Too low drag coefficient on a bus

Roland R · September 12, 2012, 09:46

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 20-100. But based on result, the drag force is very low. I made analytical calculation where the force is ~ 1800N but this value was ~ 800-900 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 => ~800-900N. 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 ~ 0,6-0,8. This value is ~ 0,3 in my simulation. The calculation has been converged. I have investigated the mesh sensitivity but it caused only 3-5% changing in terms of the drag force. I am using SST turb.model.

What can be the problem??

Best regards
Roland

singer1812 · September 12, 2012, 10:53

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.

ghorrocks · September 12, 2012, 18:51

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

Roland R · September 14, 2012, 10:34

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 ~ 0,6-0,8. My geometry is not too ideal in terms of aerodinamics therefore I think, cd sholud be ~ 0,6-0,7.

Could you help, where can I find/download simple measurements in connect with this problem to validate accurary of my calculation?

Thanks
Roland

ghorrocks · September 15, 2012, 07:05

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.

Roland R · September 20, 2012, 08:09

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

Torque_Converter · September 20, 2012, 08:50

It is a requirement of the SST model since it is a combination of turbulence models. Unlike k-epsilon 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.

singer1812 · September 20, 2012, 09:15

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.

Roland R · September 21, 2012, 05:23

OK, I understand it, Thank you for your help.

September 12, 2012, 09:46	Too low drag coefficient on a bus	#1
Roland R Senior Member Roland Rakos Join Date: Mar 2009 Posts: 131 Rep Power: 17	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 20-100. But based on result, the drag force is very low. I made analytical calculation where the force is ~ 1800N but this value was ~ 800-900 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 => ~800-900N. 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 ~ 0,6-0,8. This value is ~ 0,3 in my simulation. The calculation has been converged. I have investigated the mesh sensitivity but it caused only 3-5% changing in terms of the drag force. I am using SST turb.model. What can be the problem?? Best regards Roland

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Drag Coefficient Convergence Problem	John	FLUENT	18	June 24, 2023 09:22
low drag coefficient	Jason	FLUENT	3	August 14, 2008 00:53
Energy dissipation and Drag coefficient	Freeman	Main CFD Forum	10	January 27, 2006 07:42
about the drag coefficient	maximus	Main CFD Forum	7	April 18, 2005 19:00
Multicomponent fluid	Andrea	CFX	2	October 11, 2004 05:12

September 12, 2012, 10:53		#2
singer1812 Senior Member Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 511 Rep Power: 20	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.

September 12, 2012, 18:51		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Have you considered the basics: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

September 14, 2012, 10:34		#4
Roland R Senior Member Roland Rakos Join Date: Mar 2009 Posts: 131 Rep Power: 17	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 ~ 0,6-0,8. My geometry is not too ideal in terms of aerodinamics therefore I think, cd sholud be ~ 0,6-0,7. Could you help, where can I find/download simple measurements in connect with this problem to validate accurary of my calculation? Thanks Roland

September 15, 2012, 07:05		#5
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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.

September 20, 2012, 08:09		#6
Roland R Senior Member Roland Rakos Join Date: Mar 2009 Posts: 131 Rep Power: 17	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

September 20, 2012, 08:50		#7
Torque_Converter Member Join Date: Jan 2012 Location: Edmonton, CA Posts: 87 Rep Power: 14	It is a requirement of the SST model since it is a combination of turbulence models. Unlike k-epsilon 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.

September 20, 2012, 09:15		#8
singer1812 Senior Member Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 511 Rep Power: 20	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.

September 21, 2012, 05:23		#9
Roland R Senior Member Roland Rakos Join Date: Mar 2009 Posts: 131 Rep Power: 17	OK, I understand it, Thank you for your help.