I'd like to exchange experiencies and informations with other researchers dealing with this topic. In particoular I'm using the LES model of Fluent 5.0 that gives some satisfactory results but with some critical points (simulations at Re=2e+4):

1) The Strouhal number, in both cases (2D-3D), is a little bit too high : 0.26 instead of 0.2 and the value seems to be unsensitive to any change in the main parameters (grid size,domain size,Cs parameter of the Smagorinsky model,time-step) other ideas and experiencies are wellcome

I'm interested in comparing our results with other similar cases: as an example we found optimum values for Cs parameter equal to 0.15 in 2D simulations and 0.1 in 3D simulations of the same circular section. Any other experiences for different sections? (Drag and Lift coefficients used as reference test parameters).

What "wall function" treatment is the fluent model using? In particular, what is it doing as the flow approaches separation?

Do you have a very smooth grid with the first grid point over the top part of the cylinder at y+ < 1? - this should remove concerns about the near wall treatment so long as the expansion ratio is not too severe.

Have you wrapped the grid smoothly around the cylinder? (i.e to give only circular and radial grid lines near the cylinder surface) - strong grid distortions are a bad idea in LES simulations.

What differencing scheme are you using for the convection terms? - for a low order scheme and typical 3D grids, the truncation terms should be dominating the SGS model and you should see significant changes with grid density.

Does the scheme use "pressure smoothing". If so, can you adjust the amount to determine if it is a sensitive parameter?

What time stepping scheme is being used and what is the maximum Courant number?

I'm not using wall-function since I don't find it adequate to flow with a not well identified separation point. I've sterded my simulation trying to mantain y+<1 all around the cylinder and an expansion ratio in radial direction < 1,5 and I've made some adaption (based on y+ and static pressure)refining this mesh in the region close to the cylinder. I'm using a QUICK scheme for convective terms and I've noticed that grid density affects only the magnitude of the drag and lift coefficients but not their frequency. My time step is half of the characteristic time of the phenomenon(based on Re). Do you have ever simulate a similar case? Have yuo ever had problems with Strouhal numbers? Which parameters can affect the frequency of the vortex shadding?

How kind of time step size are you using ? You said it's one half of the "chracteristic time scale" of the flow. I wonder what the characteristic time scale is.

LES results can be affected by several factors, some of which you already referred to in your previous email.

You may want to make sure that the mesh should be fine enough to resolve the boundary layer and near-wake. I suggest that you try smaller time step size and second-order temporal scheme. And I suggest you to check inlet freestream turbulence intensity. I think it should be quite small (less than 1 %). If you used the default, it's too high a value for freestream turbulence level.

Have you done any at other Reynolds numbers ?

I do not understand your point about not using a wall-function (perhaps there is confusion over terminology). Have you turned it off? If you are using a Smagorinsky SGS model (as implied by Cs in you original posting) then there must be some wall function treatment to reduce the turbulent length scale near the wall (van Driest is common). Assuming the treatment is based on the wall friction velocity, what is being done as the flow approaches separation? How is the distance from the wall being evaluated?

Have you wrapped the grid smoothly around the cylinder? (i.e to give only circular and radial grid lines near the cylinder surface) - strong grid distortions are a bad idea in LES simulations.

QUICK is an odd choice of discretization scheme - it may be wise to set Cs=0 since QUICK is likely to be sufficiently dissipative on its own (unless the wall treatment is sensitive to Cs).

Grid density affecting Cl and Cd but not frequency is encouraging. You have a grid dependent solution which is usual and to be expected. The frequency is pretty insensitive to everything which is why getting it wrong is a concern.

As pointed out by Sung-Eun Kim, the most likely cause of your problems is a time step which is much too large. I am not sure what half the characteristic time based on Re is, but if you are not taking 50 000 time steps with a time step small enough for a fluid particle to move no more than about a grid cell the time step is almost certainly too big.

The characteristic time scale I've mentioned is the Kolmogorov's one : t=sqrt(nu/epsilon). It's more conservative than min(dx)/U. I've done only this Re number. I've tried different inlet condition but the frequency seems insensitive of this changes. Have you ever heard of Strouhal values computed by Fluent simulations ? If yes, which kind of model has been used?(k-epsilon or LES)?

I've understood what do you mean with wall-function related to LES. I suppose the Smagorinsky SGS model implemented in Fluent uses the Van Driest damping function but in the on-line manual is not mentioned clearly. So now I'm trying to solve the same case with the RNG subgrid scale model implemented in Fluent too, that seems to be better suited to resolve the flux close to walls. I've created a regular circular and radial grid around the cylinder. QUICK is the scheme suggested by Fluent for LES calculation and also in my experience it seems to be much dissipative. Have you ever use LES models of Fluent? Have you ever calculate the Strouhal number with a numerical simulation?

There is something seriously wrong if your shedding frequency is out by 30% in a reasonably resolved LES simulation. That is, first grid line at y+<1, reasonable radial expansion ratio (<1.5), orthogonal undistorted grid (assumpution - you did not tell me), a sensible time step (max(C)<1) and a reasonable differencing scheme (QUICK).

Although I was probing for details of the LES turbulence modelling (which, it would appear, you can only get by talking to FLUENT) it is very hard to believe that FLUENT could have done anything sufficiently wrong to give rise to this sort of error.

This leaves mistakes/misinterpretations of the FLUENT input/output with which I can provide no help. You really need someone who knows FLUENT to see what you see on the screen.

One final thought though, if you are using an excessively small time step (Kolmogorov time scale), how many cycles (shed vortices) are you waiting before evaluating the shedding frequency?