Discussion Groups

Simulation CFD

5 Posts
0 Kudos
Registered: ‎06-25-2012
Accepted Solution

Calculating Drag of Ahmed Body

1060 Views, 1 Replies
06-27-2012 01:12 PM

I am trying to find Drag coefficient of Ahmed Body in Simulation CFD 2013.

My boundary condition are


I am using formula for drag


As Drag force is half because area of cross section is half, so I didn’t change any coefficients.

For FD  I have taken value of Fx which I got the value -759.685N and area of cross section 0.057516m2

I got value of CD as 5.83

I don’t know where I have done wrong.

Is it correct procedure to find drag?

Can I take the value of Fx  as FD?

Please help me.

I am uploading geometry file and results file

Please tell me if there is another way

3 Posts
2 Kudos
Registered: ‎08-01-2011

Re: Calculating Drag of Ahmed Body

07-03-2012 07:19 AM in reply to: p.raviteja1992



Thanks for your post. I've posted a share file here which shows an optimum setup for simulating the ahmed body aerodynamics. The list below goes over some of the non-default modifications contained in the file:


1. 40 m/s inlet velocity (the most common velocity to test the Ahmed body, most published papers use this velocity.)

2. Slip walls used for the symmetry plane, and the top and side of the wind tunnel.

3. Uniform mesh distribution applied for the body surfaces (including standoffs)

4. Mesh surface refinement enabled

5. Automatic convergence settings to "tight"

6. Advection scheme: ADV5

7. Turbulence model: RNG

8. Adaptation settings: 3 cycles, y+ option set to 100 (You can choose to save cycles if you wish)

9. 2000 iterations


I created two surface groups for the body, one with standoffs included and one with them excluded. This makes it easy to assess drag forces with the wall calculator since you can select either of these groups via the group operation. Drag will be the sum of the forces in the X direction.


The original lab test for this model showed a drag of approximately 16.1N for the 25 degree slant and 13.9N for the 35 degree slant (I've adjusted for the half model). With the turbulence models employed in Simulation CFD (k-epsilon, RNG, etc), we can realistically expect drag to be reported on the high side. Flow trends will be reported correctly.





James C. Neville
CFD Subject Matter Expert