CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Drag and Lift modelling (https://www.cfd-online.com/Forums/fluent/27862-drag-lift-modelling.html)

Desmond Hui August 29, 2000 01:04

Drag and Lift modelling
 
Hi,

Have anybody carried out CFD for getting forces (Drag and Lift) around a bluff object at Re=1e5 to 1e6 in air ACCURATELY? How to make that accurate enough down to 10% error when compair with wind tunnel? Should I carried out an unsteady analysis, should I mesh the cell near wall down to Y^+ < 30? pls. help!

yours, Desmond

John C. Chien August 29, 2000 04:01

Re: Drag and Lift modelling
 
(1). If the question is related to the use of a code, then you need to ask the support engineer of the vendor. They should give you the first hand suggestions as to how to improve the accuracy of the results. It is also a good idea to send them this unknown bluff object geometry. (2). Assuming that you are getting mesh indenpendent solution, the the only factor which can affect the result is the turbulence model used in the code. (3).So, you may want to experiment with various turbulence models available in the code. And Y+=30 is too large for low Re or two-layer models.

Sung-Eun Kim August 29, 2000 18:52

Re: Drag and Lift modelling
 
For bluff bodies, pressure drag is dominant (over frictional drag). And it's not easy to predict pressure drag accurately for bluff bodies. Inadequate modeling of turbulence is usually fingered at as the main culprit.

We've once computed, using the RSM and wall functions, the flow around the well-known Ahmed body (Re_L = 4 x 10^6) at 30 deg slant angle. The drag prediction was within 5.0 % from the measurement for this particular slant angle. For detail, see the paper SAE-2000-01-084 'Advances in External Aerodynamics Simulation of Ground Vehicles Using Steady RANS Equations".

Resolving the inner TBL all the way down to wall (y+<1.0) doesn't reward much for its cost. In fact, it can worsen the result, inasmuch as you might end up streching your mesh rapidly in the boundary layer, in order to keep the cell count within your computer capacity. Here're some you may want to keep in mind.

Use layered cells (hex or prism) in the near-wall region. Make sure that the front stagnation region and the near-wake are properly resolved (don't use too much expansion in the near-wall meshing). Use one of the more advanced turbulence models in FLUENT.Second-moment closure is recommended along with higher-order discretization scheme.

Depending on the geometry and Reynolds number, VLES or LES might be needed to account for the effects of coherent structure, if any, in the near-wake.


All times are GMT -4. The time now is 04:44.