Race Car Moving Road( Better Ground effect simulation )

[Boris Georgiev]

Greetings, guys!

Here is in brief the situation in which i am. I couple of guys and i are desining the aero/body package of a Formula Student race car. The CAD package we are using is SolidWorks, but we are running our flow analysis in Autodesk CFD 2013. My appeal is if anyone can suggest a reasonable and efficient way of simulating moving road(ground effect) like during a normal competition. So far, after we created our computational volume ( equivalent of a wind tunnel ), we assigned boundary conditions at the inlet(NORMAL velocity) and the at bottom (Vz velocity component, with the same magnitude as at the inlet, of cource). Thanks to the Motion Setup, we assigned Rotation to the 4 wheels. However, there is some distance between the wheels and the bottom of the computational volume ( equivalent of wind tunnel ) which makes me feel a little bit worried about the accuracy of your results.

Generally, i would extremely appreciate any piece of advice/guidance for our analysis, in terms of Physical Boundary Conditions, Type of Flow Analysis(Transient/Steady State) and etc. Just anything you consider to be relevant.

Hope, more experienced people will drop some lines!

Thank you very much in advance!

[Jersey Tom]

Something to keep in mind is the line, "all models are wrong.. but some are useful."

Do you need the moving ground? What answers are you after, and will the added simulation complexity add value to your analysis? How much value? Or the time spent waiting for a way to go about it, where you could be getting answers instead?

Just things to consider.

[Greg Locock]

The traditional way is to mirror image the car at the groundplane.

Then, check what the error is compared with the free flow version, and bear those errors in mind when developing the freeflow version, and then check your final results with the mirrored one again.

Note this isn't a perfect solution, but it is correct for Z axis forces

[slimjim8201]

Boris,

A few suggestions for you.

-Make sure you are creating your virtual wind tunnel volume in CAD, and not in Simulation CFD. The latter allows for exterior volume creation, but it is limited and you cannot adjust the ground plane to get it close enough to touch the wheels of your car. The recommended approach is to ensure that the wheels of the car are slightly interfering with the ground plane, creating a sort of "contact patch". This ensures that no cusps exist where the wheel and ground surfaces come together.

- As far as boundary conditions go, you'll want a normal velocity on your tunnel inlet face, slip on the sides and the ceiling, the component velocity on the ground plane, and instead of assigning motion to the wheels, simply each group of wheel surfaces and assign a rotating velocity BC. This is much preferred over using the motion model. Motion is great for when an object moves through space, not the best for simple rotation like this.

- Mesh is pretty critical for external aero so be sure your surface density is fine enough. I'd recommend using adaptation as well, most likely with y+ control enabled.

- You may want to upgrade to Simulation CFD 2014 if you can. There are additional turbulence models in the latest version which are much better suited for aero simulation (SST k-omega, SAS, DES, etc).

James

[Boris Georgiev]

Greetings, guys!

Firstly thanks for all your responses, really appreciate it. Secondly, please, apologize me for my late answer!

To Jersey Tom:

1) Well yes, i suppose the moving ground will contribute to the accuracy and therefore i would like to add it in the analysis. Also,i forgot to mention that our primary aim is to track the levels of downforce generated by a flat undertray and a diffuser at the end. Actually the CAD model of the car is just a closed body volume, 4 tyres( without any bars between them and the body ) and the undertray with the diffuser. Even the tyres are simple circles which have been extruded, no treads nothing. We have sidepods, but when we run everything in Autodesk CFD, to many bodies appear to be assigned a material and as far as i remember the analysis crashes at some point. Therefore we suppres the sidepods. Most likely we have to fix the CAD model and make it better in terms of the sidepods and the way how they are attached to the body of the car.

To Greg Locock:

1) Please correct me if i understand you wrongly, but you mean to actually have a mirror image of the aforementioned car and running the simulation with both? Of cource, the mirror image is upside down and its four tyres contact with the four tyres of the no-image model?

To James:

1) Regarding your piece of advice about creating my computational volume in Solidworks, you think it is possible to assign Boundary Conditions when i run it in Autodesk CFD 2013. In brief computational volume from one package to be used in another one.

2) I suppose you mean the slip/symmetry (physical) boundary conditions. About the rotation of the tyres, this rotating velocity, you are talking about, is again a boundary condition, or no?

3) Concerning the mesh, in order to use Mesh Adaptation i should pick a Steady State analysis, not a Transient one? If this is the case, then i will have to read more about the Adaptation in the Solve dialogue (more specificly y+). Initially, i guessed that running a Transient Flow analysis with a mesh refinement region ( since i cannot use adaptation in a Transient Flow simulation) at the back of the car, covering the whole undertray and diffuser, should be a good alternative ( since as you know, the usual flow separation behind the back of the car is crucial for aerodynamics designs).

5) Yeah, sure i will upgrade to CFD 2014 with student licence, if possible. Does it mean that i have to entirely delete CFD 2013 or there is an option to build-up in some way on the old version?

Thank you very much again!

[Boris Georgiev]

Greetings, guys!

Hope the thread is not forgotten.