Turbulent flows contain a wide range of length and time scales, with large scale motions being generally more energetic than the small scale ones. The prediction of industrially important fluctuating flow problems can be performed using the technique of LES. LES is an approach that solves for large-scale fluctuating motions and uses "sub-grid" scale turbulence models for the small-scale motion.
The usual approach to predicting turbulent flows is to use the Reynolds Averaged Navier-Stokes equations, (RANS), which solve for time averaged quantities. However, there are some situations where the approach is not adequate, and the alternative approaches of Large Eddy Simulation (LES) or Direct Numerical Simulation (DNS) can be adopted. With these methods, time dependent equations are solved for the turbulent motion with either no approximations and all relevant scales resolved (DNS) or the equations are filtered in some way to remove very fine time and length scales (LES). These approaches require fine grids and small timesteps, particularly for wall bounded flows, as well as a large number of timesteps to generate statistically meaningful correlations for the fluctuation velocity components. However, they can give details on the structure of turbulent flows, such as pressure fluctuations and Lighthill stresses, which cannot be obtained from a RANS formulation.
Further theoretical model information is available in Large Eddy Simulation Theory in the CFX-Solver Theory Guide.
Before starting an LES simulation, you should consider if it is the most appropriate solution approach. For low Reynolds numbers (Re < 5000) or when it is important to be able to resolve all scales (for example, for transition to turbulent flow), consider DNS if you have a large computer available. For Higher Reynolds numbers, LES might be a suitable option for cases where:
The flow is likely to be unstable, with large scale flapping of a shear layer or vortex shedding.
The flow is likely to be unsteady with coherent structures (cyclone, flasher).
The flow is buoyant, with large unstable regions created by heating from below, or by lighter fluid below heavier fluid (multiphase flows in inclined pipelines).
Conventional RANS approach are known to fail (for example due to highly anisotropic turbulence).
A good representation of the turbulent structure is required for small-scale processes such as micro-mixing or chemical reaction.
The noise from the flow is to be calculated, and especially when the broadband contribution is significant.
Other fluctuating information is required (such as fluctuating forces, gusts of winds).
You can afford to wait for up to a week for results, using an 8 to 16 processor system.
It should be noted that for wall bounded flows, so called ‘streaky structures’ develop in the near wall region. These ‘streaky structures’ must be resolved and this leads to high resolution requirements and computing times for LES of wall-bounded flows. This should be kept in mind and you should consider the SAS (Scale-Adaptive Simulation) or DES (Detached Eddy Simulation) approach first before performing a LES for wall bounded flows.
Even though there might be symmetries in the geometry and flow, the geometrical model should include the full region because, while the time averaged flows may be symmetric, the instantaneous flows are not, and restricting the domain could constrain the turbulence. Two-dimensional approximations are particularly poor.
The mesh and timesteps are an inherent part of the model. LES models make use of the grid scale for filtering out the turbulence. If the mesh is anisotropic to resolve a jet, for example, the longer length scale in the flow direction may also have an undue effect on the cross-stream turbulence. For this reason, consider the use of isotropic grids, perhaps using tetrahedral rather than hexahedral elements.
If the boundary layer structure is important, you should resolve it with at least 15 points across the boundary layer and with the first grid point at a position of approximately y^{+} = 1. Note however, that large aspect rations in the mesh are not suitable for LES. This often results in excessive resolution requirements for boundary layer flows.
Three LES models are available: it is recommended that you use the wall-adapted local eddy-viscosity model by Nicoud and Ducros [200](LES WALE model) as a first choice. This is an algebraic model like the Smagorinsky model, but overcomes some known deficiencies of the Smagorinsky model: the WALE model produces almost no eddy-viscosity in wall-bounded laminar flows and is therefore capable to reproduce the laminar to turbulent transition. Furthermore, the WALE model has been designed to return the correct wall-asymptotic -variation of the subgrid-scale viscosity and needs no damping functions.
In addition to the WALE model, the Smagorinsky model [34] and the Dynamic Smagorinsky-Lilly model (Germano et al. [198], Lilly [199]) are available. The Dynamic Smagorinsky-Lilly model is based on the Germano-identity and uses information contained in the resolved turbulent velocity field to evaluate the model coefficient, in order to overcome the deficiencies of the Smagorinsky model. The model coefficient is no longer a constant value and adjusts automatically to the flow type. However this method needs explicit (secondary) filtering and is therefore more time consuming than an algebraic model. Details on the LES models can be found in Large Eddy Simulation Theory in the CFX-Solver Theory Guide.
The representation of the turbulent structures at inlets can be a difficult part of the setup. The detailed properties of the incoming flow can have a strong effect on the development of the downstream solution. This has been observed in turbulent jets, as well as developing boundary layer cases. For other cases, however, the turbulent conditions at the inlet can have relatively little impact on the flow in the device. For example, in a cyclone body, the flow can be essentially determined by very strong anisotropy effects.
If the inlet turbulence is felt to play an important role, you should consider:
Moving the inlet far upstream of the geometry of interest. This allows the correct turbulent structures to establish themselves before the flow reaches that geometry. Additional obstructions can be placed upstream of geometry to affect the turbulent structures. This procedure, however, will require the simulation of the transition process.
