Hi! I am using CFD software, Rampant, to get the power spectral density of pressure force on the building wall. My model is 2D(unsteady RNG k-epsilon model). I am comparing my result with wind tunnel results. I am using a square section of 76mm x 76mm as my model building.But my result is not camparable with that of wind tunnel result. Is there anyone who has worked on this? I need help.

Thanks in advance

Khan

Is there a reason to run your calculation 2d. This is a very strong simplification.

So try to run you case in 3d. If you dont't have enough computing power start with a coarser mesh at first.

Hi,

The flow around a square cylinder at the Reynolds number of 22,000 (based on the length of the square) or in that neighborhood has been one of our test cases since our early days. I can tell you that 2D RANS calculation with either the RNG k-epsilon or Reynolds-stress transport model gives fairly good results in terms of drag and Strouhal number.

The mesh should be fine enough to resolve the salient features of the flow, i.e., recirculation region downstream of the front edge, shear layer between the recirculation region and the freestream, the wake, particularly the near-wake. I would recommend to use high-order discretization scheme (second-order upwind).

The time step should also be reasonably small. I recall that I have used the time step size so that one shedding period is covered by 50 time steps. The first-order temporal scheme would suffice. But if you want, you could try the second-order scheme.

If you have still have problems, you can contact me directly.

I doubt that the flow around a building is comparable to a square cylinder for 2 reasons:

1) The dimensions of a building (not speakink about TV Towers) are in the same order of magnitude, where the square cylinder should be very long compared to the other dimnsions.

2) If your building is very high ( more like the test cylinder) you should not forget the effect of the atmospheric boundary layer

What was the free stream Mach number used in the 2-D square cylinder test case? Was that a compressible flow test case or an incompressible flow test case? If RAMPANT was used in the low speed flow, is there a lower limit on the free stream Mach number? I have used RAMPANT for transonic flow calculations, but normally I use UNS for low speed flows.

Dr. Chien, it's a low subsonic flow. Although known as a compressible flow solver, RAMPANT has been able to effectively deal with incompressible flows as well thanks to the preconditioning. There shouldn't be a lower limit in terms of Mach number. Since you specifically metioned our products, I will take this opportunity to brief you on our recent progress. RAMPANT and UNS are now fully integrated in a single code FLUENT 5, in which RAMPANT is available as one of many solver options. Another thing you might be interested in, especially if you've used only early version of RAMPANT, is that we haved added a "coupled implicit" solver option in FLUENT 5.

As to the choice of the solver for different speed regimes, I concur with you and would do the same as you do.

Thank you very much for your timely information about FLUENT 5. As a matter of fact, I have just attended a short training course on GAMBIT a few days ago. But I havn't had a chance to check out the new version.