[AndreP]

First of all I want to thank each one of you that has invested your time to help me!

I left various simulations to run overnight with different configurations, and although I'm not really confident I achieved convergence, I think that I'm now close! So here's a small recap of the night simulations:

I tried one simulation just changing the mesh type from Trimmed to Polyhedral (I was avoiding this because Poly suposely is more computational requiring, but soon discovered that in my problem it even has reduced the cell number!). And instantly the residuals went down and the forces start to show stabilization!

Print Screen:
Polyhedral Mesh (Without any special refinements, just used the previous trimmed mesh and change it to Polyhedral): https://imgur.com/yIuIjiM

As you can see the residuals went down, with only the Tdr and Tke on non acceptable values, and I though I could bring them down with wake refinement.

Then I picked up that mesh, and limited the maximum cell size at 200mm: https://imgur.com/UtKnGit (Flow Domain Outlet still as "Flow Split" and Air Intake as "Wall"): https://imgur.com/uD3cOwX

This is FLow Domain defined as "Pressure Outlet" @ 0 pa and Air Intake as "Wall": https://imgur.com/FP8lhHv

This is Flow Domain defined as "Pressure Outlet" @ 0 pa and Air Intake as "Pressure Outlet" @ -13 515 pa: https://imgur.com/brsDwom

This is WITH wake refinement (Flow Domain Outlet defined as "Pressure Outlet" @ 0 pa: https://imgur.com/j5TP4RJ

As you can see from the Print Screen the Drag and Downforce forces are stable in all simulations and vary not a lot throughout the different simulations (although I'm still unsure why I'm having Lift instead of Downforce (The vectors are correct!))

It doesn't make sense to me that I picked up the baseline mesh (turned into Polyhedral), showing just high Tdr and Tke above 1e-4, and after applying mesh refinement in the wake and in the all regions, these values grew up!

On the positive side, I have to send a HUGE thank you to me3840 for correcting my physics. What was happening is that, when I was assigning the value for the Pressure Outlet in the air intake of 0.8781 bar, this pressure here is Gauge with the reference pressure, which was creating a HUGE vacuum effect (hence the super high speeds). As you can see from the print screens above, the simulation with both the Flow Domain and Air Intake at Pressure Outlet, didn't "crashed" with huge residuals, so I'm guessing that for now, the physics are correct!

Although the drag and lift forces are stable, I'm not too sure about convergence because I'm not trusting the lift forces (against the Downforce expected too much). I'll post this for now and I'll try to do some more plots to see what's really happening!

[AndreP]

Here are some more plots from the post processor:

These post processors are from the Simulation with: No wake refinement, Flow Domain Outlet defined as "Pressure Outlet @ 0pa" and Air Intake defined as "Pressure Outlet @ -13 505 pa".

Mesh View 1: https://imgur.com/IorRaMx
Mesh View 2: https://imgur.com/on57teQ
Cell Quality (OK): https://imgur.com/8J8ksg8
Skewness Angle (OK): https://imgur.com/zbZuHTI
Wall Y+ Values between 5-30: https://imgur.com/Rq7g8PB
Wall Y+ Values between 3-300: https://imgur.com/ldChH9j
Pressure Coefficient: https://imgur.com/IVShH96 (Why is this still showing results that doesn't seem sensible to me? At the left you can see that I setup the Velocity, Density and Reference Pressure. What is strange is that if I put the reference pressure at 0 pa, the scale changes to -32 to 1.0235 which is much more sensible! I though this "Relative Pressure" would be related with the Physics Relative Pressure, I don't see why would we have to show the "relative pressure" of the plot, relative to the "relative pressure" of the physics
Velocity Plot 1: https://imgur.com/7qjyRfm
Velocity Plot 2: https://imgur.com/hbFTTnv
Velocity Plot 3: https://imgur.com/KAeE5a1
Velocity Plot 4: https://imgur.com/LmgMV3w

I found also this being strange: On the vector scene of the velocity, I tried to plot the velocity vectors from 0-60 m/s., given my inlet speed is 55.55m/s to confirm that the air flow is reaching the car at the right speed, but when I put the scale from 0-60m/s everything disapears. Even the zones where the speed is low, for example on the upper part of the wings, etc etc etc

With all your help, I feel like this simulation is much closer to a convergence, although, there's still something that doesn't feel right to me!

[AndreP]

My next step will be pickup on this last simulation, with the correct physics that I want to simulate, and will try to refine all the turbulent areas (Wake, cockpit and Tyre Wake), and see the results! All the simulations above are still running, because some of them still showing a trending of lowering the residuals, and also, because it's Polyhedral, I want to let them reach 1000 or 1500 iterations or at least, let the residuals reach stabilization! I'm also running one simulation where I use the SST K-Omega instead of the K-Epsilon to see how the convergence of the values and residuals go!

