Hi everyone,
I am trying to simulate turbulent flow over a sphere with the following conditions:
Freestream velocty= 100m/s
ambient density and viscosity
Sphere diameter = 0.82 m
Reynold's number = 5.6 x 10^6
experimental Cd = 0.195
Sphere enclosure = 42 x 28 x 28 m3
mesh Size 4.5 milllion
I tried using S-A model and K-omega SST model in fluent, using which I am getting Cd=0.14. which is almost 26% error.
Any suggestion as to how may I improve the result?
WMLES or SBES model with a well thought (and validated) mesh resolution.
Regards,
Dr. Th. Frank.
PS : Your question did not involve any limitations on the computational time of the proposed turbulence modeling approach. Therefore a scale-resolving simulation would clearly deliver the best possible results (I'm not proposing a diret numerical simulation, since you asked for turbulence modeling approaches; DNS is resolving turbulence, but not modeling it).
This subject has already been treated by many authors. At a Reynolds number of approximately Re = 3.8 ×105, the boundary layer switches from being predominantly laminar to predominantly turbulent, hence the separation point moves further downstream, the wake narrows, and the drag coefficient drops considerably, from around Cd = 0.40 at Re = 1.0 ×104 to approximately Cd = 0.08. A further increase in Reynolds number then leads to a slow increase in the drag coefficient again until Cd ∼ 0.20 at Re ∼ 4.0 ×106. The Fluent LES simulation at Re = 1.0 ×106 adequately captured this behaviour.
Here are some results reported in the literature.
At Re = 1.0 x 106 values of Cd are:
Fluent : 0.104
Constantinescu, G.S. and Squires, K.D (2004): 0.08
Wang, Z.J. and Kannan, R (2005): 0.09
Achenbach, E (1974): 0.12
Jones, W.P. and Launder, B.E (1972): 0.139 - 0.142
Jindal, S., Long, L.N., Plassmann, P.E. and Sezer-Uzol, N (2004): 0.141
Regards
- Badges
- Science topic