Compared to laminar flows, simulations of turbulent flows are
more challenging in many ways. For the Reynolds-averaged approach,
additional equations are solved for the turbulence quantities. Since
the equations for mean quantities and the turbulent quantities (
, 
, 
, 
, or the Reynolds stresses)
are strongly coupled in a highly nonlinear fashion, it takes more
computational effort to obtain a converged turbulent solution than
to obtain a converged laminar solution. The LES model, while embodying
a simpler, algebraic model for the subgrid-scale viscosity, requires
a transient solution on a very fine mesh.
The fidelity of the results for turbulent flows is largely determined by the turbulence model being used. Here are some guidelines that can enhance the quality of your turbulent flow simulations.
For additional information, see the following sections:
The following are suggestions to follow when generating the mesh for use in your turbulent flow simulation:
First imagine the flow under consideration, then identify the main flow features expected in the flow using your physical intuition or any data for a similar flow situation. Generate a mesh that can resolve the major features that you expect.
If the flow is wall-bounded and the wall is expected to affect the flow significantly, you should take additional care when generating the mesh. See Grid Resolution for RANS Models and Wall Boundary Layers for guidelines.
The suggestions below are provided to help you obtain better accuracy in your results:
Use the turbulence model that is better suited for the salient features you expect to see in the flow (see Choosing a Turbulence Model).
Because the mean quantities have larger gradients in turbulent flows than in laminar flows, it is recommended that you use high-order schemes for the convection terms. This is especially true if you employ a triangular or tetrahedral mesh. Note that excessive numerical diffusion adversely affects the solution accuracy, even with the most elaborate turbulence model.
In some flow situations involving inlet boundaries, the flow downstream of the inlet is dictated by the boundary conditions at the inlet. In such cases, you should exercise care to make sure that reasonably realistic boundary values are specified.
The suggestions below are provided to help you enhance convergence for turbulent flow calculations:
Starting with excessively crude initial guesses for mean and turbulence quantities may cause the solution to diverge. A safe approach is to start your calculation using conservative (small) under-relaxation parameters and (for the density-based solvers) a conservative Courant number, and increase them gradually as the iterations proceed and the solution begins to settle down.
It is also helpful for faster convergence to start with reasonable initial guesses for the
and 
(or 
and 
) fields. Particularly when a 
-insensitive wall treatment is used, it is important to
start with a sufficiently developed turbulence field, as recommended in
Providing an Initial Guess for k and ε (or k and ω), to avoid the need for an
excessive number of iterations to develop the turbulence field.When you are using the RNG
-
model, an approach that might help you achieve better
convergence is to obtain a solution with the standard 
-
model before switching to the RNG model. Due to the
additional nonlinearities in the RNG model, lower under-relaxation factors
and (for the density-based solvers) a lower Courant number might also be
necessary.
Note that when you use the enhanced wall treatment (EWT-
), you may sometimes find during the calculation that the residual
for 
is reported to be zero. This happens when your flow is such that
is less than 200 in the entire flow domain, and 
is obtained from the algebraic formula (Equation 4–366 in the Theory Guide) instead of from its transport
equation.
Using the RSM creates a high degree of coupling between the
momentum equations and the turbulent stresses in the flow, and therefore
the calculation can be more prone to stability and convergence difficulties
than with the 
-
models. When you use the RSM, therefore,
you may need to adopt special solution strategies in order to obtain
a converged solution. The following strategies are generally recommended:
Begin the calculations using the standard
-
model. Turn on the
RSM and use the 
-
solution data as a starting point
for the RSM calculation.Use low under-relaxation factors (0.2 to 0.3) and (for the density-based solvers) a low Courant number for highly swirling flows or highly complex flows. In these cases, you may need to reduce the under-relaxation factors both for the velocities and for all of the stresses.
Instructions for setting these solution parameters are provided below. If you are applying the RSM to prediction of a highly swirling flow, you will want to consider the solution strategies discussed in Swirling and Rotating Flows as well.
Ansys Fluent applies under-relaxation to the Reynolds stresses. You can set under-relaxation factors using the Solution Controls Task Page.
