Hello,

I'm trying to match experimental datas on forces acting on a bluff body (Transversal section of a vehicle). At present I'm dealing with 2D preliminary test. I'm using segeregated solver, first order discretization for all quantites, SIMPLE pressure-velocity coupling, and a user defined velocity profile at the inlet. The freestream conditon is "established" using FLUENT' symmetry boundary condition.... And I can't match experimental datas better than 20-30 %..... Any suggestion ?? PS: I'm using k-e RNG Non Equil. Wall-function .

Thanks !

This seems like a difficult calculation!

Do you have a good mesh? Is the problem steady state? Is it well converged? How big are your Y+ values?

You certainly should try the Spalart-Allmares turbulence model. It is very promising to be used for external aerodynamical calculations.

greetings,

Laika, still orbiting

I've found this problem to be quite mesh dependent..but I've finally refined the mesh to chatch the main feature of the flow, coarsening separated regions to reduce cells number in the view of 3D simulations...The problem is steady state and is converged ( checking residuals 10e-5). Y+ values on the surface of the body are between 8-18 near the stagnation point and between 34-60 in other region.

I'll try to change my turbulence model to Spalart-Allmaras...

Thank U.

seems like a good set-up of the problem.

How well defined is the separation point. Can you trigger the separation as such that you can have reproducable results?

Please let me know the performance of the S-A model.

Laika, still orbiting

The separation on the Upper half of the body is due to a wedge, so I don't think I can do anything to trigger that separation, while the lower part of the body is invested by a separated flow.... What do you think about freestream defined with a symmetry b.c.? I've read on the manual Pressure-Inlet is also used to define free boundary, but in some cases when I use pressure inlet the results are even worst... I'll certainly let you know about S-A.

I cannot judge the use of your boundary settings, since I haven't seen your geometry. But my experience is indeed that a pressure inlet can give some problems where it is in contact with another boundary.

These problems are only local, so if your cfd-domain is large enough, this should not be a real problem.

Can you tell a bit more about your geometry?

Laika, still orbiting

Truck over an embankment, side wind is blowing... If we say H the height of the hill my domain is 38 H length, 10 H height, Reynolds is 1.16 e+05. There's a long wake due to the hill but it is all contained in the domain (No reverse flow).... Thank you Laika.

Switch to 2:nd order schemes, at least for momentum, but preferably for all variables. The first order upwind scheme is very dissipative and inaccurate. I'd use Realizable k-eps instead of RNG.

In practise the non-equilibrium wall-functions are surprisingly good to predict separations sometimes. However, I've seen many cases where they fail completely, especially on 3D hill type of geometries etc. Then you should use a low-Re variant like the new "enhanced wall treatment" in FLUENT 6 or the "two-layer" model in FLUENT 5. You could also try a real low-Re k-epsilon model (only available in the text interface) or the new Wilcox k-w model (I've got strange results in 3D with the SST model so be a bit extra careful if you try that in 3D - might be a bug because it behaves very well in 2D. Anyone else seen this?).

This type of flow is always 3d and transient. Even a "converged" steady state solution just does not describe the original problem.

How was the measurement done? If you want to get comparable results you have to model what was done in the experiment.

Just using a 2d section from an originally 3d experiment is completely wrong.