Too low drag coefficient on a bus
Hello,
I have a bus geometry (in original size). I made a simulation to investigate the drag coefficient. I think, the mesh is quite fine, the y plus is 20100. But based on result, the drag force is very low. I made analytical calculation where the force is ~ 1800N but this value was ~ 800900 in the simulation. I made a very simple geometry to investigate this problem. So in this moment I have a simple body without fillets and chamfers. Main sizes of body are same to the original bus geometry. The drag force has shown correct value in this simple geometry. (compared to te analytical calculation.) So after this I created some small fillets to the edges. Based on the result, the force is lower. From ~1800N => ~800900N. I can not imagine that this reduction is the effect of the fillets. Based on general measurements, the drag coefficient of a bus should be ~ 0,60,8. This value is ~ 0,3 in my simulation. The calculation has been converged. I have investigated the mesh sensitivity but it caused only 35% changing in terms of the drag force. I am using SST turb.model. What can be the problem?? Best regards Roland 
Could be number of things. You need to do a parameter sensitivity. Could be mesh issue. SST turbulence model recommendation is y+ <= 1. Your mesh in BL might not be enough, do you have at least 10 nodes through BL. Separation might not be accuratately captured.

Have you considered the basics: http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F

Dear all,
thank you for your help and suggestions. I tried to make more exact mesh. The y plus is lower than 1. I use 13 layers in the BL. Value of the cd is ~0,5. I think that this value is low still, in the reality it is ~ 0,60,8. My geometry is not too ideal in terms of aerodinamics therefore I think, cd sholud be ~ 0,60,7. Could you help, where can I find/download simple measurements in connect with this problem to validate accurary of my calculation? Thanks Roland 
I do not fully understand what you are saying. Did you say that your geometry is not exactly the same as the experimental results? If that is the case then the path forward is pretty obvious.
For a good reference flow for this with lots of well validated results look for the Ahmed body. It was designed to be a simple body which captures most of the large scale aerodynamic effects for a car. This geomnetry has lots of high quality experimental and CFD results so you should be able to do a good benchmark to it. 
Hello Glenn,
thank you for your help. I searched after measurements of the Ahmed body. I made a simulation with this geometry and the drag coefficient is very exact in my calculation. The y plus is above 20 and under 100, the bondary layer contains 14 cells. But based on this results, I don't understand a previous comment from Singer1812: "Could be mesh issue. SST turbulence model recommendation is y+ <= 1." When does the y plus have to be under 1? A teacher (on the university) teached for me that the y plus has to be set up based on the Re number. Is this statement correct in any cases? Thanks Roland 
It is a requirement of the SST model since it is a combination of turbulence models. Unlike kepsilon is able to resolve the wall condition better, but with the requirement that there be higher mesh resolution. It is also recommended that you not only make it so your first layer thickness results in a y+ value around 1, but also that you shoot for 15 inflation layers.

Like Torque_Converter said, the SST model is a meld between kw and ke turbulnece models. If you don't have a y+<=1 for the SST model, it behaves like the ke model and you dont get the benefits from the kw portion.
This is not in of itself bad, and may be fine for alot of geometeries and flow types. As an example of one detail between SST and ke models, drag can be a function of separation, which if properly implemented, the SST model can do better than the ke model. 
OK, I understand it, Thank you for your help.

All times are GMT 4. The time now is 21:51. 