Using unsteady values computed from a separate LES simulation (pipe flows and channel flows).
With the transport of turbulent eddies outside of the computational domain, some recirculation can occur at outlets. Experience shows that if the code is allowed to bring some fluid back into the domain at outlets, it can destabilize the solution. Therefore, you should use outlet boundary conditions rather than openings when using LES. Opening types of boundary conditions enable the flow to come back in, whereas with outlet boundary conditions, the code builds artificial walls at the boundary, when the flow tries to come back in. These artificial walls are later taken away when the flow goes out again.
The use of artificial walls at outlets might introduce some un-physical behavior locally, but it increases the robustness of the calculation.
For simulations initialized with values (rather than from an
initial guess field), it is possible to perturb the initial guess
by setting an RMS Velocity Fluctuation
. This
has the effect of kickstarting the solution process. For a velocity
distribution , the fluctuation is
the quantity:
(4–8) |
The behavior of the velocity fluctuation is applied according
to the following rules when you select Automatic
or Automatic with Value
as the Initialization option, as well as specify a velocity fluctuation:
If an initial values file is not found, the fluctuation is applied to the initial velocity field.
When an initial values file is used, it is assumed that you are restarting from a previous set of results, and the fluctuation is not applied.
If you want to apply a velocity fluctuation on a restart (for
example, if the initial guess is a RANS solution), you can override
this behavior by setting the expert parameter apply ic fluctuations for les
to t
.
On the Solver Control form, it is recommend
that you use the Central Difference advection
scheme rather than the High Resolution scheme
because it is less dissipative and it has provided good answers in
CFX. Select the transient scheme as 2nd Order Backward Euler
.
First order fully implicit methods in time are usually too diffusive, and the turbulence is damped out. For highly unstable problems, such as cyclones, lower order methods may work, but the results will be very damped, unless very small timesteps are used.
For accuracy, the average Courant (or CFL) number should be in the range of 0.5-1. Larger values can give stable results, but the turbulence may be damped. For compressible flows where the acoustic behavior is being modeled (eg, for noise calculations), this conclusion still holds, but for the CFL number based on the acoustic velocity as well as the convective velocity.
1,000 - 10,000 timesteps are typically required for getting converged statistics. More steps are required for second order quantities (for example, variances) than for means. Check the convergence of the statistics. For a vortex-shedding problem, several cycles of the vortex shedding are required.
The implicit coupled solver used in CFX requires the equations to be converged within each timestep to guarantee conservation. The number of coefficient loops required to achieve this is a function of the timestep size. With CFL numbers of order 0.5-1, convergence within each timestep should be achieved quickly. It is advisable to test the sensitivity of the solution to the number of coefficient loops, to avoid using more coefficient loops (and hence longer run times) than necessary. LES tests involving incompressible flow past circular cylinders indicates that one coefficient loop per timestep is sufficient if the average CFL number is about 0.75. If the physics or geometry is more complicated, additional coefficient loops (3-5) may be required. Timesteps sizes that require more coefficient loops than this will tend to degrade solution accuracy.
You may find, especially if running averages are to be calculated, that for some cases you will need to increase the amount of memory needed for the calculation by using a memory factor above 1 (typically 1.2).
The following values can be written to results files as the solution progresses using the Solver Output tab in CFX-Pre. For details, see Output Control in the CFX-Pre User's Guide.
Although the statistics outlined in the Statistical Reynolds Stresses are useful for any simulation, they are particularly important in the context of LES. Of particular interest, are the Reynolds Stress (RS) components:
(4–9) |
where is the fluctuation of the i^{th} velocity component. For details, see Statistical Reynolds Stresses.
In LES runs, Reynolds Stress components are automatically generated using running statistics of the instantaneous, transient velocity field. As outlined above for the calculation of the standard deviation, a Reynolds Stress component can be evaluated using the difference between the running arithmetic average of the instantaneous velocity correlation and the running arithmetic average of the instantaneous velocities as:
(4–10) |
The noted running averages are also automatically generated for LES runs.
Data sampling for the Statistical Reynolds Stresses begins on the first timestep by default. This is because the transient statistics used in the stress evaluation (that is, the arithmetic averages of velocity and its correlation) start accumulating on the first timestep by default.
Sampling for the Statistical Reynolds Stresses is deferred, indirectly, by explicitly creating one of the required transient statistics (that is, the arithmetic averages of velocity or its correlation) and setting the start iteration (the starting timestep index) to a value larger than unity. If different start iterations are set for each of the velocity or velocity correlation averages, then the maximum start iteration set is used for both averages to ensure that the Statistical Reynolds Stresses are correctly evaluated.
The Statistical Reynolds Stress variable is evaluated using Equation 4–10 during every timestep, regardless of the start iteration specified for the required velocity-based statistics. This means that if the current timestep is less than the start iteration specified for the velocity-based statistics, then those statistics will be initialized as outlined in Working with Transient Statistics in the CFX-Pre User's Guide.