CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Validation case for drag and downforce prediction on a racing car

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By scipy

Reply
 
LinkBack Thread Tools Display Modes
Old   October 2, 2012, 18:20
Default Validation case for drag and downforce prediction on a racing car
  #1
Senior Member
 
Julien de Charentenay
Join Date: Jun 2009
Location: Australia
Posts: 229
Rep Power: 9
julien.decharentenay is on a distinguished road
Send a message via Skype™ to julien.decharentenay
Hi,

I am involved in the CFD modelling for a virtual design racing car challenge (www.khamsinvirtualracecarchallenge.com - if you missed the post earlier). I am looking at validating the methodology we are using for the CFD analysis - but I am unaware of a properly validated and documented test case that can be used. The Ahmed body could be used but it is overly simplified - let me know if you are aware of other test cases that could be used.

I am looking for your help to develop a benchmark using a blind test protocol. We have selected a geometry of a racing car (Lola B2/00 Las Vegas made by Timmy - not related to our project - and available on the SketchUp warehouse) and we would like if you could run one CFD analysis on it and submit the drag and downforce results. If we can get more than 5 results submitted and the results show some level of agreement, this case could represent a benchmark.

The results will be made publicly available including our results. Results can be submitted anonymously or not.

If you are interested, the geometry in STL format along with other information is available from https://dl.dropbox.com/u/40499338/Lo...as%20Vegas.zip

Submission of results will be through the Khamsin Virtual Racecar Challenge website - I will post the link when available.

Thanks in advance for your help.

Kind regards,
Julien de Charentenay, on behalf of Khamsin Virtual Racecar Challenge
__________________
---
Julien de Charentenay
julien.decharentenay is offline   Reply With Quote

Old   October 3, 2012, 00:49
Default
  #2
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 462
Rep Power: 9
Martin Hegedus is on a distinguished road
Wow, this will be challenging.

Even something simple such as one spinning wheel in front of another would be challenging because of the interference of the vortex from the front wheel on the second. Or, calculating the base drag on a vehicle at race Reynolds numbers. The only way, as far as I know, to reliably get the base drag is to use LES or DES. http://cpdl.kettering.edu/AIAA-2003-0857.pdf (I'm not sure what the Re for that paper was, probably much less than race car Re)
Martin Hegedus is offline   Reply With Quote

Old   October 3, 2012, 06:51
Default
  #3
Member
 
SergeAS's Avatar
 
Serge A. Suchkov
Join Date: Oct 2011
Location: Moscow, Russia
Posts: 73
Blog Entries: 5
Rep Power: 5
SergeAS is on a distinguished road
Send a message via Skype™ to SergeAS
As I understood your software is a frontend to OpenFOAM solver and you want to spend a cross-validation with other CFD solvers ? Or do you have the results of blowdown your model in a wind tunnel ? In any cases need some agreement concerning using grids for correct comparison of different results.
SergeAS is offline   Reply With Quote

Old   October 3, 2012, 06:56
Default
  #4
Senior Member
 
Julien de Charentenay
Join Date: Jun 2009
Location: Australia
Posts: 229
Rep Power: 9
julien.decharentenay is on a distinguished road
Send a message via Skype™ to julien.decharentenay
Hi Martin,

Thanks a lot for your comments. I could not agree less on the validity of your comments and the size of the challenge (see attached pictures - and remember the geometry is not clean).

For the KVRC Challenge, we will be comparing different designs so we will be focusing on trends (ie does this design generates more downforce than this one) rather than absolute numbers. We will have to limit ourselves with steady-state RANS simulation as we do not have the computational resources to run DES/LES.

We are conscious that any simulation is limited by its parameters (mesh, physical models, boundary conditions, software, etc). The purpose of this exercise (from our perspective) is to assess whether our modelling protocol (domain size, mesh resolution, steady-state RANS...) produces similar results to the results produced by other using similar or different assumptions. By sharing the results with the community we hope that this scenario can also be used by others for the same purpose.

KVRC is proposing to host the results and transfer them to a more neutral CFD focused entity later down the line (cfd-online for example if interested - I would be more than happy to skip the KVRC step and go straight for a neutral CFD focused entity).

