-
Notifications
You must be signed in to change notification settings - Fork 593
/
flowRateOutletVelocityFvPatchVectorField.H
218 lines (168 loc) · 6.7 KB
/
flowRateOutletVelocityFvPatchVectorField.H
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
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Copyright (C) 2017-2019 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 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&
);
//- Copy constructor
flowRateOutletVelocityFvPatchVectorField
(
const flowRateOutletVelocityFvPatchVectorField&
);
//- Construct and return a clone
virtual tmp<fvPatchVectorField> clone() const
{
return tmp<fvPatchVectorField>
(
new flowRateOutletVelocityFvPatchVectorField(*this)
);
}
//- Copy constructor 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
// ************************************************************************* //