Hi,

I'm tying to run an unsteady simulation of compressible flow past a bluff body, namely a wheel, at Reynolds number around 10^6, with the hope of capturing the chaotic, unsteady wake. I have used a number of grids, with resolutions fromm 300,000 to 3million cells, and have been using the S-A turbulence model. My time step size is 1E-5.

My problem is that I cannot get an unsteady wake to develop. My results alwas give a symmetrical solution, which looks a lot like the steady-state solution, and there is no massively separated regions, shedding or anything to indicate an unsteady wake. My solutions indicate a system of streamwise vortices which occur as flow over the sides of the wheel spills over the edges and meets with flow over the upper and lower surfaces (hope this makes sense). The solution looks very simple and something I would expect to see from a much lower reynolds number.

I know that the S-A model is overly dissipative, and would tend to damp out shedding etc, but I have seen many papers where S-A has been used to calculate similar flows around bluff bodies.

I have run the simulation for many thousands of time steps, with little or no change in the flow structure. Also, the residuals seem to be oscillating between to upper and lower points, with no variation, or reduction in overal value. This doesn't seem to indicate an unsdeady behaviour, and would suggest that running the simulation for longer would be of little benefit as there is no sign of change.

Any ideas would be much appreciated.

Tom

Did you check weather the fluid started at inlet boundary was arrived and passed your bluff body? What about using your inlet velocity to initialize your computational domain?

Hi, thanks for the response.

I ran a steady-state solver for a few thousand iterations (starting from a pressure-far-field initialisation) until the residuals levelled off. I then used this steady state as the initial conditions for the unsteady solver.

Regarding the flow time: this may be why the simulation has not become unsteady, I may simply need to run the simulation for longer. I.e, until the flow has passed from the inlet to some distance passed the wheel.

thanks

Tom

Why don't you use RNG or, better the Realizable? They capture high swirl and separated flows much better than the S-A, that is usually used only for aerodynamics of streamlined bodies.

By the way, I'm very interested in your work, because I'm also studying the influence of the wheel in cars aerodynamics. Could you send me some captures in order to see the history of the residuals, Cd and Cl? Also:

1. Tetrahedral or Quad elements? 2. Did you use boundary layer? How many layers and heigh? 3. Have you modeled only the wheel or also the contact between the wheel and the ground? If it is the latter, contact patch has a vertical blockage or you have just cut and trimmed the wheel by the ground plane? 4. What was your choice in the solver? I mean, did you started from a 1st order discretization scheme and after a few hundreds of iterations you switched to 2nd order?

Many thanks! Regards, Freeman.

Please find interesting figures as following;

http://www.fluent.com/solutions/broc...s_brochure.pdf

You are trying to simulate an unsteady mean flow with a RANS turbulent model.....wich model the effect of turbulence with an eddy viscosity. This viscosity can strongly damp transient oscillations in your system. This is a common problem of nearly all RANS models. The question is how can a RANS model distinguish between a turbulent oscillation and a mean flow fluctuation....

To verify that this is the origin of the problem, you can decrease the limit of the turbulent viscosity ratio by a factor of 10 to 50 %.

You are using the SA model, but by using other models (kepsilon, komega) you can get other magnitude and distribution of the turbulent viscosity ratio...so try...

Last think (or first) to verify is your numerical diffusivity (verify the mesh and the discretization scheme) which can also damp the instabilities....

Good luck!

Many thanks for your responses!

Freeman: My area of interest is wheels which are not in contact with the ground (i.e. landing gear wheels) so fortunately I don't have to model the dreaded ground patch. Some of my colleagues are modelling this and I know how troublesome it can be. I am using structured grids only. I can send you some residual plots but no cl or cd as currently the results are not accurate enough to warrant these... I am going to try a number of other RANS models and perhaps do a DES, which is much more suitable for this problem, but is more grid dependent (i believe), as it is the grid resolution which determines whether the turbulence is modelled or resolved. My general strategy is to run the steady solver using first, then second order schemes, then switch straight to the second order unsteady solver one the residuals have levelled off.

Kim: I have already seen those images, and that is what I am hoping to produce at some stage, using DES.

Karicha: Thanks, I will examine the turbulence viscosity ratio settings.

Tom

Tom, Please send your results (or if published, the title of your paper and journal) to me after your simulation is successful.

I tried to simulate a turbulent flow around a highrise building. The building geometry is very complicated one. Small flat louvers covered a circular cylinder core. One of the concerns was noise generated by wind. Since wind tunnel test is almost impossible to measure the noise level, we decided to use CFD analysis. And we were not sure how to interprete the noise level from a model scale to a full scale, CFD was employed.

At first we tried 3-dim. analysis (model only 2 floors of the building)using steady state simulation and coarse meshes but the results were not satisfactory. We tried 2-dim. unsteady simulation only for half of the geometry because the geometry was symmetry. It was also failed due to high turbulent viscosity ratio. Upto this point, k-e and RSM were used. It didn't work well.

Finally I used (very?) fine mesh (Number of meshes is about 300,000) and tried LES. I got very turbulent flow field around louvers and cylinder surface and wakes. The noise level was comparable with 3-dim steady simulation results. Funny thing was that I forgot to use DES. I just simply used LES. At that time, only LES was in my mind. After a long simulation, I found that I had to use DES because my mesh was not fine enough for LES.

After the simulation using LES (with Smagorinsky model)is finished, I switched turbulence model to DES and run FLUENT again. Weird thing was that simulation results were converging to a different way compared with LES results. Then I stopped it. I hope my experience help your attack for the problem. Good luck.

Kim:

I will send you the results once I successfully simulate this problem. I am currently building a grid for a DES. When using DES, the grid is crucial, because it is the grid resolution that determines whether LES is used or an eddy viscosity model (usually just S-A) is used. The reason that your DES simulation converged to a different solution to the LES was possibly because the grid resolution was not sufficient to trigger the LES model, or that there were large regions of flow (away from the surface) where the S-A model was still being used. The ideal case is that LES is triggered in all regions of separated flow, and that the S-A model is only active in the boundary layer of the attached flow, which is where it was designed for.

For my problem, I will need a grid of at least 2-3 million GPs for an accurate DES. There is a good paper called 'Young person's guide to detatched-eddy simulation grids', NASA/CR-2001-211032, by Phillipe Spalart, which is very useful for creating DES grids.

All the best

Tom