CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Ahmed body simulation (http://www.cfd-online.com/Forums/fluent/102642-ahmed-body-simulation.html)

 alenglaro May 30, 2012 12:18

Ahmed body simulation

Here the continuation of the thread about meshing of Ahmed body :)

 Far May 30, 2012 12:23

http://www.cfd-online.com/Forums/ans...tml#post363879

Do you think that the turbulence intensity has such a huge impact on drag?

 alenglaro May 30, 2012 12:28

I don't know how much is relevant but with default 10% cd was about 0.35. With 0.25% 0.289.

 alenglaro May 30, 2012 12:33

Quote:
 Originally Posted by scipy (Post 363876) Did you read any of the Ahmed body papers? :) Usual turbulence intensity of the free stream airflow in a windtunnel is around 0.25 %, so me using 1 % is already a bit higher and more "real world"-like, but 2.5 is unnecessary. You (and most others) seem to confuse a no slip wall and a no shear wall. No slip wall is what I've used for the ground and the ahmed body (since that's what they are, stationary walls with shear stress or 0 slip). However, for the side and top wall - if you are going after ultimate accuracy and recreating exact wind tunnel conditions, then those walls should also have a boundary layer (same as the ground and the Ahmed body itself), but since most of the time they're far enough away to only affect the solution a little bit (if left as no slip), they can be given no shear stress boundary conditions so their viscosity effects will be disregarded. Since this is mathematically the same as a symmetry BC for Fluent, I used that for simplicity. /edit, seems you have read about turbulence intensity :)
[/QUOTE] Sorry, 2.5% was a typing mistake :)

About no-slip wall and no-shear wall, I knew the the difference, I was just wondering if using one instead of the other could affect the solution. But if it's for simplicity now I try with symmetry

 alenglaro May 30, 2012 13:50

1 Attachment(s)
Simulation completed
Here settings used:
-Coupled with pseudo-transient, first order on momentum and turbulence kinetic energy and dissipation rate for 25 iterations and then switch to second order
- explicit relaxation factors to default except for Pressure and momentum at 0.4 and turbulent viscosity to 0.95.
-Automatic time-step method with Timescale Factor=10
-bcs with 1% turbulence intensity and symmetry also on top and lateral surfaces
-fmg initialization with default settings

Convergence in 168 iterations and 55 minutes ( about 20 seconds per iteration)
Cd=0.27444
Cl=4.2129e-02
(unfortunatly i forgot to hard copy cl and cd histories)
maximum residuals at 10^-5

 Far May 30, 2012 14:07

did you compare to experimental values? How much error is there?

What is the slant angle in current simulation and are you going to try the URANS?

These results are taken with mesh3? Try to refine mesh to 4 million and see the results.

 alenglaro May 30, 2012 14:53

I've found different experimental values for cd, from 0.25 to 0.295. For the LSTM case i found two values: 0.279 and 0.285. The ercoftac case 9.4 on which I rely doesn't report cd but only velocity profiles and pressure coefficients in some locations along the body. I have to compare those values but it will take some time. For cl I found a value of 0.004.
I used 35° configuration. I don't think I will perform a URANS simulation, I'll rather try different turbulence models to match velocity profiles as much as possibile.

 alenglaro May 30, 2012 14:58

Results are taken on mesh 3. Do you think wake zone should be refined? And at the beginning of the slanted surface? That point should be critical for flow separation

 Far May 30, 2012 15:01

http://css.engineering.uiowa.edu/~me...medcarrodi.pdf

I think mesh is similar to used by Rodi in above paper. However it is always necessary to check the mesh independence.

 alenglaro May 30, 2012 16:16

I checked yplus on veicle surface and it's between 0.05 and 1.05. Is is necessary to have such low values? Shouldn't it be sufficient between 1 and 5?

 scipy May 30, 2012 18:27

The most recent paper I could find that listed Cd and Cl for the Ahmed body was "Experiments and numerical simulations on the aerodynamics of the Ahmed body" by W. Meile, G. Brenn, A. Reppenhagen, B. Lechner, A. Fuchs in which they reported the experimental Cd of 0.279 and Cl of 0.004 for the 35° slant.

This means the agreement of Cd with the experimental value was within 0.95 % and Cl was unfortunately an order of magnitude higher at 0.044 (11x higher). However, the same paper lists their numerical figures at 0.276 for Cd and 0.013 for Cl which is again 3.25x higher than experiment.

 Far May 30, 2012 22:21

Quote:
 I checked yplus on veicle surface and it's between 0.05 and 1.05. Is is necessary to have such low values? Shouldn't it be sufficient between 1 and 5?
Yes, you are correct. Y+ between 1 and 5 is sufficient.

 Far May 31, 2012 10:48

http://www.cfd-online.com/Forums/ans...tml#post364079

 Far May 31, 2012 17:15

I have used "Higher order term relaxation" technique to accelerate the convergence.

 lihuang December 14, 2012 12:44

1 Attachment(s)
Quote:
 Originally Posted by Far (Post 364081) few updates are available here http://www.cfd-online.com/Forums/ans...tml#post364079
Hi Far,

Thanks for the tutorial. But i am having trouble to create a full car body mesh when i mirror your blocking. Basically what i did was, first, mirror the geometry and blocking, and set associations for some edges and vertices. Everywhere else looks good, except the part showing in the attached pic. The problem is i have some mesh lines converged to some points. But i have checked the Pre-mesh params for that edge and parallel ones to make sure proper params. How can I fix this part of mesh?

 lihuang December 14, 2012 13:04

Quote:
 Originally Posted by lihuang (Post 397591) Hi Far, Thanks for the tutorial. But i am having trouble to create a full car body mesh when i mirror your blocking. Basically what i did was, first, mirror the geometry and blocking, and set associations for some edges and vertices. Everywhere else looks good, except the part showing in the attached pic. The problem is i have some mesh lines converged to some points. But i have checked the Pre-mesh params for that edge and parallel ones to make sure proper params. How can I fix this part of mesh? Thanks for your help!
Hi Far,
The problem was just solved by remove association of that edge in problem. Don't know why it happened tho.
Thanks again!

 Far December 14, 2012 13:06

:) .................:D

Ahmed body

Hi all,
Thank you for your help Far. In fact I'm new in CFD and I have to work on the Ahmed body. I've seen your files ".tin" and ".blk" . What do they concern exactly ? I mean, is there one for the geometry and one for the mesh ? And do you know if it's possible to import and to work with it on OpenFOAM ?
Thanks a lot,

 scipy March 9, 2016 05:29

.tin is the ICEM CFD geometry file and .blk is the ICEM CFD hexa blocking file. You need to have ICEM CFD installed to open either of these files, then you need to generate a pre-mesh, convert it to an unstructured mesh and export in a file format compatible with OpenFOAM.

Far has a series of video tutorials on YouTube that cover the whole subject of the Ahmed body in ICEM CFD hexa. (https://www.youtube.com/watch?v=2baEaHAI-08)