[Table of Contents][Index]

7.2 Turbulence models

The turbulenceProperties dictionary is read by any solver that includes turbulence modelling. Within that file is the simulationType keyword that controls the type of turbulence modelling to be used, either:

uses no turbulence models;
uses Reynolds-averaged stress (RAS) modelling;
uses large-eddy simulation (LES) modelling.

If RASModel is selected, the choice of RAS modelling is specified in a RASProperties file, also in the constant directory. The RAS turbulence model is selected by the RASModel entry from a long list of available models that are listed in Table 3.9. Similarly, if LESModel is selected, the choice of LES modelling is specified in a LESProperties dictionary and the LES turbulence model is selected by the LESModel entry.

The entries required in the RASProperties are listed in Table 7.2 and those for LESProperties dictionaries are listed in Table 7.3.

RASModel Name of RAS turbulence model
turbulence Switch to turn turbulence modelling on/off
printCoeffs Switch to print model coeffs to terminal at simulation startup
<RASModel>Coeffs Optional dictionary of coefficients for the respective RASModel
Table 7.2: Keyword entries in the RASProperties dictionary. 

LESModel Name of LES model
delta Name of delta δ model
<LESModel>Coeffs Dictionary of coefficients for the respective LESModel
<delta>Coeffs Dictionary of coefficients for each delta model
Table 7.3: Keyword entries in the LESProperties dictionary. 

The incompressible and compressible RAS turbulence models, isochoric and anisochoric LES models and delta models are all named and described in Table 3.9. Examples of their use can be found in the $FOAM_TUTORIALS.

7.2.1 Model coefficients

The coefficients for the RAS turbulence models are given default values in their respective source code. If the user wishes to override these default values, then they can do so by adding a sub-dictionary entry to the RASProperties file, whose keyword name is that of the model with Coeffs appended, e.g.  kEpsilonCoeffs for the kEpsilon model. If the printCoeffs switch is on in the RASProperties file, an example of the relevant …Coeffs dictionary is printed to standard output when the model is created at the beginning of a run. The user can simply copy this into the RASProperties file and edit the entries as required.

7.2.2 Wall functions

A range of wall function models is available in OpenFOAM that are applied as boundary conditions on individual patches. This enables different wall function models to be applied to different wall regions. The choice of wall function model is specified through: ν t in the 0/nut file for incompressible RAS; μ t in the 0/mut file for compressible RAS; νsgs in the 0/nuSgs file for incompressible LES; μsgs in the 0/muSgs file for incompressible LES. For example, a 0/nut file:

18  dimensions      [0 2 -1 0 0 0 0];
20  internalField   uniform 0;
22  boundaryField
23  {
24      movingWall
25      {
26          type            nutkWallFunction;
27          value           uniform 0;
28      }
29      fixedWalls
30      {
31          type            nutkWallFunction;
32          value           uniform 0;
33      }
34      frontAndBack
35      {
36          type            empty;
37      }
38  }
41  // ************************************************************************* //

There are a number of wall function models available in the release, e.g.  nutWallFunction, nutRoughWallFunction, nutSpalartAllmarasStandardRoughWallFunction, nutSpalartAllmarasStandardWallFunction and nutSpalartAllmarasWallFunction. The user can consult the relevant directories for a full list of wall function models:

    find $FOAM_SRC/turbulenceModels -name wallFunctions

Within each wall function boundary condition the user can over-ride default settings for E, κ and Cμ through optional E, kappa and Cmu keyword entries.

Having selected the particular wall functions on various patches in the nut/mut file, the user should select epsilonWallFunction on corresponding patches in the epsilon field and kqRwallFunction on corresponding patches in the turbulent fields k, q and R.

© 2011-2015 OpenFOAM Foundation
CC-NC-ND 3.0