Cross-comparing CFD results?
 

I know there is already one thread dedicated for CFD simulations, but I don't think that is exactly the correct place to put this as that seems to be a bit more oriented towards discussion about the CFD programs and modelling etc.

I am revisiting my own simulations and 3D models of a 99 NB Miata with a hard-top, and I would like to cross compare with other people if my results of the stock version of the car are making sense. Keep in mind that this is my own personal stuff that I am just doing for fun.

The results I got from simulating a stock car at stock height:

Speed 44.7m/s (100mph)
Total drag 790N
Cd: 0.39
Total downforce: -494N (major contributors are nose of the car, area before windscreen and the immediate area behind the roof)
Center of downforce: 1.2m from the nose towards the rear (car lenght 3.95m)

I think that since I have not set-up a "radiator intake" I am seeing an increased pressure on the lip of the front bumper as the air can normally escape through the radiator. Also the high low pressure area around the windscreen is something I don't fully understand. Can anyone confirm or disagree with the results I have?

https://cimg1.ibsrv.net/gimg/www.mia...aa3c148a4a.png

https://cimg7.ibsrv.net/gimg/www.mia...628570acbe.png

Edit. added a underview

Both your assumptions of the radiator, but also the pressure contours in the windscreen area seem logical to me. How was your model set up? I can try and model/run this here as well to cross-compare numbers (cannot promise when as work is killing me ATM) but I will need the geometry file to do so.

Like title suggest I would rather compare results with other people who might have simulated an stock 99 NB on their own to see if we are in the same ballpark. I feel like especially the downforce center would tell a lot if I am near the real thing. I have tried for example 3d scanning my own car to get the geometry to match better by manually cross-comparing the models.

I don't know how to say this more politely, but me sending my own model for someone else to simulate kinda defeats the purpose, so I no I will not send you my model for free like you already asked twice.. How do I anyways know that you will not put it for sale on some 3D-model website immediately afterwards?

It's already a bit far fetch for even me to ask to cross-compare results as people are usually not doing any of this for free, and are really holding on to their results with teeth and nails.

What is your end goal.

I would like to build an adjustable rear-lip for my car and I would like to know what dimensions and angles would result in a balanced aero situation with a relatively low increase in drag. I don’t want to buy a lip that has been made by someone else, I want to experiment on my own instead.

To do that it would be kinda relevant to understand if the model I have made is somewhere in the correct area or not. I am not looking to get some perfect results, but knowing if my simulation is completely somewhere in the wild or not is still important.

Fair enough; was not trying to rip you off or anything, just trying to help as I like fooling around with FEA in general. I do not think you will have much luck, not because people do not wanna help, but mainly because there are NO decent quality geometry files already available out there for the NB. I tried to 3D scan my own NB2 (including underneath), but the paint was too reflective for the scanner I was attempting to use, and I could not be bothered more at that particular time, so this was abandoned.

BTW; there has been a CDF study of a NA kicking around. I know that the nose is totally different, but the hood is pretty close and the windshield is identical. This can give you a qualitative idea if your results are in the ballpack (I think they are)

Covering the car with thin blankets that have a pattern (and pulling them tight with some tape etc) helps immersely if you are trying to do a image based 3D scan. IKEA is a pretty good source with their 2 euro blankets :p This is what I learned. Another cheap trick with image based scans is to spray a mist of water on a well waxed car and get the software to pick up the small droplets from the surface instead. The reflections will still fuck up the simulation somewhat, but its a lot better than just bare paint. One more trick I can think of is covering the car with something like a thin foam etc. that you can wash away easily after scanning.

I have tried to compare to the simulations made by someone, but having more to work with would be better. I bet you are referring to these pictures on the bottom of this web-page https://robrobinette.com/S2000Aerodynamics.htm

Then again I have also seen these numbers from another source here which kinda match the results of that link, but the Cd is very different. Vastus means Drag and Noste means lift.
https://cimg4.ibsrv.net/gimg/www.mia...b4ea8dee32.png

Now when comparing to my simulation, both of these are not matching with my NB simulation as my simulation is showing that the stock car would actually have some decent downforce instead of lift as stock. I find that kinda hard to digest.

I have contemplated covering the complete car in painters' tape; just did not had the patience/time to do so! :D Your suggestions are great, might give these ideas a go.

These are indeed the pictures I was referring to; qualitatively, the distribution seems reasonable. You are right about the numbers though, I would be surprised if the actual car generates any downforce. Your assumption of the bumper opening contributing to unrealistic df numbers sounds reasonable though; and I also spot some low pressure zones under the car which are most probably due to the smooth/flat surface and can also contribute to the end result.

I need to meet this Rob Robinette. His pages on guitar amplifier design are some of the best on the internet, I’ve used them for reference in my own builds/repairs about a hundred times. Anyone who nerds out on race cars and guitars is OK with me.