Solution → 
Controls
The default settings of 0.5 are recommended for most cases. You may be able to increase these settings and speed up the convergence when the RSM solution begins to converge.
In some situations, when poor convergence is observed one might facilitate the convergence rates by modifying some of the under-relaxation values whilst leaving the others unchanged. This might be a more successful approach than the simple scaling of all under-relaxation values.
In some instances, you may want to let the current Reynolds stress field remain fixed, skipping the solution of the Reynolds transport equations while solving the other transport equations. You can enable/disable all Reynolds stress equations in the Equations dialog box.
Solution → Controls
Equations...
When you use the RSM for turbulence, Ansys Fluent reports the
equation residuals for the individual Reynolds stress transport equations.
You can apply the usual convergence criteria to the Reynolds stress
residuals: normalized residuals in the range of 
usually indicate a practically-converged solution.
However, you may need to apply tighter convergence criteria (below 
) to ensure full convergence.
Large eddy simulation involves running a transient solution from some initial condition, on an appropriately fine mesh, using an appropriate time step size. The solution must be run long enough to become independent of the initial condition and to enable the statistics of the flow field to be determined.
The following are suggestions to follow when running a large eddy simulation:
Start by running a steady-state flow simulation using a Reynolds-averaged turbulence model such as standard
-
, 
-
, or even RSM. Run until the flow field is reasonably
converged and then use the
solve/initialize/init-turb-vel-fluctuationstext command to generate the instantaneous velocity field out of the steady-state RANS results. This command must be executed before LES is enabled. This option is available for all RANS-based models except the Spalart-Allmaras model, and it will create a much more realistic initial field for the LES run. Additionally, it will help in reducing the time needed for the LES simulation to reach a statistically stable mode. This step is optional.When you enable LES, Ansys Fluent will automatically turn on the unsteady solver option and choose the second-order implicit formulation. You will need to set the appropriate time step size and all the needed solution parameters. (See Inputs for Time-Dependent Problems for guidelines on setting solution parameters for transient calculations in general.) For the pressure-based solver, the bounded central differencing spatial discretization scheme will be automatically selected for momentum equations; both the bounded central-differencing and pure central-differencing schemes are available for all equations when running LES simulations. For the density-based solver, the bounded central differencing scheme can be used for the flow equations, though it is not selected by default.
Run LES until the flow becomes statistically steady. The best way to see if the flow is fully developed and statistically steady is to monitor forces and solution variables (for example, velocity components or pressure) at selected locations in the flow.
Zero out the initial statistics using the
solve/initialize/init-flow-statisticstext command. Before you restart the solution, enable Data Sampling for Time Statistics in the Run Calculation Task Page, as described in Inputs for Time-Dependent Problems. With this option enabled, Ansys Fluent will gather data for time statistics while performing a large eddy simulation. You can set the Sampling Interval such that Data Sampling for Time Statistics can be performed at the specified frequency. When Data Sampling for Time Statistics is enabled, the statistics collected at each sampling interval can be postprocessed and you can then view both the mean and the root-mean-square-error (RMSE) values in Ansys Fluent. The Sampled Time displays the time period over which data has been sampled for the postprocessing of the mean and RMSE values. As long as the time step size has been constant, dividing this by the time step size yields the number of data sets that have been collected. If the time step size is varied, every contribution of data sets sampled is automatically weighted by the current time step size.Continue until you get statistically stable data. The duration of the simulation can be determined beforehand by estimating the mean flow residence time in the solution domain (
, where 
is the characteristic length
of the solution domain and 
is a characteristic mean flow velocity). The simulation
should be run for at least a few mean flow residence times.
Instructions for setting the solution parameters for LES are provided below.
Ansys Fluent provides both first-order and second-order temporal discretizations. For LES, the second-order discretization is recommended.
Solution → Methods
Overly diffusive schemes such as the first-order upwind scheme should be avoided, because they may unduly damp out the energy of the resolved eddies. The central-differencing based schemes are recommended for all equations when you use the LES model. Ansys Fluent provides two central-differencing based schemes: pure central-differencing and bounded central-differencing. The bounded scheme is the default option for momentum discretization when you select LES, SAS, DES, SDES, or SBES.
Solution →
Methods