Thanks again.
Attached Images
File Type: jpg Lola B2-00 Las Vegas (2) - view 1.jpg (49.1 KB, 27 views)
File Type: jpg Lola B2-00 Las Vegas (2) - view 2.jpg (38.4 KB, 19 views)
__________________
---
Julien de Charentenay
julien.decharentenay is offline   Reply With Quote

Old   October 3, 2012, 07:07
Default
  #5
Senior Member
 
Julien de Charentenay
Join Date: Jun 2009
Location: Australia
Posts: 229
Rep Power: 9
julien.decharentenay is on a distinguished road
Send a message via Skype™ to julien.decharentenay
Yes, Khamsin is a front end to openFoam. And Yes, I am looking for cross-validation of the solver+simulation methodology (grid, numerical model, physical model) with other CFD practitioner(s) using similar or different solvers. I am going through this exercise as a validation of the methodology for the KVRC Challenge purpose.

No. I do not have wind tunnel results. I wish I had. I would probably not be starting this thread if I had anything to benchmark against.

From my perspective, grid is part of the simulation process - along with selecting the size of the computational domain, the numerical model, the physical models, the solver parameters. I could generate a snappyHexMesh mesh and provide it if requested.
__________________
---
Julien de Charentenay
julien.decharentenay is offline   Reply With Quote

Old   October 3, 2012, 15:22
Default
  #6
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 462
Rep Power: 9
Martin Hegedus is on a distinguished road
Hi Julien,

I think your idea is cool and I do hope that you are able to find people to participate in it. I thought I would provide some opinions of mine in case they are of some assistance to you.

IMO, if you are interested in getting some quantitative science out of this, you will probably need to provide some structure or guidance.

Also, a vehicle such as this is an interference nightmare, even if simplified into wheels, front wing, back wing, body, and ground plane. For example, I read here, http://etheses.dur.ac.uk/3124/, that "Exposed wheels contribute significantly in terms of wheel drag and it has been reported by Dominy [16] that for an open-wheeled Grand Prix car the wheel drag, as a percentage of the overall vehicle drag, can be between 35 and 50 percent." That's a lot. Of course the wings will produce induced drag and the body will produce separation drag. And lift (or downward force) will probably be significantly harder to calculate than drag.

You're interested in increments. Unfortunately, if the physics are not captured, the increments will basically be untrustworthy since they are based on load differences which are calculated from pressure differences of very non linear flow.

Some of the things I would suggest are that you specify the Reynolds number, turbulence model, and whether wall functions are used or not. I would also suggest that the loads be broken up. For example, total loads, front wheel loads, back wheel loads, front wing loads, rear wing loads, and body loads. I would also suggest that a clean model (no struts, mirrors, etc) and a dirty model gets tested.

Sadly, as fun as this project sounds, I don't have the resources to participate in it. So my comments should not really carry any weight, if any at all. It's up to those who participate in it to chime in.

Take care, and good luck.
Martin Hegedus is offline   Reply With Quote

Old   October 3, 2012, 18:21
Default
  #7
Member
 
plucas's Avatar
 
Anonymous
Join Date: Dec 2011
Location: Everywhere
Posts: 75
Rep Power: 5
plucas is on a distinguished road
Quote:
Originally Posted by julien.decharentenay View Post
Yes, Khamsin is a front end to openFoam. And Yes, I am looking for cross-validation of the solver+simulation methodology (grid, numerical model, physical model) with other CFD practitioner(s) using similar or different solvers. I am going through this exercise as a validation of the methodology for the KVRC Challenge purpose.

No. I do not have wind tunnel results. I wish I had. I would probably not be starting this thread if I had anything to benchmark against.

From my perspective, grid is part of the simulation process - along with selecting the size of the computational domain, the numerical model, the physical models, the solver parameters. I could generate a snappyHexMesh mesh and provide it if requested.
provide your snappyHexMesh. I will also run this to help validate
plucas is offline   Reply With Quote

Old   October 4, 2012, 08:08
Default
  #8
Senior Member
 
Julien de Charentenay
Join Date: Jun 2009
Location: Australia
Posts: 229
Rep Power: 9
julien.decharentenay is on a distinguished road
Send a message via Skype™ to julien.decharentenay
Hi Paul,

Can you confirm if you have any requirements for the mesh? Do you intend to run RANS with wall functions, RANS with a low-Reynolds turbulence model, DES or LES? Any upper mesh size limit? Would a basic simpleFoam setup be required as well?

As a disclaimer, I have not attempted to run it. If it is ok I will keep you updated and provide updates of the geometry if I go through geometry cleaning.

