[AndreP]

Hello,

I'm a master student of Motorsport Engineering and for my dissertation, I'm doing a Wind Tunnel validation oh a scaled model of a Halo in our wind tunnel. I have a medium theory knowledge of CFD and low/medium practical of CFD.

Unfortunately, I think I might end up choosing a way too large model (given it's only 2.5mm separated from the wall in each sides), but still, I'm trying to do a CFD Method to validate against 12 pressure taps I put alongside the model, comparing the pressure coefficient in these 12 taps with the wind tunnel data I'll have, running from 15 to 35ms (5ms increment).

My question here is the following:

All my residuals are bellow 1e-4 except TDr (1e-2). Before you all go mad, I KNOW RESIDUALS AREN'T EVERYTHING, that's why I turned of Normalization and I'm also looking at the Drag and Lift forces, which are stabilised.
I was having higher TDr (1e-2) until I read in this forum that TDr relates to the prim layer, so I put more prism Layers and it reduced the TDr by 1 order of magnitude, but I got to the point which I can-t make it lower.
My problem here is the following: The Halo is 2.5mm away from the wall (I have 1.25mm prism layer thickness at the halo (12 layers) and 6 layers at the wall with thickness of 0.8mm. The problem is, probably I would need a bigger thickness, because the boundary layer is bigger than 1.25 and 0.8mm, but if I do it, they'll collapse and connect, since they're only separated by 2.5mm.
I used a Volumetric control with 0.3mm to fill the space between them, but still unsure about the accuracy of the values I'll have.

My biggest question is: Given your experience, would you feel that StarCCM+ will give me exact pressure coefficients alongside the Halo close enough for a Wind Tunnel validation? Even though the values of Drag/Lift seems stable, i'm afraid of the slightly high TDR!

Here are some print screen I think may help explain my doubts.

(Probably you're gonna need more screenshots to evaluate, just ask me and I'll post!)

http://imgur.com/Tw1pD2g

https://imgur.com/YM3PhLo

https://imgur.com/42wch08

https://imgur.com/Jcox9cw

https://imgur.com/qRuiZCG

My overall settings are:
Mesh (13.000.000 cells):
Surface Remesher
Surface Wrapper
Trimmer
Prism Layer mesher
Base Size: 1mm
Prism Layers: Halo - 12, Test Section - 5
Prism Layer Streching: 1.15
Prism layer Thickness: Halo - 1.25mm, Test Section - 0.8mm
Surface Relative Minimum/Target: 0.8mm / 2mm
Template Growth: Very Slow
Wrapper Scale Factor: 75
1 Volumetric Control Between Halo and Test Section: 0.3mm
Trimmer Wake Refinement: 1.5mm

Physics:
Constant Density,Gas, K-Epsilon Turbulence, K-Epsilon Two-Layer, Reynolds-Averaged Navier-Stokes, Segregated Flow, Steady, 3D, Turbulent, Two-Layer All Y+ Wall Treatment
Speed: 25ms (Initial 0ms)
Turbulence Intensity: 3%
Turbulent Lenght Scale: 0.01m
Inlet/Outlet is No Slip
Walls around are "Slip" to have boundary layer build up (Like in the test section of wind Tunnel).


ANY additional information you may need, just ask me and I'll put it straight away here!

Here are some images of the real piece in the wind tunnel:

https://imgur.com/rVXe6rG

https://imgur.com/XqY5hXH

https://imgur.com/MpEXu9j

[AndreP]

In case it helps anyone helping me, here is the StarCCM+ v12 Simulation and Results!

https://drive.google.com/file/d/15sC...ew?usp=sharing

It has around 3.2Gb! Feel free to download and to give me your input!

[AndreP]

Could anyone help me how to improve my TDR in this specific situation?

I've been going through this forum and I found that TDR is related to prism layer, I already improved my prism layer and the TDR got down, but wont go further, as the prism layer between the body/wall is only 2.5mm and I can't use higher thickness.

Is there anything I can further do to improve the prism layer in this sectioon? (Note that the prim layers are already beeing compressed at this zone)!

[AndreP]

Is there anyone that can maybe help me? I've been trying to improve it without sucess!

I should add that I'm using a cluster to run the simulations, so the limit of the cells is much higher than a normal computer! (Im now running 24M cell simulations)

[acalado]

First of all those residuals could be fine in terms of validation. You should try to plot the experimental and computational and see how you are so far.

Second, for TDR could be related to boundary layer calculations perhaps, so you could try and plot the y+ to get an idea of how fine the mesh is at the wall, and either adjust or select a specific wall model (even though All y+ should be pretty good at handling this).

Lastly, I am a bit confused on
"
Inlet/Outlet is No Slip
Walls around are "Slip" to have boundary layer build up (Like in the test section of wind Tunnel).
"

The walls should be No slip? And why Inlet should be an inlet, outlet an outlet, there is no slip/ no-slip condition for these boundaries as the flow is going through them.

[AndreP]

Hello acalado, first of all let me thank you for your answer! So, going point by point:

- I already compared the Wind Tunnel data and CFD data, here it is:

https://imgur.com/a/0530eHZ

For better understanding, here is an image with the position of the different pressure tappings:

https://imgur.com/a/D1wnS9Z

As you can see, basically the pressure tappings at the centre, I have a good validation, but as closer to the wall, the values start to get worst! I think this might be one of two things: The prism layer beeing condensed due to wall proximity, or the Turbulence model that I choose (Realizable K-Epsilon) that it's not very accurate for Wall interactions!

