[matthieu57000]

Hello everybody,

My name is Matthieu and this year I m part of the Metz Racing Team (french fs team) in the aero division. Last year, we developped our first full aero kit using a K Epsilon model but it wasn't accurate so this year we decide to use K Omega SST model.

General problem: our simulation doesn't converge enough, residuals are too high and even force coefficient aren't enough stabilized.

So when we run our simulation, we always launch it by using 1st order upwind scheme during +/- 150 iterations because it s more stable (in order to get an initial solution) and after that we switch in 2nd order to get a results more accurate.
So each time we launch the simulation, all residuals drops correctly until a certain value where TKE residuals rise up and after it doesn't decrease again.
You will find a picture of it just below.

https://zupimages.net/viewer.php?id=20/08/vl8y.png
https://zupimages.net/viewer.php?id=20/08/y60y.png

So we checked the mesh quality (volume change, face validy/quality and skewness) and all is good. Wall Y+ is around 1 on the whole car and goes up to 3 locally (see picture).

https://www.zupimages.net/viewer.php?id=20/08/dsb0.png

After we take a look to the results and we find that just behind the air filter we get some turbulence which seems weird as we have kind of "black holes" where velocity is zero. So we though the problem came from here and was because mesh cell's weren't enough small to catch the vortex etc ... Considering that we refined it, it improves a bit the results but we keep having the same problems.

https://zupimages.net/viewer.php?id=20/08/7xob.png

We ve seen another thing which maybe can prevent which is the total heigh ot the prism layers on the trailing edge of our wings due to the curvature of it and the small cells neighbours). Can it be a source of problem ?

https://zupimages.net/viewer.php?id=20/08/kwwy.png

Each time we change mesh settings, we launch the simulation using previous simulation results, is it a good thing or can it blocks the simulation ?

Settings (simulation executed on a half model)
+/- 65M of cells
10 prism layers on the car and 12 on the wings
Steady
K Omega SST

If someone had any idea or suggestion it will help us a lot
Thanks for your attention
Matthieu

[arjun]

which software are you using?

[plucas]

1. Wasn't accurate according to what?

2. What software are you using?

3. You have no pictures attached.

4. 65 million cells seems a little large for half-model on FSAE car.

5. K-omega SST is usually a better turbulence model to use. Bad convergence could be from a few things. It almost sounds like you are trying to run before you walk. I am personally not a fan of using half-car models as the flow is usually not symmetrical. I would make sure your model is simplified, target a y+ of 30-300 and use standard wall functions. This should speed up each run and simplify your setup and start from there. That will be an easy point to nail down convergence. Then work on making your model more advanced.

[matthieu57000]

Thanks for answering.

Refering to the pictures, I ve updated it, so you should see it.

We re using Star CCM+.

When I said accurate it was because the results we get were wrong. For instance, the diffuser outlet had an angle overpassing 30/35° and when we see the results, it shows that all the flow stayed attached to it whereas it should separate. I ve seen values for diffuser's angle and it s around 14°.
Besides, last year when we went on competion, we were reviewing on the model we chose (K Epsilon) because it doesn't predict very well the detachment near wall so this is the reason why we changed.

Concerning the number of cells, we increased it because in some regions some vortex seemed to be collapsed into a point. So we thought we needed to increase the mesh refinement. We also asked to teams how many cells they had approximately for their model in order to have an idea.

After that, refering to the half model, can it be the reason for non convergence and can results between a half car and a full car model be very different?

[plucas]

I am unsure on the diffuser angle aspect. I do know I have had better results with k-omega sst compared to k-e with track testing and in wind tunnel. Diffuser angle doesn't really matter as it is really more about expansion rates and ride heights.

Your geometry is rather simple and I cannot believe you are in that cell range for a half-car model and the lower speeds that FSAE car should be tested at. Start simple and work your way up which might solve your convergence issue there. I do not know your computing resources so it might not be an issue. I only run that cell count on much more complex geometry, full car, and probably higher speeds.

I do not think a full car will solve your convergence issue. However, I think you would get better results. I think you would also get better results running it always at slight yaw as the perfect straight flow is never seen on track.

