File size: 8,703 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 99 100 101 102 103 104 105 106 107 108 109 110 111 112 113 114 115 116 117 118 119 120 121 122 123 124 125 126 127 128 129 130 131 132 133 134 135 136 137 138 139 140 141 142 143 144 145 146 147 148 149 150 151 152 153 154 155 156 157 158 159 160 161 162 163 164 165 166 167 168 169 170 171 172 173 174 175 176 177 178 179 180 181 182 183 184 185 186 187 188 189 190 191 192 193 194 195 196 197 198 199 200 201 202 203 204 205 206 207 208 209 210 211 212 213 214 215 216 217 218 219 220 221 222 223 224 225 226 227 228 229 230 231 232 233 234 235 236 237 238 239 240 241 242 243 244 245 246 247 248 249 250 251 252 253 254 255 256 257 258 | /*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Copyright (C) 2016-2026 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::plenumPressureFvPatchScalarField
Description
This boundary condition provides a plenum pressure inlet condition. This
condition creates a zero-dimensional model of an enclosed volume of gas
upstream of the inlet. The pressure that the boundary condition exerts on
the inlet boundary is dependent on the thermodynamic state of the upstream
volume. The upstream plenum density and temperature are time-stepped along
with the rest of the simulation, and momentum is neglected. The plenum is
supplied with a user specified mass flow and temperature.
The result is a boundary condition which blends between a pressure inlet
condition condition and a fixed mass flow. The smaller the plenum
volume, the quicker the pressure responds to a deviation from the supply
mass flow, and the closer the model approximates a fixed mass flow. As
the plenum size increases, the model becomes more similar to a specified
pressure.
The expansion from the plenum to the inlet boundary is controlled by an
area ratio and a discharge coefficient. The area ratio can be used to
represent further acceleration between a sub-grid blockage such as fins.
The discharge coefficient represents a fractional deviation from an
ideal expansion process.
This condition is useful for simulating unsteady internal flow problems
for which both a mass flow boundary is unrealistic, and a pressure
boundary is susceptible to flow reversal. It was developed for use in
simulating confined combustion.
Reference:
\verbatim
Bainbridge, W. (2013).
The Numerical Simulation of Oscillations in Gas Turbine Combustion
Chambers,
PhD Thesis,
Chapter 4, Section 4.3.1.2, 77-80.
\endverbatim
Usage
\table
Property | Description | Required | Default value
gamma | ratio of specific heats | yes | none
R | specific gas constant | yes | none
supplyMassFlowRate | flow rate into the plenum | yes | none
supplyTotalTemperature | temperature into the plenum | yes | none
plenumVolume | plenum volume | yes | none
plenumDensity | plenum density | yes | none
plenumTemperature | plenum temperature | yes | none
U | velocity field name | no | U
phi | flux field name | no | phi
rho | inlet density | no | none
inletAreaRatio | inlet open fraction | yes | none
inletDischargeCoefficient | inlet loss coefficient | yes | none
timeScale | relaxation time scale | yes | none
\endtable
Example of the boundary condition specification:
\verbatim
<patchName>
{
type plenumPressure;
gamma 1.4;
R 287.04;
supplyMassFlowRate 0.0001;
supplyTotalTemperature 300;
plenumVolume 0.000125;
plenumDensity 1.1613;
plenumTemperature 300;
inletAreaRatio 1.0;
inletDischargeCoefficient 0.8;
timeScale 1e-4;
value uniform 1e5;
}
\endverbatim
SourceFiles
plenumPressureFvPatchScalarField.C
\*---------------------------------------------------------------------------*/
#ifndef plenumPressureFvPatchScalarField_H
#define plenumPressureFvPatchScalarField_H
#include "fixedValueFvPatchFields.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
/*---------------------------------------------------------------------------*\
Class plenumPressureFvPatch Declaration
\*---------------------------------------------------------------------------*/
class plenumPressureFvPatchScalarField
:
public fixedValueFvPatchScalarField
{
// Private Data
//- Ratio of specific heats
scalar gamma_;
//- Specific gas constant
scalar R_;
//- Mass flow rate supplied to the plenum
scalar supplyMassFlowRate_;
//- Total temperature of the gas supplied to the plenum
scalar supplyTotalTemperature_;
//- The volume of the plenum
scalar plenumVolume_;
//- The mean density of the gas in the plenum
scalar plenumDensity_;
//- The old-time mean density of the gas in the plenum
scalar plenumDensityOld_;
//- The mean temperature of the gas in the plenum
scalar plenumTemperature_;
//- The mean old-time temperature of the gas in the plenum
scalar plenumTemperatureOld_;
//- The constant density used when phi is volumetric
scalar rho_;
//- Whether or not the constant density has been specified
bool hasRho_;
//- The ratio of open area to total area at the inlet
// Allows a grid or mesh to be represented
scalar inletAreaRatio_;
//- The discharge coefficient at the inlet
scalar inletDischargeCoefficient_;
//- The time scale over which changes in pressure are smoothed
scalar timeScale_;
//- The time index used for updating
label timeIndex_;
//- The name of the flux field
word phiName_;
//- The name of the velocity field
word UName_;
public:
//- Runtime type information
TypeName("plenumPressure");
// Constructors
//- Construct from patch, internal field and dictionary
plenumPressureFvPatchScalarField
(
const fvPatch&,
const DimensionedField<scalar, fvMesh>&,
const dictionary&
);
//- Construct by mapping given plenumPressureFvPatchScalarField
// onto a new patch
plenumPressureFvPatchScalarField
(
const plenumPressureFvPatchScalarField&,
const fvPatch&,
const DimensionedField<scalar, fvMesh>&,
const fieldMapper&
);
//- Disallow copy without setting internal field reference
plenumPressureFvPatchScalarField
(
const plenumPressureFvPatchScalarField&
) = delete;
//- Copy constructor setting internal field reference
plenumPressureFvPatchScalarField
(
const plenumPressureFvPatchScalarField&,
const DimensionedField<scalar, fvMesh>&
);
//- Construct and return a clone setting internal field reference
virtual tmp<fvPatchScalarField> clone
(
const DimensionedField<scalar, fvMesh>& iF
) const
{
return tmp<fvPatchScalarField>
(
new plenumPressureFvPatchScalarField(*this, iF)
);
}
// Member Functions
// Evaluation functions
//- Update the coefficients associated with the patch field
virtual void updateCoeffs();
//- Write
virtual void write(Ostream&) const;
// Member Operators
//- Inherit assignment
using fixedValueFvPatchScalarField::operator=;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //
|