The Y+ values are pretty good, I have less than 5, either in the body and in the wall! Here is 3 print screens with the Wall Y+ both in the body and in the wall! As you can see, both the Halo and the wall have Low Y+ values, even in the zone that is 2.5mm away from the wall!

https://imgur.com/yXULqMB

https://imgur.com/0hVaFSe

https://imgur.com/gQ1wVlz

About the Inlet/Outlet, nevermind! I got confused! Of course the inlet is defined as inlet with 25ms speed and the outlet as outlet.

What I wanted to say is that the walls are defined to "no slip"to create boundary layer (to recreate the walls of the wind tunnel)!

I think that the only problem here will be the Turbulence model right? I guess it's the only justification for the problems validating near the walls? Or is there something that I can further do?

I tried to use the SST K-Omega Turbulence model, but it's harder to converge, and because my prism layers in the body near the wall is not very refined (due to Prism Layers being collapsed) the residuals don't seem very good!

[acalado]

Have you tried using less prism layers? Try 6 instead of 12 and check the differences

[AndreP]

Originally Posted by acalado

Have you tried using less prism layers? Try 6 instead of 12 and check the differences

Yes, when I was using less Prism Layers, (8 instead of 12), the TDr was bigger (0.01 instead of 0.001)!

[acalado]

Hmm... well then perhaps it could be mesh-related. If you tried K-Omega and it was worse.

I know the surface wrapper isn't as good by default as the other one.

Also I'm not sure using a trimmed mesh is better than the default polyhedra since the flow should not be particularly aligned with any of the axis and should be considerably 3-dimensional.

[AndreP]

Originally Posted by acalado

Hmm... well then perhaps it could be mesh-related. If you tried K-Omega and it was worse.

I know the surface wrapper isn't as good by default as the other one.

Also I'm not sure using a trimmed mesh is better than the default polyhedra since the flow should not be particularly aligned with any of the axis and should be considerably 3-dimensional.

Well, that is definitely two things I didn't considered before!

K-Omega I didn't compared with Wind Tunnel data because I didn't had it at the time! But since the residuals went up I though it was worse, but maybe I'll try now to compare the results to see if it's really worse!

I'll try to simulate with polyhedra mesh then!

Thank you for the two heads up! Will give it a try and then will report!

I was thinking it was related to the Turbulence model itself, but also, it was a little suspicious because the flow on that area is not that turbulent, it's just... compressed!

Thanks once again!

[AndreP]

In case anyone still minding about this, here's the validation results for the different Mesh+Turbulence Models that I tried to run.

Unfortunately, even with Poly mesh the TDr was still high, and when running SST the residuals just went crazy (This might be because SST needs a more refined mesh, and in the wall interaction zone, I'm unable to control the prism layers, because they're almost touching!)

Polyhedral Mesh + K-Epsilon
Validation Results: https://imgur.com/UkRU95P
Residuals: https://imgur.com/2WvL94J

SST + Trimmer Mesh
Validation Results: https://imgur.com/trdsZSH
Residuals: https://imgur.com/KTdwd9j

SST + Polyhedral Mesh
Validation Results: https://imgur.com/qgBFQja
Residuals: https://imgur.com/dsBJ6aj

SST (Gamma Transition) + Polyhedral Mesh
Validation Results: https://imgur.com/jCya3TY
Residuals: https://imgur.com/HLh9hjG

I'm now moving forward in the dissertation, going for a Full F1 Car simulation and then add the Halo there. But I would still like to learn how can I control the prism layers with near wall interaction (StarCCM+ is collapsing the prism layers)

[Maddin]

Sounds more like you make trial and error without understanding of what you are doing?

Cause you mentioned it's your dissertation
Can you summarize your setting please - for each point.
Why you choice this - 2-3 sentences.

I wasn't aware that Motorsport is already a Master, thought years about doing my Master of Automotive Engineering only for the email signature

[AndreP]

I never mentioned to be a professional in CFD, in fact, I'm really a begginer.

My Dissertation is the aerodynamic impacts of the Halo, my dissertation is not CFD. As CFD is one of the tools I'm using, i'm not expected neither I have time, or knowledge, to go 100% indepth of pure CFD, but instead, CFD applied to race cars.

I feel I have a good understanding of physics and mesh settings, that allow me to reasonably being able to setup a CFD simulation. Although, I'm not confidence in reading post processor (using post processor to fix simulation problems, aka understanding the real meaning of each residuals, etc etc etc)

[Maddin]

That’s why I’m asking for explaination for your choices.
Constant density wouldn’t be my choice for example.

Read the manual of ccm, for the most settings some good explanations are in.
You don’t need to be a Professional Cfd guy to understand the settings.

[AndreP]

Originally Posted by Maddin

That’s why I’m asking for explaination for your choices.
Constant density wouldn’t be my choice for example.

Read the manual of ccm, for the most settings some good explanations are in.
You don’t need to be a Professional Cfd guy to understand the settings.

I know there's not enough things we can read, and Help menu is definitely a good help! But, it's just hard to find time to Design changes, CFD them, Print the model, validate on Wind Tunnel. In any of these steps I have to read and research literature to validate each decision!

I love it, don't get me wrong. But of course, some specifics will be left out!

I choose the Constant Density not based on anything to be honest, but only for the Tutorials that my supervisor provided! I will have a look at the help file on this, and will try to see if it's the most adecquate one for my problem! Thank you for the heads up!

[AndreP]

Originally Posted by Maddin

thought years about doing my Master of Automotive Engineering only for the email signature

That would be an expensive email signature!

[Maddin]

Well, it's nothing more. You don't earn the money later on... 2 years are 150-200k in europe you have to earn more + the money you needed during the 2 years master. So at the end you need a 300k+ higher income over the years.
This will be really hard - but may this changed today cause of the bachelor stuff...