OpenFOAM includes support for the following types of turbulence modelling:
- Reynolds Averaged Simulation (RAS),
- Detached Eddy Simulation (DES), and
- Large Eddy Simulation (LES).
Usage🔗
Turbulence models are specified in the
$FOAM_CASE/constant/turbulenceProperties
file, taking the form, e.g. when specifying the RAS
kOmegaSST model:
simulationType RAS;
RAS
{
RASModel kOmegaSST;
// On/off switch
turbulence on
// Optionally write the model coefficients at run-time
printCoeffs no;
// Optionally override default model coefficients
kOmegaSSTCoeffs
{
...
}
}
Default coefficients are available for all models, based on their reference
literature. Optionally users may override the default values by specifying
a <model>Coeffs
sub-dictionary. Coefficient names can be found by observing
the solver output when setting the printCoeffs
to yes
.
Mesh requirements🔗
Effective use of turbulence models requires close attention to their respective meshing requirements, particularly in near-wall regions.
DNS data from Lee and Moser [39]
RAS
- high Reynolds number: first cell height should be in the region of 30 < \(y^{+}\) < 200. Note that the upper limit is imposed by the location of the outer layer, which depends on the Reynolds number
- low Reynolds number: mesh required to resolve the viscous sub-layer, typically using 10-20 layers
LES
- mesh required to resolve the viscous sub-layer
- requires high order schemes to adequately resolve the high-energy containing eddies
- preferably isotropic mesh
Numerical settings🔗
Turbulence generation is driven by the velocity gradient. Errors arising from the gradient calculation, e.g. due to poor quality meshes, can lead to spurious turbulence predictions and solver instability. This effect can be partly compensated by the application of limited schemes.
Further information🔗
Source code: