CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Validation case for drag and downforce prediction on a racing car (http://www.cfd-online.com/Forums/main/107635-validation-case-drag-downforce-prediction-racing-car.html)

julien.decharentenay October 2, 2012 18:20

Validation case for drag and downforce prediction on a racing car
 
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

Martin Hegedus October 3, 2012 00:49

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)

SergeAS October 3, 2012 06:51

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.

julien.decharentenay October 3, 2012 06:56

2 Attachment(s)
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.

julien.decharentenay October 3, 2012 07:07

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.

Martin Hegedus October 3, 2012 15:22

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.

plucas October 3, 2012 18:21

Quote:

Originally Posted by julien.decharentenay (Post 384705)
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

julien.decharentenay October 4, 2012 08:08

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

plucas October 4, 2012 09:08

Quote:

Originally Posted by julien.decharentenay (Post 384899)
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.

mohw2002 October 6, 2012 17:38

perforated pipe (wellbore)
 
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.

scipy October 7, 2012 07:20

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.


All times are GMT -4. The time now is 04:29.