);
    }
    \endverbatim

    Example of the boundary condition specification for a mass flow rate:
    \verbatim
    <patchName>
    {
        type                flowRateOutletVelocity;
        massFlowRate        0.2;
        rhoOutlet           1.0;
        value               uniform (0 0 0);
    }
    \endverbatim

    The \c flowRate entry is a \c Function1 of time, see Foam::Function1Types.

Note
    - \c rhoOutlet is required for the case of a mass flow rate, where the
      density field is not available at start-up
    - The value is positive out of the domain (as an outlet)
    - May not work correctly for transonic outlets
    - Strange behaviour with potentialFoam since the U equation is not solved

See also
    Foam::fixedValueFvPatchField
    Foam::Function1Types
    Foam::flowRateInletVelocityFvPatchVectorField

SourceFiles
    flowRateOutletVelocityFvPatchVectorField.C

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

#ifndef flowRateOutletVelocityFvPatchVectorField_H
#define flowRateOutletVelocityFvPatchVectorField_H

#include "fixedValueFvPatchFields.H"
#include "Function1.H"

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

namespace Foam
{

/*---------------------------------------------------------------------------*\
           Class flowRateOutletVelocityFvPatchVectorField Declaration
\*---------------------------------------------------------------------------*/

class flowRateOutletVelocityFvPatchVectorField
:
    public fixedValueFvPatchVectorField
{
    // Private data

        //- Outlet integral flow rate
        autoPtr<Function1<scalar>> flowRate_;

        //- Is volumetric?
        bool volumetric_;

        //- Name of the density field used to normalize the mass flux
        word rhoName_;

        //- Rho initialisation value (for start; if value not supplied)
        scalar rhoOutlet_;


    // Private member functions

        //- Update the patch values given the appropriate density type and value
        template<class RhoType>
        void updateValues(const RhoType& rho);


public:

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


   // Constructors

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

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

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

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

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

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


    // Member functions

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

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


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

} // End namespace Foam

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

#endif

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