[AndreP]

I refined the Wake of the car, 3 incremental steps with mesh size of 20mm, 30mm and 50mm. Refined also the cockpit zone and wake of the tyres with 20mm, and the air intake zone with 7.5mm.

Checked the Y+ values, and all the car is between 30-300 (theres only a couple of cells between 300-600), but all the air intake, the inside faces, are between 5-30! Maybe this is also causing some problems.

At this moment, has run 630 iterations and the residuals are the following:

Continuity: 5e-6
Z-Momentum: 1.4e-3
Y-Momentum: 2.8e-3
X-Momentum: 2.8e-3
Tke: 7.4e-3
Tdr: 2.4e-1

All of them showing still intention to go down. But in all the preliminair simulations I've done the Tdr is always too high (between 0.001 and 1)...

The forces are starting to stabilise (only rising a little bit of the drag and the lift is stopping oscilating):
Drag: 2040 N
Lift: 2870 N (This wasn't expected, as I was expecting Downforce generation)

From my previous experience, I would fix the Tdr by refining the Prism Layer mesh, but this time I can't, because I don't want the car to fall on the 5-30 Wall Y+ region. SO I consider that my Wall Y+ values are correct now (still need to remove the air intake from the 5-30 zone), but on the overall I wouldn't change a lot of the Prism Layer settings, because the Wall Y+ value is the desired one.

How could I potentially improve the Tdr? I already have Volumetric Control on the wake of the car, wake of the weels, and two turbulence zones (Cockpit and Air Intake). I really don't know how to bring it down. Maybe needs further volumetric refinement?

Also, througout the simulations, sometimes I have warnings popping up on "Turbulent Viscosity Limited on X cells in Region", these warning come up, and then come down. From what I've read, this is not alarming if they're coming down and eventually fade away. But, can this be telling me something about my physics?

[AndreP]

After going through a lot of forum topics and Help files, I think I might start to face the problem as converged.

Both the drag and lift forces are stable for hundreads iterations and in fact, they all share the same values in almost 10 different simulations with various types of mesh configurations and refinements! And the residuals doesn't show any spikes and show a linear decrease and flattening over time... Although, I was still expecting the generation of downforce and not lift!

The residuals normalization is turned off, that's why the Tdr being around 0.1 is giving me a hard time accepting convergence (Although it goes to about e-7 after turning "Auto" normalization)!

Would you feel the simulation has reached a state of convergence, and hence, the results may be assumed?

[AndreP]

After freaking out a little bit about the lift, I tested by plotting the downforce only on the rear wing (one region I knew FOR SURE there was downforce) and yes, it was giving 800N of downforce, so the Lift "issue" is not an issue, it's correct!

[me3840]

Originally Posted by AndreP

After freaking out a little bit about the lift, I tested by plotting the downforce only on the rear wing (one region I knew FOR SURE there was downforce) and yes, it was giving 800N of downforce, so the Lift "issue" is not an issue, it's correct!

I'm not sure I agree with this. If the whole car gives lift together that's pretty unexpected. Put any plate close to the ground and push flow through it, and it'll suck down.

You have to remember that residuals aren't the end-all. The way the residuals are calculated depend a lot on the code, as you saw in that other thread. They can lie, being poisoned by some really bad cell which on the grand scheme is unimportant. It's most important that you use engineering judgment to see if your answer is correct. Do you know how your airfoils are expected to perform? Have you looked at papers reporting force coefficients for bodies similar to yours? Can you do some hand calculations to ensure you're in the ballpark?

Look at your simulation and figure out if you can see why you have lift. I would not expect that to occur at all, certainly not at that force level. Also I would really encourage the use of force coefficients instead of real forces. It's really hard to compare to other cases using raw force values.

The reference pressure for Cp in the field functions is also gauge. Set it to 0 (as you found). Relative pressure is a field function not really related to gauge, it's related to moving reference frames, which I don't think you need to worry about right now.

[AndreP]

Well, unfortunately I can't compare with values generated from other simulations because my car was completly simplified, as shown in these screenshots:

Baseline 1: https://imgur.com/9u5Q2oO
Baseline 2: https://imgur.com/mh7jSCE

Simplified 1: https://imgur.com/Icqmrwj
Simplified 2:https://imgur.com/ra2uK3D

I was using forces instead of coefficients because forces are "faster" to setup on the report, because what I use these forces to is JUST to see if they're converging or not, and actually changing to Coefficients would give me the same plot variations. When reporting in my final document, I always use coefficients!

