CFD - PERRINN F1 Car (w/ spec mods)

[Dipesh1995]

Otherwise, sounds good, I think it will yield some really interesting results.

Thanks heaps for the tip mate, really cool to add this to my tool belt of things I can do

No worries mate, glad I could be of help.

[Just_a_fan]

Took me a couple hours to figure out the correct reference frames and BCs to use in the ANSYS environment, but hey - I made a rainbow

Oooh! Pretty!

[Vyssion]

No worries mate, glad I could be of help.

Mayyyyyyyyyyy need just a quick sanity check from you if that's alright mate...?

So, following on from the "success" of the empty domain which has a curved velocity field now, I went home at set up my F1 car model with it:




Set it all up to go and executed it etc, and was greeted by this:






Which looks somewhat sensible... however, the Coefficients of [Total] Pressure's etc, were completely off the charts... For example, there seems to be a somewhat "higher" pressure throughout the domain which I cant work out is the dynamic pressure of the rotating reference frame being interpreted as just an arbitrary static pressure increase by the stationary frame, or whether there's some sort of mistake in the definitions of my equations... So I did some research on Keogh's paper and found these two little gems:






Now, I took these, and basically reassured myself that the "setup" was correct (I double and triple checked it), and so I'm sort of left wondering how to interpret the field data when it comes to defining my own custom variable equations... For example, CFX doesn't calculate Pressure Coefficient by default - you have to create an expression, convert to a variable, then plot it. Here are my current equations as ANSYS requires you to define them just for completeness:




It was interesting to define the velocity field algebraically via the "omega * r" definition he has, then to define the Pressure Coefficient based on this new "Curved Velocity" as I called it arbitrarily. However, when I created this new CP variable and plotted it, I thought I might just swap out the Pressure field for Total Pressure field... There is a "Total Pressure in Stationary Frame" which exists as well that kind of "removes" the radial component of the rotating reference frame from the Total Pressure, but I just left it as this for now. And what I got out of it, did look remarkably similar to what I was getting before the curved flow adaption was made:






However... the upper and lower bounds extend from like -0.0005 to +0.00009 or something insane... and then I look at the units of degrees^2..................... Which makes me wonder if it is somehow generating a dimensionless parameter in terms of area on a sphere...??? (i.e. in terms of "steradians" of a full sphere -- equal to 41,253 degrees^2)...

I feel like this is soooooo close to being correct etc, but I am missing something in terms of units or variable etc... Any thoughts on it??

[Dipesh1995]

No worries mate, glad I could be of help.

Mayyyyyyyyyyy need just a quick sanity check from you if that's alright mate...?

So, following on from the "success" of the empty domain which has a curved velocity field now, I went home at set up my F1 car model with it:

https://imgur.com/y9FSLCg.png


Set it all up to go and executed it etc, and was greeted by this:

https://imgur.com/WlS3dpI.png

https://imgur.com/rOJHUzT.png


Which looks somewhat sensible... however, the Coefficients of [Total] Pressure's etc, were completely off the charts... For example, there seems to be a somewhat "higher" pressure throughout the domain which I cant work out is the dynamic pressure of the rotating reference frame being interpreted as just an arbitrary static pressure increase by the stationary frame, or whether there's some sort of mistake in the definitions of my equations... So I did some research on Keogh's paper and found these two little gems:

https://imgur.com/PPNMSQu.png

https://imgur.com/yw3uA0W.png


Now, I took these, and basically reassured myself that the "setup" was correct (I double and triple checked it), and so I'm sort of left wondering how to interpret the field data when it comes to defining my own custom variable equations... For example, CFX doesn't calculate Pressure Coefficient by default - you have to create an expression, convert to a variable, then plot it. Here are my current equations as ANSYS requires you to define them just for completeness:

https://imgur.com/T8Vt9a2.png


It was interesting to define the velocity field algebraically via the "omega * r" definition he has, then to define the Pressure Coefficient based on this new "Curved Velocity" as I called it arbitrarily. However, when I created this new CP variable and plotted it, I thought I might just swap out the Pressure field for Total Pressure field... There is a "Total Pressure in Stationary Frame" which exists as well that kind of "removes" the radial component of the rotating reference frame from the Total Pressure, but I just left it as this for now. And what I got out of it, did look remarkably similar to what I was getting before the curved flow adaption was made:

https://imgur.com/IboI7ys.png

https://imgur.com/YB3hO9V.gif


However... the upper and lower bounds extend from like -0.0005 to +0.00009 or something insane... and then I look at the units of degrees^2..................... Which makes me wonder if it is somehow generating a dimensionless parameter in terms of area on a sphere...??? (i.e. in terms of "steradians" of a full sphere -- equal to 41,253 degrees^2)...

I feel like this is soooooo close to being correct etc, but I am missing something in terms of units or variable etc... Any thoughts on it??

Sorry for the late reply, I was on holiday

I don’t know how much help I can be with this as I’ve not ever experienced such an issue.

The first thing that came into mind was that presumably, the “curved velocity” defined by omega etc is giving you the correct velocity field distribution throughout the domain?

Your equations look correct but for the curved coefficient of pressure, should the numerator not be p-p_inf?

[paddyf1]

Alright...

So, over the past week or so, jjn and I have been CADing up some 2019 spec wings for the PERRINN model in the future. jjn has created a "somewhat parametric" aerofoil profile distribution which allows us some control over the geometry, and hopefully we can take these models, and after I prepare them for meshing, get some of our own "design attempts" out there too (or rather, more likely, we will CAD up something similar to existing teams wings and see if we can make any assumptions on performance... but shh!!)

For now though, we have somewhat "modified" the 2018 wings of the Perrinn to fit the 2019 spec and CFD'd them for you. I will say that I wanted this to be the start of what will eventually become a "replacement" of all components of the Perrinn F1 model. The export of the baseline Perrinn CAD to .step was "dubious" and has taken me around about 20+ hours total of surface repairing and preparation for meshing, to the point now where part of the issues I am having with the meshing is that generating a patch conforming tetrahedral mesh is doable... just!! The inner "perfectionist" in how I prepare my own CAD for CFD is getting more and more frustrated with the lack of attention to creating good quality surfaces, most likely because the people running simulations just stick a mesh wrap over it and accept whatever it spits out. Not me...

Anyways, so... This time, I have prepared the CAD to a much higher standard (FW and RW only of course) and have replaced the originals. The result is a much higher quality mesh for the FW and RW, as well as, with many... MANY... meshing attempts... a slightly better overall quality mesh. I have now put our new geometry through a 4° Yaw case (similar to before) and finished post-processing as well.

The results are now in, and both jjn and I are studying the images and forces/torques outputs etc and will be back sometime soon with another update etc, but for now, here are some images of the new wings.

https://imgur.com/JKa0gUo.png
https://imgur.com/cwRwybU.png
https://imgur.com/phaJnEe.png
https://imgur.com/3bAbC50.png
https://imgur.com/3jmKvTd.png

How about doing what you have done here but with a 2007 spec front wing? See how they wings helped or hindered the airflow.

[Vyssion]

How about doing what you have done here but with a 2007 spec front wing? See how they wings helped or hindered the airflow.

Hmm... That's kinda a bit tricky to do I think for not that much reward...

Whilst I would absolutely LOVE to have a 2008ish era CAD model to do these sorts of studies with, alas, I do not have them and I wouldn't currently have enough time to do that right now However, there is quite a bit of literature out there which analyze the 2008 vs. 2009 change over which saw similarly large aerodynamic regulatory changes come about. Nakagawa wrote a paper in 2016 looking at the vortical flow structures involving the FW, Wheel, and Bargeboard area etc which is very good, as well as Perry and Marshal in 2008, and Torbjorn Larsson in 2009.

