[AndreP]

Hello,

I'm performing a external flow simulation of a simplified version of a Formula One Car, although I'm facing some problems... I've been the last 2 weeks around this, and between some cluster problems and CAD problems, I'm now clueless what I'm doing wrong... But sometimes, after so many days looking at this, I just lose the ability to see the small details! Everything seems fine to me! So here I explain and give further details!

Lenght Of the Car: 5m
Flow Domain: 55m x 22m x 10m

Inlet -> Flow Domain, Velocity Inlet @ 55ms (Boundary Normal)
Outlets -> Flow Domain, Flow Split Outlet
-> Air Intake of the Car, Pressure Outlet @ 0.8781 bar
Walls and Floor -> Defined as Walls with Slip (for now I'm still not modelating the BL on the floor)

Mesh Models: Surface Wrapper, Surface Remesher, Trimmer Mesh & Prism Layer (10mm base)
Physics Models: Realizable K-Epsilon, Steady, Constant Density, Segregated Flow.

26.8 M cells

Volumetric Controls:
Around Air Intake - 7.5 mm
Behing Front Wheels - 15 mm
Around Cockpit - 12.5 mm
Car Wake (Up to 2.5m distance) - 10 mm
Car Wake (Up to 5m distance) - 15 mm
Car Wake (Up to 7.5 distance) - 20 mm
Around the Whole Car - 20 mm

After doing the volume mesh, the following Mesh Quality indicators were plotted (Accordingly with the Help File on "Mesh Quality"):
Cell Quality - All cells above 1e-5
Cell Warpage - All cells above 0.15
Chevron Cells - All cells are 0
Face Validity - All cells above 1
Least Square Quality - All cells above 1e-3
Skewness Angle - 99% of cells bellow 85, there are some between 85 and 163 but I can't see them on regions
Volume Change - All above 0.01

Wall Y+: Majority of the car between 0-30, around air intake goes around 175 (Currently fixing that in the simulations now meshing/running)

But even with a reasonably quality mesh, I'm still facing strange results (Negative Drag Forces, and stupid residuals!). The residuals have the normalization turned off. Here are the following print screen that might help you! I know there's only 360 iterations which is not a lot, but this ran for 24h, and I think it's enough to see that the simulation is not going anywhere good!

Also, I'm having very strange results on EXTREME speed (around 400 ms at the intake) and extreme pressure coefficient, so I'm guessing it might be something on the physics and setup of the simulation!

Could anyone point me what I could potentially look at to make the simulation retrieve good results?

I can provide extra info, just ask me!!!

Residuals: https://imgur.com/Z4HvXpg
Negative Drag / Positive Downforce: https://imgur.com/xNyGVPS
Mesh 1: https://imgur.com/ynakVUK
Mesh 2: https://imgur.com/58Lr6Pw
Mesh 3: https://imgur.com/BWFbmv0
Mesh 4: https://imgur.com/a2fLFJW
Mesh 4 (Contact Patch): https://imgur.com/QzjAQm2
Velocity Plot at Intake: https://imgur.com/rIfqMRO
Pressure Coefficient Plot at Intake: https://imgur.com/rdBtvin
Air Intake Physics Setup: https://imgur.com/Sf5bruM

[lightning0]

Did you not use the k omega SST solver for a particular reason?
How many prism layers do you have on the surface?
Regarding the values for drag and downforce, maybe your vectors in the report definition is facing the wrong direction?
At 400ms constant density is not a correct assumption as you have to take into account compressibility

[AndreP]

Originally Posted by lightning0

Did you not use the k omega SST solver for a particular reason?
How many prism layers do you have on the surface?
Regarding the values for drag and downforce, maybe your vectors in the report definition is facing the wrong direction?
At 400ms constant density is not a correct assumption as you have to take into account compressibility

I choose K-Epsilon over SST due to less computational power. It's for my dissertation and I backed this choice with literature!

Around the car I have 8 prism layers, with 1.15 growth and 5mm thickness. Around the air intake I have 10 prism layers, 1.15 growth and 5mm thickness.

I put constant density because the simulation is at 55 ms! But It's speeding up crazy around the air intake (which have a pressure outlet at 0.8781 bar) I don't know why!

Edit: But actually the K-Epsilon is a starting point only, the K-Omega SST will be a backup technique (alongside with Poly mesh) in a case where the problem is not converging! It's just that I feel that it's still not converging for other reasons that are not the Turbulence Model or the Mesh type!

[AndreP]

The drag and downforce vectors are setup correctly I assume! Here's a print screen of the settings:

https://imgur.com/oZG5oXU

In this URL you can see the car and the axis to confirm the direction of the vectors: https://imgur.com/58Lr6Pw

[lightning0]

Regarding the solver, I know that star ccm recommends omega sst or Sparata Allmaras (not sure about the spelling) for vehicle external flows so maybe try it if the epsilon doesn't work. Star ccm also recommends a prism layer thickness of 24-32 for external flows around wings. I don't have links but it's presentations by them that you could find through google. Regarding the downforce, the positive value is correct as it's parallel with the normal. As for the negative drag I don't know why that's happening. Link a pic to your y plus values. Also did you see the simscale seminar on the f1 cars? Maybe it could help. I'd recommend using simscale for your project as you'll get results much faster than your laptop

[AndreP]

Originally Posted by lightning0

Regarding the solver, I know that star ccm recommends omega sst or Sparata Allmaras (not sure about the spelling) for vehicle external flows so maybe try it if the epsilon doesn't work. Star ccm also recommends a prism layer thickness of 24-32 for external flows around wings. I don't have links but it's presentations by them that you could find through google. Regarding the downforce, the positive value is correct as it's parallel with the normal. As for the negative drag I don't know why that's happening. Link a pic to your y plus values. Also did you see the simscale seminar on the f1 cars? Maybe it could help. I'd recommend using simscale for your project as you'll get results much faster than your laptop

Those 24-32 prism layers will certainly be for a Y+ value between 0-5, which for a external flow of the full car I won't achieve and I don't want... I'm into High Wall Y+ values (30 to 300)! Also, when having so many prism layers in a complex geometry as a full car, when there's angles they would be very difficult to merge into each other and would create a bad quality prism layer! Hence, although still not perfect, (still need to make the values lower than 300, I don't think the prim layer is making any problems).

Yes, I saw that seminar! And I'm not running the simulations on my laptop, I'm using Oxford University Cluster! It's just that I start to run them in my laptop, to make sure they run a few iterations without problem, and then submit to the cluster (which these last days have been flooded, and jobs queueing for 2 days!).

I can't use SimScale because this work is for my dissertation, so I can't make it public (which is what happens when you upload to free account of SimScale, they become public).

But thanks for the help anyway!

I don't think that K-Omega would make such a different in this case (turning a negative Drag to a Positive drag), but I'll try it either way, it doesn't hurt!

I really think it is something related with the Air Intake Outlet Boundary! (I'll try disabling this outlet, and make it a simple wall and leave it to run Overnight to see what happens!).

[lightning0]

Ok I did not know about high prism layers and merges with high angles.

Did you get your air intake BC from that seminar? As there is one where you are guided through a simulation. You can actually register with your student email and then email support asking for you account to be made private as is my account. Check your y+ values though. Sometimes with high curvature you can get well over 300

[AndreP]

Yes, if you have a big number of prism layers, and lets say, it faces a 60 degrees or 120 degress change in geometry, sometimes it starts to deform the cells and it's not so easy to control them and made them good quality! But it's possible, it's just that I can't control the prim layers that good!

Well, my air intake is simply defined as a Pressure Outlet, which I assigned the value of 0.8781 bar! I didn't saw from the Webinar (which I'm reviewing to the boundary conditions part), because it seemed pretty simple and straight forward!