Well... Once again, I was dumb... very dumb! Basically what I did is, in the report of the Drag and Lift, (again) I used the reference pressure on the physics and put it on the reference pressure of the report! Thats why it was generating the Lift.

How did I found this out?

I plotted the Lift generation alongside the car: https://imgur.com/0zj5XTq

And I saw that the accomulated force was, in facte, Downforce! So I went to the report and saw that I should've left the "Reference Pressure" as zero!

Now I'm generating, FINALLY, expected values:

923N of Drag
568N of Downforce!

Really really thankfull for all of your help!

[AndreP]

My stress levels on the last couple of weeks have been going over the top, because this is the Baseline simulations! All of the other simulations I'm doing next are based in this one, so I really needed to get this one done with a good mesh and good results, to be able to run the other ones (different Halo geoemetries)! And I'll not be able to run simulations after the 29th August, and I was facing problems and I couldn't see way around! I was getting very nervous and stressed! But with your help, my dissertation is back on track! Can't thank you all enough! Especially to me3840!

[AndreP]

Yesterday I left another simulation, improving the mesh on the Air Intake area (which was between the 5 to 30 Wall Y+ values), I got almost all the values out of this zone, putting them in the 30 to 300 zone, and the Tdr and Tke residuals went down to the 1e-7 and 1e-8 almost immediately! Before fixing this Wall Y+ region of 5-30 they were around 0.05 and 0.01!

So, to recap all the problems that I had in this project, in case anyone is having the same problems:

- Problem in the Physics:
What was causing: I was assigning a pressure outlet of 0.8781 on the Air Intake of the car.
How did I found out there was a problem? Residuals and Velocity/Pressure Coefficient Plots
How did I fix? ALL the Reference Pressures, are GAUGE with the Reference Pressure assigned in the Physics. So instead of 0.8781 bar (87810 pa), I assigned -13515.0 Pa to this intake (and 0 pa to the Flow Domain Outlet). The value was calculated by subtracting the desired value by the Reference Pressure defined in the Physics: 101325.0 Pa - 87810 pa = 13515 pa! (You put it negative of course because this pressure was bellow the reference).

- Problems in the Tdr and Tke convergence:
What was causing: Wall Y+ values between 5-30!
How did I found out? Plot the Wall Y+ values on your domain
How did I fix? Increase/Reduce your Wall Y+ values, to the point you have the minimum possible cells with Wall Y+ values between 5-30! (You'll end up with little ones, but if these are in non problematic areas and are just a little, it's alright)

- Problems in the Force reports and Pressure Coefficient Plot:
What was causing: Reference Pressure defined as 101325.0 Pa.
How did I found out? Drag and Lift forces were strange also the Pressure Coefficient Scalar Plot
How did I fix? Just out the "Reference Pressure" on these plots defined as 0 pa! (Or, if you want to be even more precise, place a probe on the begining of the flow domain, make it report the Maximum velocity and Maximum Pressure (to obtain the Free stream pressure and Free Stream Velocity) and use these values instead for the Reference Velocity and Reference Pressure!) (In my case the reference pressure instead of being 0 pa was 9 pa... Is a small difference, but it's a more correct procedure)!

I hope this helps someone that may face similar problems as mines!

[Maddin]

Nice that you made progress.
May you could upload the modell without mesh (smaller file sizes) and I will take a look into it.

[AndreP]

Thnak you Maddin! Yeah, finally the solutions converged and fixed all the physics problems!

I'll get the model in a few days, I'm now a little bit busy running all the more than 60 yawed simulations!

[AndreP]

Guys, I would need to ask one more thing.

All my simulations have been giving me the warning of "Turbulent viscosity limited on 48524 cells in Region".

It starts midway the simulation and stay all the way until the end with the maximum number of cells around 45000/50000 and never more than that in all the different simulations!

I plotted the Turbulent Viscosity and this is what I got:

https://imgur.com/mA1IVC0

https://imgur.com/I1EAQOQ

Just for checkup, this is the Residuals and Forces Plot (They're both converged and flat):

https://imgur.com/nxUKTCD

https://imgur.com/xetl7Gf

As you can see the turbulence viscosity is reaching its maximum at the Wake Refinement at the 30mm cell size zone. Which obviously indicated a need for further refinement.

My problem is, I'm almost reaching the Computational Power of the computers I'm using.

Given it's in the wake zone (My main focus on this project is the Car area, studying the Mass Flow and Vorticity at the Intake and Rear Wing), and that the Residuals and Forces Plot are already pretty converged and flat.

Do you think this 40.000 cells with turbulent viscosity reaching its maximum, are worth refining? Will that change a lot of my results for the Air Intake and Rear Wing?

Thank you for your input!