Need some help from all the Aeroheads over here for my final year project.
i have conducted a few wind tunnel tests for a simplified race car model, and i compared these results to my CFD simulation results. The results were quite close to each other for both simulation and test. For this i consider my CFD simulation is valid and verified. But generally i observe a trend:
The drag coefficient for CFD simulation is higher than drag coefficient for a wind tunnel test.
can anyone please suggest any possible reason for this?
Need some help from all the Aeroheads over here for my final year project.
i have conducted a few wind tunnel tests for a simplified race car model, and i compared these results to my CFD simulation results. The results were quite close to each other for both simulation and test. For this i consider my CFD simulation is valid and verified. But generally i observe a trend:
The drag coefficient for CFD simulation is higher than drag coefficient for a wind tunnel test.
can anyone please suggest any possible reason for this?
thanks in advance.
It depends on a lot of things and I mean a lot.
The quickest solution I could suggest is to check your y+ value, if you are using the Spalart Allamaras model then make sure your y+ is between 30 and 45. Drag is calculated by integrating the log law of the wall, i.e, your y+. If thats not correct then your Cd values would not be correct either.
Using what turbulence model (I assume they were RANS based simulations)? The k-omega SST turbulence model is generally accepted as the best of the two equation models*.
What solver did you use? (CFX, Fluent, Star etc?)
Wall functions generally shouldn't be used in sims with adverse pressure gradients, so I would recommend a y+ of around 1 for fluent, and 1-2 for CFX (haven't used star so can't say, consult your manual).
Even if your y+ is good, if there isn't enough mesh nodes in the Boundary Layer you won't get prediction right, should be around 10-15 nodes in the BL. But since you are indicating good lift agreement I assume thats ok.
The k-epsilon model isn't great in the low Re region near the wall, and will tend to over predict the turbulent shear stresses. This is due to it violating the observation of Bradshaw "that the principal turbulent shear stress is proportional to the turbulent kinetic energy in the wake region of the boundary layer". AKA, the numerically model in the k-E equations cannot and do not represent this proportionality properly.
*uhh, see the paper (goes searching) this will explain everything in much better detail:
Menter, F.R.
Two equation eddy viscosity turbulence models for engineering applications
AIAA Journal Vol. 32 No 8 1994 (August)
Get a copy of this, it should be available in your uni library, and take the relevant stuff from it and be sure to cite it as a reference.
Most turbulance models over predict the attachments and don't seperate as early as the true flow. SST is the best for areas of stong adverse pressure gradients as its one of the best at predicating transition and seperation
Educated guess...you are using fluent...terrible at drag predications; out by a factor of two sometimes
Need some help from all the Aeroheads over here for my final year project.
i have conducted a few wind tunnel tests for a simplified race car model, and i compared these results to my CFD simulation results. The results were quite close to each other for both simulation and test. For this i consider my CFD simulation is valid and verified. But generally i observe a trend:
The drag coefficient for CFD simulation is higher than drag coefficient for a wind tunnel test.
can anyone please suggest any possible reason for this?
thanks in advance.
It depends on a lot of things and I mean a lot.
The quickest solution I could suggest is to check your y+ value, if you are using the Spalart Allamaras model then make sure your y+ is between 30 and 45. Drag is calculated by integrating the log law of the wall, i.e, your y+. If thats not correct then your Cd values would not be correct either.
Hope this helps and good luck.
Spalart-Allamaras only uses EWT (enhanced wall treatment), so Y+ values need to be less that 1, or rather the first cell much be as close to one as possible. Just dont let the first cell fall in the buffer layer (anywhere between 4-15)
RACKITUP wrote:
Spalart-Allamaras only uses EWT (enhanced wall treatment), so Y+ values need to be less that 1, or rather the first cell much be as close to one as possible. Just dont let the first cell fall in the buffer layer (anywhere between 4-15)
As far as I was aware, the S-A model in fluent triggered to wall functions at around 12/13.
You are supposed to be able to use it for low Re (Y+ 1) or wall funct (Y+30-60). Indeed, I've used it both ways in the past and it works all right for attached flows.
RACKITUP wrote:
Spalart-Allamaras only uses EWT (enhanced wall treatment), so Y+ values need to be less that 1, or rather the first cell much be as close to one as possible. Just dont let the first cell fall in the buffer layer (anywhere between 4-15)
As far as I was aware, the S-A model in fluent triggered to wall functions at around 12/13.
You are supposed to be able to use it for low Re (Y+ 1) or wall funct (Y+30-60). Indeed, I've used it both ways in the past and it works all right for attached flows.
CFD analysis is still a new tool in my arsenal, but from my research (see reference) S-A is great for for a lot of flows but will need a well defined grid, y+ less than one.
(I doubt fluent would switch to wall functions at 12-13 as 11 is the worst vlues possilbe; right smack bang in the middle of the buffer region)
rkp
