-
Notifications
You must be signed in to change notification settings - Fork 604
/
totalPressureFvPatchScalarField.H
244 lines (195 loc) · 7.8 KB
/
totalPressureFvPatchScalarField.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
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
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Copyright (C) 2011-2023 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::totalPressureFvPatchScalarField
Description
Inflow, outflow and entrainment pressure boundary condition based on a
constant total pressure assumption.
For outflow the patch pressure is set to the external static pressure.
For inflow the patch pressure is evaluated from the patch velocity and the
external total pressure obtained from the external static pressure \c p_0
and external velocity \c U_0 which is looked-up from the the optional \c
tangentialVelocity entry in the \c pressureInletOutletVelocity velocity
boundary condition for the patch if that boundary condition is used,
otherwise \c U_0 is assumed zero and the external total pressure is equal to
the external static pressure.
The patch pressure is evaluated from the external conditions using one of
the following expressions depending on the flow conditions and
specification of compressibility:
1. incompressible subsonic:
\f[
p_p = p_0 + 0.5 |U_0|^2 - 0.5 |U|^2
\f]
where
\vartable
p_p | pressure at patch [m^2/s^2]
p_0 | external static pressure [m^2/s^2]
U | velocity [m/s]
U_0 | external velocity [m/s]
\endvartable
2. compressible subsonic:
\f[
p_p = p_0 + \rho (0.5 |U_0|^2 - 0.5 |U|^2)
\f]
where
\vartable
p_p | pressure at patch [Pa]
p_0 | external static pressure [Pa]
\rho | density [kg/m^3]
U | velocity [m/s]
U_0 | external velocity [m/s]
\endvartable
3. compressible transonic (\f$\gamma = 1\f$):
\f[
p_p = \frac{p_0}{1 + \psi (0.5 |U|^2 - 0.5 |U_0|^2)}
\f]
where
\vartable
p_p | pressure at patch [Pa]
p_0 | external static pressure [Pa]
\psi | compressibility [m^2/s^2]
\rho | density [kg/m^3]
U | velocity [m/s]
U_0 | external velocity [m/s]
\endvartable
4. compressible supersonic (\f$\gamma > 1\f$):
\f[
p_p = \frac{p_0}
{(1 + G \psi (0.5 |U|^2 - 0.5 |U_0|^2))^{\frac{1}{G}}}
\f]
where
\vartable
p_p | pressure at patch [Pa]
p_0 | external static pressure [Pa]
\psi | compressibility [m^2/s^2]
\rho | density [kg/m^3]
G | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$ []
\gamma | ratio of specific heats (Cp/Cv) []
U | velocity [m/s]
U_0 | external velocity [m/s]
\endvartable
The modes of operation are set by the dimensions of the pressure field
to which this boundary condition is applied, the \c psi entry and the value
of \c gamma:
\table
Mode | dimensions | psi | gamma
incompressible subsonic | p/rho | |
compressible subsonic | p | none |
compressible transonic | p | psi | 1
compressible supersonic | p | psi | > 1
\endtable
Usage
\table
Property | Description | Required | Default value
U | Velocity field name | no | U
phi | Flux field name | no | phi
rho | Density field name | no | rho
psi | Compressibility field name | no | none
gamma | (Cp/Cv) | no | 1
p0 | External pressure | yes |
\endtable
Example of the boundary condition specification:
\verbatim
<patchName>
{
type totalPressure;
p0 uniform 1e5;
}
\endverbatim
See also
Foam::dynamicPressureFvPatchScalarField
Foam::fixedValueFvPatchField
Foam::pressureInletOutletVelocityFvPatchVectorField
SourceFiles
totalPressureFvPatchScalarField.C
\*---------------------------------------------------------------------------*/
#ifndef totalPressureFvPatchScalarField_H
#define totalPressureFvPatchScalarField_H
#include "dynamicPressureFvPatchScalarField.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
/*---------------------------------------------------------------------------*\
Class totalPressureFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
class totalPressureFvPatchScalarField
:
public dynamicPressureFvPatchScalarField
{
protected:
// Protected Data
//- Name of the velocity field
const word UName_;
//- Name of the flux field
const word phiName_;
public:
//- Runtime type information
TypeName("totalPressure");
// Constructors
//- Construct from patch, internal field and dictionary
totalPressureFvPatchScalarField
(
const fvPatch&,
const DimensionedField<scalar, volMesh>&,
const dictionary&
);
//- Construct by mapping given totalPressureFvPatchScalarField
// onto a new patch
totalPressureFvPatchScalarField
(
const totalPressureFvPatchScalarField&,
const fvPatch&,
const DimensionedField<scalar, volMesh>&,
const fieldMapper&
);
//- Disallow copy without setting internal field reference
totalPressureFvPatchScalarField
(
const totalPressureFvPatchScalarField&
) = delete;
//- Copy constructor setting internal field reference
totalPressureFvPatchScalarField
(
const totalPressureFvPatchScalarField&,
const DimensionedField<scalar, volMesh>&
);
//- Construct and return a clone setting internal field reference
virtual tmp<fvPatchScalarField> clone
(
const DimensionedField<scalar, volMesh>& iF
) const
{
return tmp<fvPatchScalarField>
(
new totalPressureFvPatchScalarField(*this, iF)
);
}
// Member Functions
// Evaluation functions
//- Update the coefficients associated with the patch field
virtual void updateCoeffs();
//- Write
virtual void write(Ostream&) const;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //