Hi,

I'm having trouble converging a simulation of our College's solar car design... as far as the geometry is concerned, I'm using a box for the flow domain of 1500x1500x4500 (inches) for a 196" car, 5 prismatic tri layers for boundary layer resolution based on first aspect ratio of 5, 1.2 growth, largest surface tri on the car is about 1", using 200" intervals at farfield. Mesh is approx 2.9 million cells, using a non-conformal boundary between the bounding box on the car and the rest of the domain. Running Fluent beta 6.3 parallel, double precision across 25 nodes. Inlet is a velocity inlet, 25m/s flow, rear is pressure outlet, sym walls for sides and top with a moving wall on the ground, 25m/s flow. I'm using the Realizable KE model, and can converge 1st order fairly well, but moving to second order discretization, the turbulent viscosity ratio tends to diverge (ratio limits at 1x10^5 in a few cells and number of cells being limited slowly grows to around a couple hundred and stays) but x-y-z residuals and continuity residuals drop off nicely. My guess is that my initial guesses for K and E are off... I don't really know what values I should be using, so I specified by viscosity ratio and intensity, using .05% intensity at the inlet with ratio of 5, 10% intensity at the outlet and ratio of 10. If someone could help me out with ideas on how to improve the convergence, I'd really appreciate it.

Thanks,

Andy Berner Principia College Solar Car Team www.prin.edu/solar

Don't worry about the viscosity ratio. If its limited in a few hundred cells out of 2.9 million, it's no problem at all. I've seen the same effect in my automotive simulations before, and it never caused wrong results.

I did some experiments with the freestream turbulence settings, and it seemed to have little effect on the final solution. Near ground freestream turbulence is difficult to model, and in reality its intensity can vary due to wind, surface rougness, trees, buildings etc. I usually set intensity to 1% and length scale to 0.04m on the inlet and 4%/0.04m for backflow on the outlet plane.

I obtained good results with RSM as well, but it's more mesh-dependent than k-epsilon.

Try to avoid a non-conformal interface, sometimes Fluent has difficulties with it.

Vincent,

Thanks so much for the response, that's somewhat reassuring. Based on tweaking a number of settings and looking at convergence histories, I'm fairly comfortable about a realistic range for the Cl on the vehicle. The CdA, however, is varying quite a bit, and I'm not quite sure the best way to pin it down. Our vehicles are very streamlined, so viscous drag is the primary aero loss. This is of course very sensitive to the state of the boundary layer. I know fluent doesn't handle BL transition, so is there any way I can assure a fully turbulent boundary layer and then compute a drag reduction for assumed laminar based on Cp plots?

Thanks,

Andy

Hi Andy!

When you give the boundary conditions for the tunel, better always choose intensity and hydraulic dia than using intensity and viscosity ratio for turbulent discretisation.

I think Standard K-W model and SST K-W of fluent would predict transition flow. Go through the fluent overview for confirmation.

Hi,

SST K-W I've heard is better for transitional flows... the main issue there is the Y+ required for accurate near wall stuff... The mesh is currently at 3 million cells with a Y+ of around 150. When using prismatic cells for the boundary layer, I'm using first aspect ratio of five with five layers at 1.2 growth to avoid a huge volumetric gradient at the transition from prisms to tets. To get a Y+ of 5 on the model, I'd need first height of about .003 inches (assuming I'm using the Y+ calculator correctly... five meter car and Re of about 8x10^6), which would be pretty horrendous aspect ratio and give me serious grid issues; otherwise I'd have to move to an impractically fine surface mesh. I appreciate the suggestions, anyone else have thoughts on this?

Thanks,

Andy