I took down some notes in my CFD bible of Nakagawa's paper, which amongst my fellow writers and mods, is "high praise"

They can be found online quite easily with a google search or I can send them to you if you want to PM me.

In summary, the changes in regulations were:

• Narrower and taller rear wings were placed higher up

• Wider and lower front wing with unloaded centre section

• Underbbody diffuser starts further back

• Far fewer add-on air control devices (winglets, bargeboards, etc.)

And some noticeable observations were:

• Rear wing becomes more of a stand alone device and flow interactions with the underbody and diffuser are much reduced

• Revised diffuser design has a dramatic effect on underbody flow where most of the overall downforce is being generated

• Exclusion of auxiliary wings has a large direct and indirect impact on downforce

• Front wing flow and its interaction with the rest of the car is remarkably different

The prime and immediate effect of the rule changes that were seen was thought to be around about a 50% reduction in overall downforce. Also, due to the major overhaul of the concept of how the front wing works was done, the front tyre wake flow was radically different which then, of course, affected the downstream components in quite a different way. The ban on all the extra winglets, bargeboards and other devices, meant that controlling the wake flow was much more difficult than before. Some initial transient CFD was done and found there to be more flow fluctuations and instabilities present as well.

@jjn9128 pointed out to me that although a 50% reduction in downforce was aimed at, in reality because of the double decked diffuser (DDD), it was only around the 10-20% range, and most of the downforce which was "lost" with these changes were recuperated pretty much entirely by 2010. Nakagawa mentions that in his paper if we both recall correctly.

[boerface16]

Very cool topic, thanks for sharing! I am interested to see what you guys will do in the future. I would love to know how you got the model? I am interested in playing around with this

Personal question that you don't have to answer, whats your background?

The Perrin model is an opensource project available from onshape, which is an online CAD program. The car can be found here. Not sure if it will force you to create a profile to view it or not. Onshape is made by some guys who left solidworks, if you've used that it'll be familiar but I think it's not quite as good, e.g. I wouldn't even bother trying surfacing.

Awesome, thanks for the reply I will check it out and start playing around with the model.
Also, I just took a look at the rest of the thread... great work guys! Very insightful, interested to see what else you guys come up with in the future.

I am having a think about the curved domain Cp0 problem, the degrees^-2 is really tripping me up... there has to be an error in units of something right? Did you double check to see that everything else gave you the units you were expecting? You probably have but just in case...

[Vyssion]

Awesome, thanks for the reply I will check it out and start playing around with the model.
Also, I just took a look at the rest of the thread... great work guys! Very insightful, interested to see what else you guys come up with in the future.

I am having a think about the curved domain Cp0 problem, the degrees^-2 is really tripping me up... there has to be an error in units of something right? Did you double check to see that everything else gave you the units you were expecting? You probably have but just in case...

Thanks mate. Unfortunately, I don't think I'm gonna have time to devote to this for a little while yet, but I do miss it; and I also really want to hurry up and get my new computer so I can run these much smoother given I wont be maxing out my current machine.

Re: curved flow problem, yeah it is something to do with units. I haven't loaded it back up since then, however, the CFD-Post expression editor will take whatever units that you explicitly state in the equation definition, and then so the unit conversions on its own automatically for you. 95% of the time, this results in the perfect conversions etc, however sometimes it will throw a curveball at you such as defining a torque in "Joules"... which when you think about it, isn't technically "wrong"

As for the °^2 unit, that unit is actually something called "steradians" which is a weird unit that Astronomers sometimes use to denote the area of the "sphere of the night sky" that a particular object either takes up or can be found within: i.e. a sphere = 41,253 steradians. Given that my velocity field that define, prior to then using that value within the definition for the Cp and CpT equations, is done algebraically rather than actually taking the nodal values of it within the mesh (basic pythagoras based on a circle centre point and a postion within the mesh), I am leaning towards that expression somehow carrying through an angular variable due to the fact that the entire domain is said to be rotating at 0.5rac/sec (which gives me ~50m/s @ the car's CoG location)...