Julien
__________________
---
Julien de Charentenay
julien.decharentenay is offline   Reply With Quote

Old   October 4, 2012, 09:08
Default
  #9
Member
 
plucas's Avatar
 
Anonymous
Join Date: Dec 2011
Location: Everywhere
Posts: 75
Rep Power: 5
plucas is on a distinguished road
Quote:
Originally Posted by julien.decharentenay View Post
Hi Paul,

Can you confirm if you have any requirements for the mesh? Do you intend to run RANS with wall functions, RANS with a low-Reynolds turbulence model, DES or LES? Any upper mesh size limit? Would a basic simpleFoam setup be required as well?

As a disclaimer, I have not attempted to run it. If it is ok I will keep you updated and provide updates of the geometry if I go through geometry cleaning.

Julien

I say that you pick what turbulance model, solver, and basic setup parameters. I would say that simpleFoam will work pretty well. Off that, we can prepare our own setup and run. I think geometry cleaning would be a good idea.
plucas is offline   Reply With Quote

Old   October 6, 2012, 17:38
Default perforated pipe (wellbore)
  #10
New Member
 
Mohammed
Join Date: Oct 2012
Posts: 27
Rep Power: 4
mohw2002 is on a distinguished road
Please how can I geting in CFX the wall shear stress due to friction, and how get friction factor at the perforated pipe. I am using k-epsilon model for turbulent.
mohw2002 is offline   Reply With Quote

Old   October 7, 2012, 07:20
Default
  #11
Senior Member
 
Join Date: Aug 2011
Posts: 114
Rep Power: 6
scipy is on a distinguished road
Send a message via Skype™ to scipy
Hehe, it's obvious that no one here even tried to open the STL model provided.

Julien, first step that you should take (if you plan on using this model for validation) is to make it suitable for CFD analysis. There are a lot of openings that end nowhere (such as engine intake, radiator cooling ducts), there is a lot of unnecessary details inside the model - spring/damper assemblies, simplified engine, rods going through the driver's helmet, steering wheel buttons, whole inside of the cockpit with the driver's legs etc.

All of this should be fixed according to the level of detail you plan on achieving in your CFD analysis. Even though the airflow through the car is especially important in a openwheel race car, I think you should disregard it for now. Everything should be closed up and then boundaries such as engine intake can be used as boundary conditions for mass flow inlet, radiator ducts can be specified as BC on which a certain amount of heat is disipated (say from peak engine power and engine efficiency of about 30-40 %), exhaust pipe end face can be assigned a mass flow outlet of air at elevated temperature etc.

Wheels should also be intersected with the ground and a small wedge/fillet should be added in this area to avoid sharp elements (model is currently floating about 2.5 mm above ground), origin (0,0,0) is currently on the ground below the front wheel centerline and it should be on the ground in the middle of the wheelbase. The wheelbase itself is slightly wrong (3091,4 mm instead of 3098,8 mm - calculated from 122" information found on the web for the Lola B2/00), but these are all minor details. The disc brakes are not modeled properly anyway, so they should be removed and the rims should be patched up from the outside to provide a "cylindrical wheel". Same goes for brake cooling ducts.

Suspension pickup points are a nightmare area for prism elements (sharp corners, tight spaces), plus the suspension members themselves are not streamlined (they're basically quadratic rods) so they should either be remodeled in CAD or avoided completely for simplicity's sake.

Wings are not any "airfoils" and they're basically planks with sharp leading and trailing edges and will not provide any significant downforce, or at least nowhere near the amount of downforce that they should provide. They should be replaced with NURBS airfoils of choice (something similar to ones used on the Lola, but any airfoil will have to be modified since none of them have this level of curvature in original form).

As far as solver setup goes, Paul is right and you should specify everything if you want comparable results later on. What's mostly used in automotive cases is: Realizable k-epsilon model, non-equilibrium wall functions (in Fluent, don't know about other software) and the domain size should be 5-10L in front, 10-15L behind, 5L up and 4-5L to the side. Also, you should specify if people can use symmetry (since this model is not really symmetric, fuel filler cap location, some stuff on the nose of the car etc).

If you can fix the model up, I'd be glad to make a mesh and run a RANS case. I've started fixing the model but gave up immediately after seeing what's inside the car Just don't have that kind of time.
Anna Tian likes this.
scipy is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Meshing 3D Model of Racing Car T1M Main CFD Forum 7 April 13, 2012 16:30


All times are GMT -4. The time now is 13:08.