The open source CFD toolbox
turbulentInletFvPatchField.H
Go to the documentation of this file.
1/*---------------------------------------------------------------------------*\
2 ========= |
3 \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
4 \\ / O peration |
5 \\ / A nd | www.openfoam.com
6 \\/ M anipulation |
7-------------------------------------------------------------------------------
8 Copyright (C) 2011-2016 OpenFOAM Foundation
9-------------------------------------------------------------------------------
11 This file is part of OpenFOAM.
12
13 OpenFOAM is free software: you can redistribute it and/or modify it
15 the Free Software Foundation, either version 3 of the License, or
16 (at your option) any later version.
17
18 OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
19 ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
20 FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License
21 for more details.
22
23 You should have received a copy of the GNU General Public License
24 along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
25
26Class
27 Foam::turbulentInletFvPatchField
28
29Group
30 grpInletBoundaryConditions
31
32Description
33 This boundary condition produces spatiotemporal-variant field by summing
34 a set of pseudo-random numbers and a given spatiotemporal-invariant mean
35 field. The field can be any type, e.g. scalarField. At a single point and
36 time, all components are summed by the same random number, e.g. velocity
37 components (u, v, w) are summed by the same random number, p; thus, output
38 is (u+p, v+p, w+p).
39
40 The pseudo-random number generator obeys the probability density function
41 of the uniform distribution constrained by the range [0:1]. The seed for
42 the random number generator is hard-coded; therefore, it will produce the
43 same sequence of random numbers at every execution.
44
45 \f[
46 x_p = (1 - \alpha) x_p^{n - 1} + \alpha (x_{ref} + c s R |x_{ref}|)
47 \f]
48 where
49
50 \vartable
51 x_p | patch field
52 x_{ref} | spatiotemporal-invariant patch scalar
53 n | time level
54 \alpha | a scalar attempting to build two-temporal-point correlations
55 by heuristically adding a fraction of the new random component
56 to the previous time patch field
57 c | a heuristic automatically calculated correction term
58 to compensate energy level losses due to the alpha scalar
59 R | pseudo-random number [HARD-CODED seed]
60 s | fluctuation scale (proportional to the xRef)
61 \endvartable
62
63Usage
64 \table
65 Property | Description | Required | Default value
66 fluctuationScale | RMS fluctuation scale (fraction of mean) | yes |
67 referenceField | reference (mean) field | yes |
68 alpha | fraction of new random component added to previous | no | 0.1
69 \endtable
70
71 Example of the boundary condition specification:
72 \verbatim
73 <patchName>
74 {
75 // Mandatory entries
76 type turbulentInlet;
77 fluctuationScale 0.1; // the term s above
78 referenceField uniform 10; // the term xRef above
79
80 // Optional entries
81 alpha 0.1; // the term alpha above
82 }
83 \endverbatim
84
85Note
86 This boundary condition should not be used for DES or LES computations as a
87 turbulent velocity inflow condition, because the BC will not produce
88 turbulence-alike time-series, and will decay almost immediately downstream
89 of the inlet boundary although its historical name suggests the opposite.
90
91 Nevertheless, the BC may be still used for other applications, e.g. as a
92 uniform-random noise source in aeroacoustics.
