## Formula One wheel aerodynamics

Here are our CFD links and discussions about aerodynamics, suspension, driver safety and tyres. Please stick to F1 on this forum.
0
Hey,

I have just been told by, fluent help, that I have to place my rotating wheel slightly above the bottom of the wind tunnel, however this would not be a true study of the aerodynamics around it. However, I have seen people doing analyses with the bottom of the wheel slightly cut off/straight and they have placed it at the bottom of the wind tunnel. Does anyone know if this is possible and would I have to follow the same principles in setting the boundary conditions as the one with the wheel slightly above the bottom of the wind tunnel.

I am using GAMBIT 2.4.6 to model it and Fluent 6.3.26 to run it.

Abz
a6zz
0

Joined: 21 Dec 2008

0
I would not go along with their suggestion. As always with CFD, the simulation is only as accurate as you make it. If the wheel is sitting 5mm off the ground in real life, then we should model it as such in CFD. If not, then our results will not be accurate with the assumption they have given you.

I would model the wheel as a deformed body. Simply lop off a section at the bottom...this is more or less what happens in real life anyways. Be sure that the rotational velocity you assign to the wheel surfaces matches up to the linear velocity of the ground plane. Done and done.
slimjim8201
9

Joined: 30 Jul 2006

0
Hi,
I was interested in performing a simulation of this sort of thing before but never got around to it, there is a good bit of info in the literature on rotating wheels. I found this link from the fluent website actually.

www.fluent.com/solutions/automotive/ex1 ... _wheel.pdf

They say they used a flattened patch which was in contact with the ground so it must be possible! Interestingly they have pressure coefficient results from experiment and cfd so it would be good if you set up the problem like that and then compare the results to benchmark your simulation and then evaluate what you want afterwards. Let us know how you get on with it.
mikhak
0

Joined: 10 Jul 2006
Location: Stockholm

0
Hi

I am performing this analysis at the moment however when I am comparing it against the theoritical values given in the .pdf file above I can't seem to capture results from fluent in terms of different degrees, like at 90, 180... degrees to the wheel also I do not know which area they have used to calculate the coefficient of pressures

Does anyone have a clue?

ohh and also does anyone have a copy of

CFD Simulations and Experimental Measurements of the Flow Over a Rotating Wheel in a Wheel Arch, SAE Paper No. 2001-01-0487, 2000
A. F. Skea and P. R. Bullen

cheers
a6zz
0

Joined: 21 Dec 2008

0
well to get the cp data from the wheel on a single plane.....create a circle

in Surface/Quadratic, under Type select Circle and input x0, y0, z0 as coordinates for the centre of the circle and then r2 for the radius of the tyre.
Then in Plot xy you can select this Circle you've created and plot cp versus x(pos).
Use trigonometry to turn xpos into theta, i suggest writing the data to a file and then mess around with it in a spreadsheet like Excel. As far as i know fluent will write the data to the file starting at the extreme right of the circle and go in an anti-clockwise direction so that 90degrees is the top of the tyre, 180 is the front and 270 is bottom.
so to get from xpos to theta and also to rotate the coordinates so that 0degrees corresponds to the front, 90 to bottom, 180 to rear and 270 to the top (just like in the .pdf) use the following 2 equations on the data.....
Eq.1 for the top surface (ie. the first half of your data) 180+cos-1(x/R)*180/pi
Eq.2 for the bottom surface....... 180-cos-1(x/R)*180/pi

Theres probably a far simpler way of doing this but so far i havent found any way of plotting it with fluent alone.
mikhak
0

Joined: 10 Jul 2006
Location: Stockholm

0

Mikhak do You mean create a circle on the wheel, or just simply a circle within a wind tunnel (2D CASE)?

And also equation one and two, the value of R, i take it is just the radius of the wheel?

Abzz
a6zz
0

Joined: 21 Dec 2008

0
Yes i mean create a circle on the wheel. You just create the circle in fluent to get the data points, it doesnt affect the flow in any way, its just to get the data from the wheel.
If you're doing a 3d case then you can specify where u want to take the data from by adjusting the z position of this circle you create.
And yes R is the radius of the wheel. I hope you understand where these equations come from, its simple trigonometry but a bit mixed up cos of the way in which fluent writes data to files and the way you have to rotate it to get the theta from the correct reference.
mikhak
0

Joined: 10 Jul 2006
Location: Stockholm

0
Good Morning to all.

I have been working ona rotating wheel vehicle simulation. First, I did some simulations of the whole vehicle without rotating wheels and they converged giving reasonable results. Then I just put the wheel to rotate in a free environment (without the wheel well) and again it converged and gave reasonable results.Anyways, when I try to join both things the simulation diverges.

I have tried to refine the mesh inside the wheel well (although I don´t know if it is still to coarse)and it hasn´t worked. I have even tried to simulate 1/4 of the car (just to check on convergence) but it still diverges.

The link goe to an image of the geometry.

I cut the wheel on its bottom a little bit to make the simulation more real. The body on the wake is just an aid for a mesh refinement. My mesh is no dynamic. I just put a condition in the wheel of a rotating wall which is congruent with a moving floor.

I would appreciate very much if someone could give me a hint.

Thank you very much,

http://postimage.org/image/8mwj2dwud/dcdc4148/
Natalia Castro
0

Joined: 14 May 2012

0
In windtunnel testing you never put the vechicle on the actual tunnel floor the always but it on a raised floor so they can simulate laminar flow moving across the boundary of the road surface. I think it called "tripping" the boundary layer.

This due the windtunnel walls weather they are open or closed will generate a boundary from the flow streighteners. that will go from laminar to turbulent by the time the flow gets to the test subject.

This is the reverse of what happens in reality where the body is moving assumed "stagnated" flow over and under around and through the body of the vehicle.

Other problem is the flow interaction between the front wing and wheel assumed open wheeled will give different results to just simulating the wheel on it own.
Smokes
1

Joined: 30 Mar 2010