[Jacob Flanagan]

Hi,

I am having some trouble with a CFD simulation I am running on fluent. I am trying to simulate the drag force on a cyclist travelling at 11.5m/s. I would expect a drag force of around 18-22N (definitely no less that 17N) however after running multiple simulations with different turbulence models I am only getting drag forces around 11-13N, which is far to low. Of the drag I am getting 12N of force from pressure drag and 1N from viscous drag, which seems a little low. I have examined the flow field and everything seems to be looking right in terms of flow structure. I was wondering if anyone would be able to shed some light on this issue as I am not really sure what to change in my model.

My setup parameters are as follows:
Domain size: 40m x 15.5m x 10m

Mesh sizing:
-Poly-hexcore mesh
-10 prism layers with 1.2 growth rate and 0.05mm first layer
-Global min=0.5mm max=1000mm
-far boi min=0.5mm max=20mm max
-wheel boi min=0.5mm max=10mm
-surface mesh of rider min=0.5mm max=10mm
-max skewness of volume mesh 0.91
-number of cells 7.8million

Boundary conditions:
-velocity inlet 11.5m/s
-pressure outlet 0Pa
-moving ground boundary 11.5m/s (to match inlet velocity)
-Symmetry walls
-No slip wall condition on rider and Frame
-Rotating boundary condition on wheels

Turbulence model:
I am using the SST-Kw model primarily to solve and using second order SIMPLE scheme.

If anyone has any idea on why I am getting such low values for drag I would be extremely grateful.

Thanks,
Jacob

NearWallYPlus.PNG

VelocityMagClose.PNG

VelocityMagFar.PNG

YPlus Far.PNG

Streamline 4.PNG

[flotus1]

-Rotating boundary condition on wheels

Not the only possible source of error, but the front wheel can not be accurately represented by a rotational velocity on its walls. Frozen rotor or more accurate modeling approaches would be needed for that,because some portion of the boundary has a velocity vector that is not orthogonal to the wall normal vector.
https://www.cfd-online.com/Wiki/Best...stage_analysis

The drag values you are comparing to: where do they come from? Wind tunnel testing? The CFD model seems very simplified, missing lots of small parts a regular bicycle would have. And humans tend to have a different, more complex shape.

[Jacob Flanagan]

Thanks for the advice flotus1,

For the rotating wheel I also simulated a solution with no wheel rotation and just a no slip wall condition and the result was extremely similar. My drag estimations are based off research papers such as https://www.sciencedirect.com/scienc...67610518305762 which have a CdA of around 0.25 for a cyclist similar to mine. There are also other similar studies which have made the simplifications that I have made which get more accurate results.

Would those minor simplifications cause that much decrease in drag?

Thanks.

[arjun]

Originally Posted by Jacob Flanagan

Thanks for the advice flotus1,

For the rotating wheel I also simulated a solution with no wheel rotation and just a no slip wall condition and the result was extremely similar. My drag estimations are based off research papers such as https://www.sciencedirect.com/scienc...67610518305762 which have a CdA of around 0.25 for a cyclist similar to mine. There are also other similar studies which have made the simplifications that I have made which get more accurate results.

Would those minor simplifications cause that much decrease in drag?

Thanks.

It could you never know with turbulence.



Here in this video where the tyres are rotated you could see the flow pattern at front tyre is much different than the back trye.



Rotation seems to matter


https://youtu.be/jAfJnUZAMco

[FMDenaro]

At the first glance, I would advice that computing "accurately" the drag requires a very very fine grid close to the walls. Have you estimated your y+ distribution around the walls?

[Jacob Flanagan]

Originally Posted by FMDenaro

At the first glance, I would advice that computing "accurately" the drag requires a very very fine grid close to the walls. Have you estimated your y+ distribution around the walls?

FMDenaro, how much finer would you recommend for the model? The current model has a 50um first inflation layer that can be seen in the figure I attached. Would a 10um layer be fine enough or are you thinking finer than that?

I did some rough y+ calculations but I wasn't 100% sure as the Reynolds numbers was hard to get right (not sure what the characteristic length should be) and then I also wasn't 100% sure what equation to use for the skin friction coefficient (Cf) used to determine the wall shear stress and therefore y+.

Any advice on the y+, Re and Cf calculations would also be greatly appreciated.

Thanks.

[FMDenaro]

Originally Posted by Jacob Flanagan

FMDenaro, how much finer would you recommend for the model? The current model has a 50um first inflation layer that can be seen in the figure I attached. Would a 10um layer be fine enough or are you thinking finer than that?

I did some rough y+ calculations but I wasn't 100% sure as the Reynolds numbers was hard to get right (not sure what the characteristic length should be) and then I also wasn't 100% sure what equation to use for the skin friction coefficient (Cf) used to determine the wall shear stress and therefore y+.

Any advice on the y+, Re and Cf calculations would also be greatly appreciated.

Thanks.

Viscous drag prediction requires to use a wall-resolution, that is at least 3-4 nodes having y+<=1.

[Jacob Flanagan]

Originally Posted by FMDenaro

Viscous drag prediction requires to use a wall-resolution, that is at least 3-4 nodes having y+<=1.

Thanks FMDenaro, from the figure I uploading showing the velocity profile in the near wall region, would you expect the near wall cells need to be significantly smaller to meet that criteria? Would having 3-4 nodes say between the wall and 10um from the wall be a good place to start to try and resolve that flow?

Thanks.

[FMDenaro]

Originally Posted by Jacob Flanagan

Thanks FMDenaro, from the figure I uploading showing the velocity profile in the near wall region, would you expect the near wall cells need to be significantly smaller to meet that criteria? Would having 3-4 nodes say between the wall and 10um from the wall be a good place to start to try and resolve that flow?

Thanks.

You have to compute explicitly the values of y+, that requires to evaluate the u_tau velocity. An estimation of the bulk based Reynolds number is of O(10^6) therefore you need a well refined grid, a rough estimation would suggest you need to put the nodes at a distance lesser than 10^-3 m.

[Jacob Flanagan]

Originally Posted by FMDenaro

You have to compute explicitly the values of y+, that requires to evaluate the u_tau velocity. An estimation of the bulk based Reynolds number is of O(10^6) therefore you need a well refined grid, a rough estimation would suggest you need to put the nodes at a distance lesser than 10^-3 m.

I am currently have my cell thickness at 5 x 10^(-5)m (50 micro-meters) which would suggest that the boundary layer would be resolved in that case?

[FMDenaro]

Originally Posted by Jacob Flanagan

I am currently have my cell thickness at 5 x 10^(-5)m (50 micro-meters) which would suggest that the boundary layer would be resolved in that case?

That depends not only on the node closest to the wall but on the description of the BL, that is on the next nodes normal to the wall. Again, you need to explicitly compute the y+ distribution around the body to ensure that is fully described by at least 3-4 nodes within y+. To do that you need to evaluate u_tau from your computation.

[JBeilke]

I would do a transient simulation at first.