Sorry OP, carry on. I can’t help your aero project at all.

Thanks for the valuable input :D

It is very hard to compare results to others unless you both have similar mesh resolution and similar boundary conditions/physics. I have compared Fluent --> OpenFOAM --> wind tunnel results with very good correlation between all. Assuming you are using OpenFOAM based on the paraview post work, what was your mesh cell count? What was your layering and how was the coverage? What y+ did you target and/or achieve? Was this done with symmetry? Tires have rotational boundary condition? What turbulence model are you using?

The reason I ask is that your numbers look on the high end based on me just looking at the car (could be wrong as aero eyes do not exist). I most likely would guess that is a meshing issue more so than anything. The post pictures don't look abnormal assuming we are looking at pressure. Add some pictures in Cp from -1 to 1 and that could help more to see if anything is out of whack. I can help more with some of that.

Hi..from Greece..
Im a 3d Designer, i have an Nb mk2,5 and have design it as close as possible in 3ds max and Fusion 360. If someone wants it please tell me what file do you want it and i will see if i can provide it... To be used in cad/cfd.
some 3d samples
https://imgur.com/a/RTp3Cdh

That looks amazing! :party:

Would you be able to attach (both?) files on the forum, or are they too big.

Both files are the same.... what im asking is what type of file... i can export to most file types from cad.

Standard exchange format for CAD-neutral files is STEP and IGES. You could host your files to Grabcad and then link here if they are too big to upload. How did you get about modelling? Pictures scaled to basic dimensions? I plan to 3D scan my car at some point so it would be nice to compare as well.

Yes started with blueprints/images and then fine tuned it with real measurements from my car. Perfect i will export step file and upload it to Grabcad...

Im not sure if they are correct...files

https://grabcad.com/library/934276

Before anything, like I said I am doing this for fun and to learn, I am using a pre-made script (by Julien De Charentenay) to get easy and quick results, as I am not a fluid dynamics expert, I am a CAD and 3D modeller. I don't think I would be able to use OpenFOAM to this level that is required for this simulation, Fluent maybe. To answer some of your questions:

OpenFOAM with paraview. The simulation is done with a symmetry, no rotational boundary conditions, turbulence model is incompressible RAS k-Omega-SST.

Simulation is done in two parts, first 500 iterations with a low mesh resolution (266519 cells), mapping the results to a high resultion mesh (98513832 cells) and then running until the simulation for 1300 iterations.

I don't know what y+ exactly stands for, but I was able to extract this: y+ : min: 0.00408475 max: 397.64 average: 34.405


To continue further, I made more detailed geometry under the car and refined the shape of the roof slightly, and I was able to make the car perform a lot worse (44.7 m/s):

• Length (y axis direction): 3.95 m (Y from 1.01 to 4.96 m)
• Width (x axis direction): 1.82 m (X from -0.87 to 0.94 m)
• Height (z axis direction): 1.22 m (Z from -0.01 to 1.21 m)
• Frontal area - A: 1.71 m2. This is the projected area of the vehicle in the y axis direction.

• Total drag: 967.91 N
• Drag coefficient - Cd: 0.47
• Drag area - Cd.A: 0.81 m2
• Total Lift: 238.54 N
• Lift coefficient - Cl: 0.12
• Lift area - Cl.A: 0.20 m2
• CoP of lift: 7.831 m along streamwise (Y) direction from Y = 0.00 m.

https://cimg1.ibsrv.net/gimg/www.mia...1de99733b6.jpg
https://cimg5.ibsrv.net/gimg/www.mia...166ef4bdb9.jpg
https://cimg7.ibsrv.net/gimg/www.mia...7c26d36cb5.gif
https://cimg8.ibsrv.net/gimg/www.mia...aea67b9166.gif
https://cimg0.ibsrv.net/gimg/www.mia...f2a32b73f9.gif

Is the high-resolution mesh really 98 million? That seems astronomical for the simple geometry using symmetry. I have never seen the pre-made script from Julien, do you have a link as I would be more curious of the setup. I use CFD in both OpenFOAM and Fluent.

Y+ is basically a way to tell in you near wall mesh will capture the boundary layer properly. The y+ target values will depend on wall functions and turbulence models.

The drag value seems a little high. I am assuming the solver is simpleFoam and if so, more iterations are usually needed to converge the force values.

Hi! Thanks a lot for explaining the y+. Here is a link for the most useful document for this script I am using :) It is meant to be used for a competition on race car aerodynamics design, but also contains features for normal car and even sailboat simulations.

https://www.slideshare.net/mobile/Ju...fd-users-guide

Drag was a lot lower when I had flat floor if you look at the upper posts.