I didn't knew that about the SimScale! I'll definitely have that in mind, but now I would like to stick with StarCCM as it's been in my Project Proposal, and actually changing the software of use, I would have to justify and bla bla bla...

By the way, if you're using it more. How long does it take to run a simulation? (Queueing, Meshing, Solve) and what size simulations do you run there? Thanks!

[lightning0]

You said this: "Majority of the car between 0-30"...I read in a journal article that between 5 and 30 is not recommended. The article compared the different solvers not sure if I downloaded it. Maybe this could be your issue.

I'm not sure about intake BC's but I can forward you a pdf that was used for formula student cfd. It has info about the radiator modelling. Simscale converges a 3mil mesh for vehicle cfd in about 1.5 hours. Que time is a few minutes at most. I actually started my thesis on star ccm and i'm swapping over to simscale as it's just so quick. My university did not want to give me access to their cluster so...

Also you could use the 2015/6 F1 cars designed by Perin (if you can change your vehicle). They are much simpler in geometry

[AndreP]

Actually, after researching and talking with some friends, I find that maybe the Wall Y+ values might be screwing it all up for me!

I just backed up the prim mesh to try to make all the values between 30-300 and see the results!

Also, put up another simulation to run with the air intake as a simple flow split outlet, and bigger refinement in the wake. Another one with SST (although, if the K-E is not converging, I doubt K-Omega will!).

Yes, if you could forward that to me I would be thankfull! My email is affp_93@hotmail.com

I'll definitely have a look at the simscale (I'm already registered), because I'm actually using the 2017 Perrinn Formula One Car (Very simplified for lower cells number)!

Thank you for the heads up!

[me3840]

If you have a Cp on the surface of the car of 38, you get velocities over mach 1, and have negative drag, then your problem is not related to turbulence models or y+ values. You have some fundamental problems in your boundary conditions or mesh.

Why are you using flow split outlet? Your only pressure now specified in the domain is from the engine intake. I would switch this BC for a pressure outlet as is standard practice for 99% of aero simulations.

I would also just turn the engine intake BC to a wall for now. If you can't solve it with the engine off, you certainly will not with it on.



Your mesh gets very fine in the wake and very coarse extremely quickly. I would drop the wake refinement and make sure the domain has a pretty uniform size far away from the car that's not absurdly large. I usually use cells in the 200-100mm range far from vehicles, no larger.

Why are you using the surface wrapper? This geometry looks pretty clean, there's no reason you should need it.

Are you sure you set the pressure coefficient reference values correctly?

When you start on more complex geometries like this the key is to start with a coarse mesh with easy BCs. If you can't get that to work, moving to a 25M cell mesh with questionable BCs is an exercise in frustration.

[AndreP]

So, couple of notes from yesterday's simulations...

Tried to simulate with SST, and alghough looking a little bit better residuals, they're still too high.

The reason that the drag was negative, it was because in the Report, I selected the whole car to show the force (including the pressure outlet boundary), which because it was sucking, it would actually push the car. Deselecting this boundary, made the drag become positive!

The simulations where I changed the air intake from Pressure Outlet (0.8781 bar) to flow split outlet, they all went CRAZY residuals E+13!

The simulations where I changed the air intake from Pressure Outlet to Normal wall, were still at the same.

I tried one simulation where I have less prism layers, to increase the Wall Y+ values above 30, and at just 40 iterations (i know it's too small yet), it's already looking better than the others (although the Tdr is higher than before, but all the rest are lower!).

I'm really unsure about how to properly setup the boundary conditions at the Air Intake of the Engine (given I want to assign a sucking pressure of 0.8781 bar)

[AndreP]

Originally Posted by me3840

If you have a Cp on the surface of the car of 38, you get velocities over mach 1, and have negative drag, then your problem is not related to turbulence models or y+ values. You have some fundamental problems in your boundary conditions or mesh.