I would lean towards the mesh is the issue for convergence as that is always where my convergence issues were. If you are pretty sure it isn't the mesh, I would look at your boundary conditions and overall setup. I am not 100% sure on Star-CCM+ setup as we use OpenFOAM. My thoughts are just my 2cents though and take it with a grain of salt.

[matthieu57000]

In the beginning we were using around 30-40M cells but we thought that our convergence problems came from the fact we didn't have enough cells to well represent the flow.
We also think that our problem comes from our mesh but we don't know where exactly. Refering to skewness, face quality/validity and volume change all is correct, we don't know what other settings can help us to diagnose the quality of our mesh.
I heard about aspect ratio, but I didn't find values to analyze with Star CCM since it's calculated differently than in other sofware like ANSYS.
Could you give us an approximate cell range just to have an idea for an FSAE half car (speed is around 45kph).
Thank you

[arjun]

Originally Posted by matthieu57000

In the beginning we were using around 30-40M cells but we thought that our convergence problems came from the fact we didn't have enough cells to well represent the flow.
We also think that our problem comes from our mesh but we don't know where exactly. Refering to skewness, face quality/validity and volume change all is correct, we don't know what other settings can help us to diagnose the quality of our mesh.
I heard about aspect ratio, but I didn't find values to analyze with Star CCM since it's calculated differently than in other sofware like ANSYS.
Could you give us an approximate cell range just to have an idea for an FSAE half car (speed is around 45kph).
Thank you

Are you using trimmer mesh if yes then the problems come from prism layer and the transition from prism to interior.



Check the hybrid gradient algorithm that ccm uses, in this pay attention the parameter that would decide green gauss and lsqr method. Set it such a way that all the prisms are using green gauss.

[Penny67]

Something that may help:
Ansys has added a new CFD tutorial for Formula teams that walk-through CAD simplification and cleanup on real FSAE geometry (from the University of Pittsburg FSAE team), proper mesh settings and quality metrics, boundary conditions, run, and post processing:
https://courses.ansys.com/index.php/...an-fsae-car-2/

If you want a full license, fill out the partnership form here:
https://www.ansys.com/academic/students/student-teams

[CFDfan]

Originally Posted by matthieu57000

Thanks for answering.

Refering to the pictures, I ve updated it, so you should see it.

We re using Star CCM+.

When I said accurate it was because the results we get were wrong. For instance, the diffuser outlet had an angle overpassing 30/35° and when we see the results, it shows that all the flow stayed attached to it whereas it should separate. I ve seen values for diffuser's angle and it s around 14°.
Besides, last year when we went on competion, we were reviewing on the model we chose (K Epsilon) because it doesn't predict very well the detachment near wall so this is the reason why we changed.

Concerning the number of cells, we increased it because in some regions some vortex seemed to be collapsed into a point. So we thought we needed to increase the mesh refinement. We also asked to teams how many cells they had approximately for their model in order to have an idea.

After that, refering to the half model, can it be the reason for non convergence and can results between a half car and a full car model be very different?

This is an old thread I came across by chance and was very surprised to see that the Academics who are usually very active when the CFD model is trivial, or from the textbooks, kept quiet about this one from the real life. Meanwhile, this is exactly the case where their contribution would have been greatly appreciated

[arjun]

It seems from version 18.02 Starccm has taken out these options and the gradient algorithm is now replaced with new algorithm.

With new algo if you see divergence etc then just know that you are not alone. I have heard from few people about divergence from newer version of starccm.

Originally Posted by arjun

Are you using trimmer mesh if yes then the problems come from prism layer and the transition from prism to interior.



Check the hybrid gradient algorithm that ccm uses, in this pay attention the parameter that would decide green gauss and lsqr method. Set it such a way that all the prisms are using green gauss.

[MariyJacksions]

Assuming you've done some kind of intro to fluid mechanics, if you haven't... stay well away from CFD until you have

Look up books on the Finite Volume Method.Derive the Navier stokes equations. Learn how they are discretized. Learn what RANS and turbulence modelling are. Go from there and read up on mesh convergence studies, and how to mesh aerofoils.