File size: 6,599 Bytes
5a600cf | 1 2 3 4 5 6 7 8 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 51 52 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 | /*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Copyright (C) 2017-2026 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::flowRateOutletVelocityFvPatchVectorField
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 |
rho | Density field name | no | rho
rhoOutlet | Outlet density | no |
\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 volumetricFlowRate or \c massFlowRate entry is a \c Function1 of
time, see Foam::Function1s.
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::Function1s
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 the flow-rate volumetric?
bool volumetric_;
//- Name of the density field used to normalise 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, internal field and dictionary
flowRateOutletVelocityFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, fvMesh>&,
const dictionary&
);
//- Construct by mapping given
// flowRateOutletVelocityFvPatchVectorField
// onto a new patch
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField&,
const fvPatch&,
const DimensionedField<vector, fvMesh>&,
const fieldMapper&
);
//- Disallow copy without setting internal field reference
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField&
) = delete;
//- Copy constructor setting internal field reference
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField&,
const DimensionedField<vector, fvMesh>&
);
//- Construct and return a clone setting internal field reference
virtual tmp<fvPatchVectorField> clone
(
const DimensionedField<vector, fvMesh>& 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;
// Member Operators
//- Inherit assignment
using fixedValueFvPatchVectorField::operator=;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //
|