Mesh sensitivity "holes"

[MadMatt]

Matteo's message in the KVRC 2015 thread about mesh sensitivity made me realize I never talked about mesh sensitivity "holes" as I call them. To summerize, when you do CFD you have to evaluate your results to the mesh, which gives you something like this:



As you see here for a hillclimb Subaru Impreza I designed 2 years ago, the lift coefficient suffer from drops as the cells number increases (these are the "holes" I am talking about).

3.5m cells


5.7m cells


10m cells


21.3m cells


45.1m cells


59.4m cells


80m cells


To this day I still have no explanation of what is really happening here. One would tend to trust the results with higher cell numbers and cleaner residuals which is the reason why I chose to run all this project with the settings of the 10m cells model, but I am still very surprised about the variation of results.

I used a k-epsilon solver, steady state, with rotating wheels, an air speed of 100mph and big control volume so no blockage involved, and I had a very fine control volume right behind the car to capture the wake precisely.

This issue came to me recently with the KVRC 2015 competition so I was wondering if this is something common or just with me (and the settings I am using). My understanding is that some aero phenomenon (vortices) are badly captured with some models and how the cells are built, but that is not really a scientific answer.

You also get the case where you do a minor adjustement to the car (changing slightly an end plate for example) and the results vary by something like 20% which is absolutely not correct. I think this is linked with the issue I am mentioning here.

Anybody got the answer to this behavior?

P.S.: The models above 25m cells were ran on a cluster with tons and tons of RAM, there is no way I could have done this on my computer even with 32GB of RAM!

[mep]

I try to give an explanation from my experience.
Too small mesh elements can cause wrong spikes in pressure, which probate to neighbouring elements, giving wrong results. Obviously, the smaller the mesh the higher the probability for this occurrence. So a finer mesh is not necessarily better. It needs to be balanced.

[MadMatt]

It makes sense. Haven't checked skewness angle for all simulations, but I am not sure this would cause the issue you mention.

Strange tho as serious automotive/motorsport simulations are ran with models well over 100m cells, so they wouldn't do that if they couldn't trust the results. Again this model was refined where needed (wake, rear wing) and the mesh looked mint, hence why it can only be an issue similar to what you are saying.

[olefud]

Would the “dynamic” discussion 8/7/14 apply;

http://mccabism.blogspot.com/

[mandark]

Hi Matt

While increasing mesh resolution, are you maintaining y+? Not sure if boundary layer functions alone would cause those changes in CL though, seems more like you have yet to reach mesh independency in a critical area.

[n_anirudh]

Can you do a structured meshing and progressively increase the resolution in high gradients and post results?

[MadMatt]

Hi Matt

While increasing mesh resolution, are you maintaining y+? Not sure if boundary layer functions alone would cause those changes in CL though, seems more like you have yet to reach mesh independency in a critical area.

When I increased mesh resolution I just reduced the cells size but the prism layer thickness remained the same so the y+ should remain the same as well.

Can you do a structured meshing and progressively increase the resolution in high gradients and post results?

I am afraid I cannot do this anymore as (if I understand correctly) you want me to do this at very fine mesh? I did the 40m+ cells models on a cluster. But tell me more specifically what you want and I might try this with the KVRC 2015 model that I have now

[n_anirudh]

I may not be understanding what "prism layer" is. Is it possible to manually place grid points and successively increase them until you reach convergence? Have you done any base line studies to compare with other work?

May sound tedious, but start off with a simple airfoil and obtain convergence.

[MadMatt]

I may not be understanding what "prism layer" is. Is it possible to manually place grid points and successively increase them until you reach convergence? Have you done any base line studies to compare with other work?

May sound tedious, but start off with a simple airfoil and obtain convergence.

I obtained convergence. If you take a look at the residuals they have converged. I didn't show my values of interest, but they converged.

[gixxer_drew]

and what happens when you optimize your geometry for every mesh density...

[erikhfp]

I think what might be happening is that you are capturing smaller flow effects such as vortices. What happens when you have, lets say one element where a vortex would normally be, you tend to average the effect of that vortex in that area and its effect is not present.

The problem with vehicle models are that they are extremely resource intensive and its hard to run a full model on a normal computer and they have a ton of places which generate different flow effects and I know that formula 1 is the industry which uses the largest amount of elements (I recall a number of 10^9) to capture small flow effects.

I have also found that the SST k-omega model better captures real life flow effects and it might actually be your solver which is causing problems as I have also found that mesh convergence tends to be different for some models as the turbulent viscosity calculated by each one is different. I have had cases where a k-epsilom model would predict a large turbulent area where in fact there is only a small one.

It is difficult to say exactly what could be causing the variation in your results without having a validated case to compare the mesh results and turbulence models with and that is exactly why formula 1 teams use wind tunnels because they can then validate their cfd models as well as gain actual results for their car.

Your residual plot has some oscillations which can be damped by under relaxing some of the equations such as the momentum equation.

[MadMatt]

Thanks for the answer erik. I haven't been able to test the SST model unfortunately but I heard the same, that it may be more suited to vehicle aero. Anyway I needed to perform all my simulations in a limited time scale so I needed a robust and forgivable model hence why I chose k-epsilon which to be honest is quite well adapted as well.

But the theory in which the finer the mesh, the more variations you are getting is not that stupid in the sense that as it was said in this thread, you would get quite a lot of error propagation, eventho the mesh is refined in key areas.

andrew, I haven't tried to do this at the time, the aim was just to do a mesh sensitivity analysis. What is you idea behind your proposal? Do you think you would get much different optimum airfoil AoAs for example?

[chuckdanny]

Maybe it has already been said, i don't remember all answers but maybe it has to do with growth rate of neighbouring cells, are you able to control it especially in high gradient zones? you should, i recognize the soft.

Or it is just by nature of the phenomena, turbulent area may produce variations that a steady state can not show, well depending on when you stop iteration your values of interest will change, there is an averaging process that mask discrepancies. Turbulence and steady state makes no sense, von karman spanwise vortex shredding for example, fluid structure interaction, what does it mean to obtain a steady result with a turbulent flow?

Have a look there :
http://www.symscape.com/steady-state-or ... simulation

[chuckdanny]

Another interesting article on the subject you might be interested in
It took me a while to find where i read this one...

"We know embarrassingly little about how the mesh affects the CFD solution"
http://blog.pointwise.com/2012/07/05/ac ... h-quality/

[dans79]

I've seen this issue before, in college I worked for a team that modeled the earths magnetosphere for NASA. Our model was was highly chaotic as could be shown by calculating the Lyapunov exponent.

The model was 6 linked partial differential equations that where a function of time. We originally solved the problem by making the step size really small, but that let to long run times (days or even weeks), as well as issues with machine precision limit.

We finally got it to work reliably using http://en.wikipedia.org/wiki/Richardson_extrapolation on every time step. Depending on how much control you have over the simulation, you might want to look into it.