# Drag and Lift modelling

 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 29, 2000, 01:04 Drag and Lift modelling #1 Desmond Hui Guest   Posts: n/a 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

 August 29, 2000, 04:01 Re: Drag and Lift modelling #2 John C. Chien Guest   Posts: n/a (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.

 August 29, 2000, 18:52 Re: Drag and Lift modelling #3 Sung-Eun Kim Guest   Posts: n/a 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.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post icemaniac178 CFX 6 August 17, 2011 18:40 Josh CFX 24 May 9, 2011 10:38 Yogibear STAR-CCM+ 4 June 20, 2010 10:11 zx Main CFD Forum 4 July 27, 2007 23:38 Noé Siemens 5 July 13, 2004 10:21

All times are GMT -4. The time now is 10:08.