Why are you using flow split outlet? Your only pressure now specified in the domain is from the engine intake. I would switch this BC for a pressure outlet as is standard practice for 99% of aero simulations.

I would also just turn the engine intake BC to a wall for now. If you can't solve it with the engine off, you certainly will not with it on.

Your mesh gets very fine in the wake and very coarse extremely quickly. I would drop the wake refinement and make sure the domain has a pretty uniform size far away from the car that's not absurdly large. I usually use cells in the 200-100mm range far from vehicles, no larger.

Why are you using the surface wrapper? This geometry looks pretty clean, there's no reason you should need it.

Are you sure you set the pressure coefficient reference values correctly?

When you start on more complex geometries like this the key is to start with a coarse mesh with easy BCs. If you can't get that to work, moving to a 25M cell mesh with questionable BCs is an exercise in frustration.

First of all thank you for this huge input. answering to you:

- The negative drag i found out it was because I was also selecting the air intake boundary on the report, and because it was sucking, It was generating forward force and hence the drag was negative. I deselected this boundary from the report, and the drag is now positive.

- About the Cp and Velocity I still can't figure out what's causing it!

- I'm trying to use Flow Split Outlet on the FlowDomain back, and Pressure Outlet at the Air Intake of the Car (0.8781 bar), I though this would be the ideal BC for these two outlets. Don't you agree? What do you think I should be using?

One thing I might found it could be causing problems is that I assigned a Pressure Outlet at the air intake of the car of 0.8781 bar, but it depends if its absolute pressure or gauge pressure that StarCCM is reading. I don't think it's gauge, otherwise a 0.8781 bar would actually spit flow outside, and not sucking, which by the velocity vectors, he's doing! (Although, accelerating the flow until 300 m/s which is wrong...)

- Yes, I tried to turn it into a wall, and the residuals didn't really came much better. So I'm finding it can be also related with the Wall Y+ values and also maybe needing some more lenght of the wake refinement!

- The geometry, although looking clean it still has some flaws, so I really need to use Surface Wrapper, when I tried not to use it, it encountered so many problems it wouldn't mesh

- Thanks for the input of the refinement of the wake. I now reduced the refinement (a little bit more coarse mesh), and extended so the total lenght of the wake refinement (3 step) is now 11m (the car has 5m lenght). I can still try to change the Template Growth, but I don't want to absurdely increase the cell size, so i'll try like this, and if it's not enough, I'll use this!

- For the pressure coefficient I used the velocity of 55.55 which is the inlet speed, 1.18 for the density and the reference pressure given in the Physics Continua!

- The problem with starting with a much coarse mesh, is that at start, I'll not achieve convergence, and I'll not know if it's because the mesh needs refinement of if the physics are incorrect. So I always start at an intermediate point, with some volumetric controls in zones I already know I'll need refinement!

[me3840]

You can't just remove a surface and call the drag positive. (can you prove to yourself why? hint: draw a control volume around the car)

No, I do not agree those would be the ideal BCs. Make them both pressure outlets. Flow split outlet (without specification of the mass flux) is a hand-wavy BC for internal flows. Personally I'd never use that BC for anything.


Leave the engine BC as a wall for now. Until you get forces that are reasonable from just wall boundary conditions you should not move on. I would encourage the use of force coefficients instead, they will give you a better idea if your answer is ridiculous or not.



That being said, you need to see if your pressure is gauge or absolute. You can do a hand calculation to see how big the velocity in the snorkel will be, approximately. STAR-CCM+ is using gauge pressure, I would recommend you read the user guide on pressure referencing.


The problem is not your wake refinement, but the maximum cell size you've specified for the trimmer is too big. The cells should not grow to be larger anywhere than 200mm or so for external simulations. Refining the outer box to that size will cost an insignificant number of cells.