93
94SeeAlso
95 Foam::fixedValueFvPatchField
96
97SourceFiles
98 turbulentInletFvPatchField.C
99
100\*---------------------------------------------------------------------------*/
101
102#ifndef turbulentInletFvPatchField_H
103#define turbulentInletFvPatchField_H
104
105#include "Random.H"
107
108// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
109
110namespace Foam
111{
112
113/*---------------------------------------------------------------------------*\
114 Class turbulentInletFvPatchField Declaration
115\*---------------------------------------------------------------------------*/
116
117template<class Type>
118class turbulentInletFvPatchField
119:
120 public fixedValueFvPatchField<Type>
121{
122 // Private Data
123
124 //- Random number generator
125 Random ranGen_;
126
127 //- Fluctuation scale
128 Type fluctuationScale_;
129
130 //- Reference field
131 Field<Type> referenceField_;
132
133 //- Fraction of RMS component to apply to last time step values
134 scalar alpha_;
135
136 //- Current time index (used for updating)
137 label curTimeIndex_;
138
139
140public:
141
142 //- Runtime type information
143 TypeName("turbulentInlet");
144
145
146 // Constructors
147
148 //- Construct from patch and internal field
150 (
151 const fvPatch&,
152 const DimensionedField<Type, volMesh>&
153 );
154
155 //- Construct from patch, internal field and dictionary
157 (
158 const fvPatch&,
159 const DimensionedField<Type, volMesh>&,
160 const dictionary&
161 );
162
163 //- Construct by mapping given turbulentInletFvPatchField
164 //- onto a new patch
166 (
167 const turbulentInletFvPatchField<Type>&,
168 const fvPatch&,
169 const DimensionedField<Type, volMesh>&,
170 const fvPatchFieldMapper&
171 );
172
173 //- Construct as copy
175 (
177 );
178
179 //- Construct and return a clone
180 virtual tmp<fvPatchField<Type>> clone() const
181 {
183 (
185 );
186 }
187
188 //- Construct as copy setting internal field reference
190 (
193 );
194
195 //- Construct and return a clone setting internal field reference
197 (
199 ) const
200 {
202 (
204 );
205 }
206
207
208 // Member Functions
209
210 // Access
211
212 //- Return the fluctuation scale
213 const Type& fluctuationScale() const
214 {
215 return fluctuationScale_;
216 }
217
218 //- Return reference to the fluctuation scale to allow adjustment
219 Type& fluctuationScale()
220 {
221 return fluctuationScale_;
222 }
223
224 //- Return the reference field
225 const Field<Type>& referenceField() const
226 {
227 return referenceField_;
228 }
229
230 //- Return reference to the reference field to allow adjustment
231 Field<Type>& referenceField()
232 {
233 return referenceField_;
234 }
235
237 // Mapping functions
238
239 //- Map (and resize as needed) from self given a mapping object
240 virtual void autoMap
241 (
242 const fvPatchFieldMapper&
243 );
244
245 //- Reverse map the given fvPatchField onto this fvPatchField
246 virtual void rmap
247 (
248 const fvPatchField<Type>&,
249 const labelList&
250 );
251
253 // Evaluation functions
254
255 //- Update the coefficients associated with the patch field
256 virtual void updateCoeffs();
257
258
259 //- Write
260 virtual void write(Ostream&) const;
261};
262
263
264// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
265
266} // End namespace Foam
267
268// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
270#ifdef NoRepository
272#endif
273
274// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
276#endif
277
278// ************************************************************************* //
Field with dimensions and associated with geometry type GeoMesh which is used to size the field and a...
Generic templated field type.
Definition: Field.H:82
An Ostream is an abstract base class for all output systems (streams, files, token lists,...
Definition: Ostream.H:62
Random number generator.
Definition: Random.H:60
A list of keyword definitions, which are a keyword followed by a number of values (eg,...
Definition: dictionary.H:126
This boundary condition supplies a fixed value constraint, and is the base class for a number of othe...
A FieldMapper for finite-volume patch fields.
Abstract base class with a fat-interface to all derived classes covering all possible ways in which t...
Definition: fvPatchField.H:82
A finiteVolume patch using a polyPatch and a fvBoundaryMesh.
Definition: fvPatch.H:71
A class for managing temporary objects.
Definition: tmp.H:65
This boundary condition produces spatiotemporal-variant field by summing a set of pseudo-random numbe...
virtual void autoMap(const fvPatchFieldMapper &)
Map (and resize as needed) from self given a mapping object.
Type & fluctuationScale()
Return reference to the fluctuation scale to allow adjustment.
virtual void updateCoeffs()
Update the coefficients associated with the patch field.
turbulentInletFvPatchField(const fvPatch &, const DimensionedField< Type, volMesh > &)
Construct from patch and internal field.
virtual void rmap(const fvPatchField< Type > &, const labelList &)
Reverse map the given fvPatchField onto this fvPatchField.
virtual tmp< fvPatchField< Type > > clone() const
Construct and return a clone.
const Field< Type > & referenceField() const
Return the reference field.
Field< Type > & referenceField()
Return reference to the reference field to allow adjustment.
const Type & fluctuationScale() const
Return the fluctuation scale.
TypeName("turbulentInlet")
Runtime type information.
virtual tmp< fvPatchField< Type > > clone(const DimensionedField< Type, volMesh > &iF) const
Construct and return a clone setting internal field reference.
Namespace for OpenFOAM.
runTime write()
#define TypeName(TypeNameString)
Declare a ClassName() with extra virtual type info.
Definition: typeInfo.H:73