I do need to dig this up and work on it again soon: I really enjoyed sharing it all with you each week or two with the newest addition to the whole model Soon..... soon.....

[peaty]

Hi all,

As mentioned earlier, here is our new article going through some of the findings that jjn and I have seen with the 2018 vs. our 2018-modification to 2019 spec wings on the Perrinn baseline model.

Please give it a read, and let us know what you think!!

(p.s. 2019 Vyssion-jjn wings have been CFD'd at 0° gust; just waiting on 4° gust now before we release those pictures and gifs to you all ... stay tuned!!)

https://www.f1technical.net/features/21995

https://f1tcdn.net/images/features/2019 ... 19-big.png

I just found your work and it's amazing!! are you working with Fluent or CFX!? I would love to learn to run simulations. Could you please recommend me a good tutorial that covers the entire process -from surface preparations to post-processing-!? I've been trying to find a good one without luck so far!

Cheers!!

[Vyssion]

I just found your work and it's amazing!! are you working with Fluent or CFX!? I would love to learn to run simulations. Could you please recommend me a good tutorial that covers the entire process -from surface preparations to post-processing-!? I've been trying to find a good one without luck so far!

Cheers!!

I don't really know of a "one size fits all" guide to be honest, as there is quite a lot of, kinda, "expert guesswork" in just knowing how the mesher and solver are likely to deal with the flow or mesh as you create it... Some of my advice would be to:

• Think about what you are trying to simulate; i.e. if you are looking at larger scale flow structures, then you probably don't need to resolve that teeny tiny gap between two bits of the car do you? So you can fill it as a solid, or just widen the gap to stop the mesh resolving down that fine. It's important to realize that you are in 3D which means that half a cell edge length is not half a cell volume...

• Once you have simplified down as much as possible, look at what the individual surfaces look like. Are there really long and thin surfaces? Are there surfaces that go into a spike (like at the ends of fillets)? Are there any surfaces which look like you would kind of struggle to manually divide up into even and simple shapes? If the answer to this is yes, then you need to either find a new way of creating the feature you want, or you need to cut away parts of the surfaces and manually loft a filler

• Always build in solids. Now this is a personal preference of mine, simply because it is more robust, however, I do build in surfaces, but ensure that it is watertight and convert to solid prior to meshing. Once it is a complete solid body, you can subtract it from your computational domain and it should be much simpler than intersecting surfaces and wrapping etc, at least in my opinion

• Don't go for the most complex thing first. I know it is tempting to grab a model online or to try and do it all in one go, but simply put, you just won't. Get something running, simple, easy, test your process, and gradually add complexity. If it is simple, then it will only take 30-60mins at first to test the first simulations anyways, so you aren't missing out on anything at all

• Read the error messages!! The amount of questions I get on this forum from people who send me their error messages asking "how do I fix this?" is astonishing: the answer is literally right there 99% of the time, and by reading it, googling it, checking your settings and then testing out a few fixes, you not only learn yourself what not to do, but you will remember it next time so that whenever you see that error, you can navigate your way past it with ease.

• With meshing, I personally prefer edge controls in areas of high importance, and trying to map my surfaces to a grid. i.e a straight rectangular wing's leading edge. I would split the leading edge along it, and I would also split the top and bottom surfaces about 10-15% of the way down the chord so I am left with two curved surfaces. I would then place a control on the edges forcing say 8-10 cells along that line, and bias their sizes so the smaller sizes were on the leading edge, and they grew out to the 15%c line by ~3-5x or something. I would then place a set number of divisions along the 15%c line and the LE line, to ensure that the cell height from the curved edge bias vs. the cell width from the LE bias didnt cause those first few cells to be at too high an aspect ratio, and then I would map the surface using just a normal mapping operation. This way, all the cell divisions on the curved edges would be connected up horizontally, and all the LE and 15%c divisions would be connected up so you would be left with a 2D grid mapped to the surface, which had smaller cells on the leading edge where you need them, and larger ones at the 15%c line, so you could then grow the surface mesh unstructurally towards the trailing edge (which has a finite thickness!!) in the same manner as just done for the LE