Do not gauge a CFD simulation as good or bad based solely on the residuals. Look at engineering quantities as well.

[AndreP]

Originally Posted by me3840

You can't just remove a surface and call the drag positive. (can you prove to yourself why? hint: draw a control volume around the car)

No, I do not agree those would be the ideal BCs. Make them both pressure outlets. Flow split outlet (without specification of the mass flux) is a hand-wavy BC for internal flows. Personally I'd never use that BC for anything.


Leave the engine BC as a wall for now. Until you get forces that are reasonable from just wall boundary conditions you should not move on. I would encourage the use of force coefficients instead, they will give you a better idea if your answer is ridiculous or not.

That being said, you need to see if your pressure is gauge or absolute. You can do a hand calculation to see how big the velocity in the snorkel will be, approximately. STAR-CCM+ is using gauge pressure, I would recommend you read the user guide on pressure referencing.

The problem is not your wake refinement, but the maximum cell size you've specified for the trimmer is too big. The cells should not grow to be larger anywhere than 200mm or so for external simulations. Refining the outer box to that size will cost an insignificant number of cells.

Do not gauge a CFD simulation as good or bad based solely on the residuals. Look at engineering quantities as well.

Once again thank you so much for your input!

Well, I didn't emoved a surface of the car, basically this was a virtual surface, which is the plane cut of the air intake system, which doesn't belong to the car, it's just a Outlet Boundary! That's why i deselected in the drag and downforce report! All the rest of the car is still selected!

I'll try to run some simulations with both outlets as pressure outlets (Engine Outlet @ 0.8781 bar and the Flow Domain Outlet @ the reference pressure in the Physics)! I'll let you know the result tomorrow!

I'll also reduce the maximum cell size for the trimmer to reduce the cells at the end of the flow domain and see the results!

Once again thank you for your input! I'll let you know how it's going!

[AndreP]

I put to run 2 simulations. One with Flow Domain Outlet as Pressure Outlet (101325 Pa) and Engine Intake with Wall BC. And another one with Engine Intake as Pressure Outlet (0.8781 bar).

They're half car simulations, so should take 1h until I have a taste of how they're going!

I also limited the biggest cell size to be 200mm!

[me3840]

Did you set the domain outlet pressure explicitly to 101325 or did you leave it as 0? What is your reference pressure?

[AndreP]

Originally Posted by me3840

Did you set the domain outlet pressure explicitly to 101325 or did you leave it as 0? What is your reference pressure?

My reference pressure is 101325, so I went to the Domain Outlet Pressure and explicitly put 101325 pa! Because from my understanding, the pressure outlet is an absolute value! Or am I wrong?

[me3840]

Originally Posted by AndreP

My reference pressure is 101325, so I went to the Domain Outlet Pressure and explicitly put 101325 pa! Because from my understanding, the pressure outlet is an absolute value! Or am I wrong?

Yes, that is wrong. Please read the documentation on pressure referencing and the boundary conditions you're using. Putting in numbers without being absolutely sure of what they mean just causes far more trouble.

[AndreP]

I read the "Flow Boundaries Reference" and although not specifically saying there it's gauge or absolute, I understanded it was absolute.

So I guess that's where my problem with the Engine Air Intake is. Because I was assigning a Pressure Outlet of 0.8781 bar, so this will actually mean it's pressure above the reference. So, the correct value, to specify it'll have to be -13515 pa? 101325 (reference pressure) - 87810 pa (pressure at the inlet)

Either way, I'll first try to follow your idea of defining the air intake as a Wall, defining the Flow Domain Outlet as a Pressure Outlet, with a pressure value of 0 pa. And try to converge the solution!

Can't thank you enough for the help! I know if may sound as I'm just here wandering for help and for people to tell me exactly what to do, but that couldn't be far away from the truth. I've been working on these simulations on the past 3 weeks 8h/day! And between CAD & Cluster problems, it all starts to get frustrating!

Thank you!