Newer
Older
mattijs
committed
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
259
260
261
262
263
264
265
266
267
268
269
270
271
272
273
274
275
276
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2015 OpenCFD Ltd.
\\/ 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::pressurePIDControlInletVelocityFvPatchVectorField
Group
grpInletBoundaryConditions
Description
This boundary condition tries to generate an inlet velocity that maintains
a specified pressure drop between two face zones downstream. The zones
should fully span a duct through which all the inlet flow passes.
An incompressible, lossless analysis of the flow between the inlet and the
two face-zones is performed. An ideal inlet velocity is thereby calculated
from the user-specified pressure drop. This analysis can include the
transient effect of the inlet velocity change. In this case, a shape factor
is included to represent non-linearity in the duct cross section.
The average pressure drop between the two face zones is measured. The same
incompressible, lossless analysis is performed using this pressure drop.
The difference between the two computed velocities is considered as an
error. The ideal inlet is modified so as to drive this error to zero. This
is accomplished by means of a PID control algorithm, for which
non-dimensional gains are specified by the user.
The shape factor takes a value of 0 for a linear change in cross sectional
area between the two face zones. A value of 1 represents a step change in
area at the mid-point between the zones. A smooth cubic or cosine profile
between two zones with zero divergence is typically represented by a factor
of between 0.2 and 0.25.
\heading Patch usage
\table
Property | Description | Required | Default value
upstream | upstream face zone name | yes |
downstream | downstream face zone name | yes |
deltaP | desired pressure drop | yes |
shapeFactor | non-linearity in the nozzle | no | 0
p | pressure field name | no | p
phi | flux field name | yes | phi
rho | density field name | no | none
P | proportional gain | yes |
I | integral gain | yes |
D | differential gain | yes |
\endtable
Example of the boundary condition specification:
\verbatim
myPatch
{
type pressurePIDControlInletVelocity;
upstream upstream;
downstream downstream;
deltaP 200;
shapeFactor 0;
p p;
phi phi;
rho none;
P 0.5;
I 0.5;
D 0.1;
value uniform (0 0 0);
}
SeeAlso
Foam::fixedValueFvPatchField
SourceFiles
pressurePIDControlInletVelocityFvPatchVectorField.C
\*---------------------------------------------------------------------------*/
#ifndef pressurePIDControlInletVelocityFvPatchVectorField_H
#define pressurePIDControlInletVelocityFvPatchVectorField_H
#include "fixedValueFvPatchFields.H"
#include "Switch.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
/*---------------------------------------------------------------------------*\
Class pressurePIDControlInletVelocityFvPatchVectorField Declaration
\*---------------------------------------------------------------------------*/
class pressurePIDControlInletVelocityFvPatchVectorField
:
public fixedValueFvPatchVectorField
{
// Private data
//- Name of the upstream face zone
const word upstreamName_;
//- Name of the downstream face zone
const word downstreamName_;
//- Desired pressure difference between upstream and downstream
const scalar deltaP_;
//- Nozzle shape factor
const scalar shapeFactor_;
//- Name of the pressure field
const word pName_;
//- Name of the flux field
const word phiName_;
//- Name of the density field (if any)
const word rhoName_;
//- Proportional gain
const scalar P_;
//- Integral gain
const scalar I_;
//- Derivative gain
const scalar D_;
//- Volumetric flow rate
scalar Q_;
//- Error
scalar error_;
//- Error integral w.r.t. time
scalar errorIntegral_;
//- Old volumetric flow rate
scalar oldQ_;
//- Old error
scalar oldError_;
//- Old error integral w.r.t. time
scalar oldErrorIntegral_;
//- Time index of the last update
label timeIndex_;
// Private member functions
//- Return the pressure interpolated to the faces
const surfaceScalarField& facePressure() const;
//- Calculate the average on a face zone
template <class Type>
void faceZoneAverage
(
const word& name,
const GeometricField<Type, fvsPatchField, surfaceMesh>& field,
scalar& area,
Type& average
) const;
public:
//- Runtime type information
TypeName("pressurePIDControlInletVelocity");
// Constructors
//- Construct from patch and internal field
pressurePIDControlInletVelocityFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&
);
//- Construct from patch, internal field and dictionary
pressurePIDControlInletVelocityFvPatchVectorField
(
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const dictionary&
);
//- Construct by mapping given
// flowRateInletVelocityFvPatchVectorField
// onto a new patch
pressurePIDControlInletVelocityFvPatchVectorField
(
const pressurePIDControlInletVelocityFvPatchVectorField&,
const fvPatch&,
const DimensionedField<vector, volMesh>&,
const fvPatchFieldMapper&
);
//- Construct as copy
pressurePIDControlInletVelocityFvPatchVectorField
(
const pressurePIDControlInletVelocityFvPatchVectorField&
);
//- Construct and return a clone
virtual tmp<fvPatchVectorField> clone() const
{
return tmp<fvPatchVectorField>
(
new pressurePIDControlInletVelocityFvPatchVectorField
(
*this
)
);
}
//- Construct as copy setting internal field reference
pressurePIDControlInletVelocityFvPatchVectorField
(
const pressurePIDControlInletVelocityFvPatchVectorField&,
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 pressurePIDControlInletVelocityFvPatchVectorField
(
*this,
iF
)
);
}
// Member functions
//- Update the coefficients associated with the patch field
virtual void updateCoeffs();
//- Write
virtual void write(Ostream&) const;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#ifdef NoRepository
# include "pressurePIDControlInletVelocityFvPatchVectorFieldTemplates.C"
#endif
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
mattijs
committed
#endif
// ************************************************************************* //