• For solving, stick to incompressible, ideal gas laws with an upwind differencing scheme at first, before moving to 2nd order and higher schemes where you can. Again, you want stability for your first run; not accuracy. As for the turbulence model, personally, K-omega SST I prefer just because I find it to be a more superior model, however, you only ever get the best out of it if you are resolving the boundary layer to a y+ of 0.1 < y+ < 0.5, otherwise you will be using wall functions to start: which again, is the way to go. Ensure you have a boundary layer, perhaps 8-10 cells to start, and run it with your wall functions to get something running. Prism layer cells are where the real cell count numbers are driven up, as each surface element has, on some of my sims, 30-40 cells above it that are down to the 1 micron in height at times. And when your surface mesh is in the millions, things can get quite computationally expensive...

• With post processing, again, think about what you want. If you are looking for flow separation, then create a contour or surface wallShearStressX (nose to tail) and set your limits to 0Pa - 5Pa... anywhere you see blue (i.e. <0Pa) there is most likely separation going on. Think about what you are looking for, and then plot accordingly.

Hope some of this helps, and I am always here to answer questions as anyone needs them.

[Jonas]

Hey,

can you please send me the CAD Files of the PERRINN F1 Car, so i could do some simulations with about 80 mio to 120 mio cells and a Y+ lower 5 in star-ccm+. Tires will be modeled with MRF and if you want, i can also do cornering simulations in a MRF region.
I can use free licenses and a high performance Cluster with more than 17k processors

Feel free to contact my by private message...

Best regards and really looking forward to simulate the car,
Jonas

[jjn9128]

Hey,

can you please send me the CAD Files of the PERRINN F1 Car, so i could do some simulations with about 80 mio to 120 mio cells and a Y+ lower 5 in star-ccm+. Tires will be modeled with MRF and if you want, i can also do cornering simulations in a MRF region.
I can use free licenses and a high performance Cluster with more than 17k processors

Feel free to contact my by private message...

Best regards and really looking forward to simulate the car,
Jonas

You can find the Perrinn car via the usual channels (https://www.onshape.com/cad-blog/this-2 ... ublic-plan). Anything we added for the purpose of this thread and our front page articles is ours. Sorry.

[turbof1]

That is a question that is passing the venue quite often: people wanting the modified perrin CAD model.

Understand that our writers put in a LOT of hours into the modified models, and we are genuine grateful for that. It would not be fitting for them to just hand the model over; there is an actual learning process involved and anyone who just got the model handed would miss out on said learning process.

Of course, our writers stand at the ready for anyone who is stuck at something or wants advice.

[maunde]

Thank you all for such an amazing contribution. This article is very enlightening (especially in regards to the curved flow). Vyssion or jin mentioned early on some scripting for post processing. I am interested in creating scripts for the same purpose, how do you go about doing this? What is the workflow for creating a script with ANSYS?

[Jonas]

I got the Perrin F1 car and did some simulations with my self developed front wing. You can find all data of my simulations here:
https://grabcad.com/library/f1-car-cfd-simulation-1

If you have any questions, feel free to contact me.
I did the simulation with STAR-CCM+ on a high performance computing cluster.
Here are some details about the simulation:
- half car
- 83 mio cells
- Y+ below 2
- 13 boundary layers
- k-epsilon
- steady state
- 2500 iterations
- segregated flow
- constant density
- at 180 kph
- wheels modeled with tangential velocity on the tires and MRF for the rims
- moving ground
- 0.5 degree rake angle