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.
Note for OpenFOAM versions prior to v3.0.0: the keyword options are instead RASModel and LESModel respectively.
If RAS is selected, the choice of RAS modelling is specified in a RAS sub-dictionary, 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 LES is selected, the choice of LES modelling is specified in a LES dictionary and the LES turbulence model is selected by the LESModel entry. Note for OpenFOAM versions prior to v3.0.0: the RAS modelling is specified in a separate RASProperties file rather than in a RAS sub-dictionary of turbulenceProperties; similarly, LES modelling is in a separate LESProperties file.
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.
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 RAS sub-dictionary 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 RAS sub-dictionary, 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 RAS sub-dictionary file and edit the entries as required.
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 the turbulent viscosity field in the 0/nut file. Note for OpenFOAM versions prior to v3.0.0: wall functions for compressible RAS are specified through the field in the 0/mut file, through in the 0/nuSgs file for incompressible LES and in the 0/muSgs file for compressible LES. For example, a 0/nut file:
18 dimensions [0 2 -1 0 0 0 0];
20 internalField uniform 0;
26 type nutkWallFunction;
27 value uniform 0;
31 type nutkWallFunction;
32 value uniform 0;
36 type empty;
41 // ************************************************************************* //
There are a number of wall function models available in the release, e.g. nutWallFunction, nutRoughWallFunction, nutUSpaldingWallFunction, nutkWallFunction and nutkAtmWallFunction. The user can consult the relevant directories for a full list of wall function models:
Within each wall function boundary condition the user can over-ride default settings for , and 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.