Race Car Moving Floor( Ground effect ) simulation

[930328]

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 and etc.

Hope, more experienced people will drop some lines!

Thank you very much in advance!

[Jon.Wilde]

Hello,

Firstly I would suggest that you model the 'wind tunnel' in Solidworks, this way it can touch the geometry and be more like reality. Your Boundary Conditions sound sensible (although do you have a p=0 at the outlet, a nice long wat downstream?)

.

Advection Scheme 5 will probably be your best bet here (Solve -> Solution Controls -> Advection)

I would also suggest that you trial a 2D analysis first (keep everything in the x-y plane, insert into a new assembly if needs be) just to get an idea of the level of mesh you will need to properly capture this. Maybe you could do it all in 2D, depends what you are changing from one run to the next.

Mesh adaption will also be very useful here, but be sure to adapt the mesh from a well converged solution, not just 100 iterations.

Hopefully that helps, feel free to share some nice images if you can!

[930328]

Greetings, Mr Wiilde!

Thank you for the response and apologize for my late reply! 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.

1) Yes i have assigned gauge pressure as a boundary condition both at my intlet and outlet of the wind tunnel. 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) Advection scheme...i will do my best to find more information about it. Hope will find some guidance and explanation on the page of CFD 2013 altoghter with the other tutorials and etc.

3) The 2D analysis you are talking about...to be honest i really do not get it. However i will try to find more about it.

4) Concerning the mesh, in order to use Mesh Adaptation i should pick a Steady State analysis? Initially, i guessed that running a Transient Flow analysis with a mesh refinement region 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) Lastly, i would like to ask you if it is alright to assignt Slip/Symmetry as a bouncary condition on both sides of my Computational Volume, as well as, on the top of it. Of cource, i mean the inside walls. Should this make the analysis more realistic?

Thank you again!

[Jon.Wilde]

Hello,

Let me see if I can help further here, based on your bullet points:

1) Yes i have assigned gauge pressure as a boundary condition both at my intlet and outlet of the wind tunnel. 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. Please only assign a flow rate at the inlet and a pressure at the outlet (no pressure at the inlet).

I am not quite sure what you mean by your other question here.

2) Advection scheme...i will do my best to find more information about it. Hope will find some guidance and explanation on the page of CFD 2013 altoghter with the other tutorials and etc.

I am sure you will, please let us know if you cannot.

3) The 2D analysis you are talking about...to be honest i really do not get it. However i will try to find more about it.

2D is when we take a slice along the entire model, so that rather than running a full 3D simulation, we can run in 2D, allowing us to use more mesh and capture what is happening more accurately and faster. I recommend you try it:

Start with a new part in your assembly, right through the cente of the car.

Then sketch on a plane through the centre, projecting all of the car edges (and the wind tunnel) onto it. 

Then create a surface, leave the car hollow, you only need the air around it

Run only this part in CFD (Boundary Conditions will now be applied to edges rather than surfaces and Materials to surfaces rather than volumes).

The results should be available much faster than with the 3D approach.

You cannot always achieve everything you need with a 2D model, but you may find that you can glean enough information to save you running large 3D studies. Well worth bearing in mind.

4) Concerning the mesh, in order to use Mesh Adaptation i should pick a Steady State analysis? Initially, i guessed that running a Transient Flow analysis with a mesh refinement region 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).

Yes, use Steady State initially.

Once you gain insight into how much mesh is required (through the 2D model) and the runtimes you are likely to see when applying this in 3D, a transient analysis will be the final run to make. I would not recommend it for the early stages of analyses. There is no reason why you will not see the correct flow separation in Steady State, you just won't see all of the transient features.

5) Lastly, i would like to ask you if it is alright to assignt Slip/Symmetry as a bouncary condition on both sides of my Computational Volume, as well as, on the top of it. Of cource, i mean the inside walls. Should this make the analysis more realistic?

Yes, you can do this. Really all you are doing is removing the boundary layer/friction from the walls, nothing more complex.

Best regards.

Jon

[930328]

Hello again!

1)  Please only assign a flow rate at the inlet and a pressure at the outlet (no pressure at the inlet).

By assigning flow rate at the inlet you mean volume flowrate m^3/s? If this is the case then does it mean that we should not assign normal velocity?

2) I am not quite sure what you mean by your other question here.

Sorry, i will try to put it forward in a better and shorter way. It is possible to create computational volume in one software package and use it in another? One CFD package recognizes a modeled 'wind tunnel' in another CFD package. (e.g as you advised me to create it in SolidWorks and use it in CFD 2013, where assigning all the boundary condtions and etc.). 

3) About the Advection scheme and incompressibility.

Probably i should have mentioned this fact earlier, but the average speed for a Formula Student car is maybe between 60-70 km/h. However, we are determined to run the CFD at around 90-100km/h. Surely, at such speeds no compressibility effects are evident. Should this be taken into considerations for selecting the advection scheme?

Also i suppose that in the solve dialogue we should go for incompressible, since the other option Subsonic maybe assumes some tiny compressiblity effects?

4) Concerning the 2D analysis.

Should i always attempt it or it is just here to prevent me from running dozens of simulations in 3D and thus save a lot of time. Simply saving efforts...

5) Lastly, can we add a mesh refinement region, just in case to help with anything?

All the Best!

[Jon.Wilde]

Hello

1)  Please only assign a flow rate at the inlet and a pressure at the outlet (no pressure at the inlet).

By assigning flow rate at the inlet you mean volume flowrate m^3/s? If this is the case then does it mean that we should not assign normal velocity? You can use a flow rate or velocity, it does not matter. I suggest a velocity, as this will stay the same if we move to 2D, a flow rate would need to change with the reduction of thickness (2D assumes a unit thickness of whatever units you are using). If you do find that you have velocities where we are staring to see compressible effects, we will need to change the setup to use a mass flow rate, but let's do one run first and then assess.

2) I am not quite sure what you mean by your other question here.

Sorry, i will try to put it forward in a better and shorter way. It is possible to create computational volume in one software package and use it in another? One CFD package recognizes a modeled 'wind tunnel' in another CFD package. (e.g as you advised me to create it in SolidWorks and use it in CFD 2013, where assigning all the boundary condtions and etc.). I cannot really comment on other packages, I would have thought though that if they integrate properly with CAD then it should work OK, as we will also.

3) About the Advection scheme and incompressibility.

Probably i should have mentioned this fact earlier, but the average speed for a Formula Student car is maybe between 60-70 km/h. However, we are determined to run the CFD at around 90-100km/h. Surely, at such speeds no compressibility effects are evident. Should this be taken into considerations for selecting the advection scheme?

Also i suppose that in the solve dialogue we should go for incompressible, since the other option Subsonic maybe assumes some tiny compressiblity effects? ADV5 would cover both scenarios. See the note above though, run incompressible first and see what the max velocities are before switching to subsonic.

4) Concerning the 2D analysis.

Should i always attempt it or it is just here to prevent me from running dozens of simulations in 3D and thus save a lot of time. Simply saving efforts... Yes, exactly right. It can be a massive time saver and a nice way to understand how much mesh will be required. Try running a model and then this will become clearer.

5) Lastly, can we add a mesh refinement region, just in case to help with anything? You can add as many regions as you would like to. Probably useful where you know there will be turbulence and in the wake region. But then let th emesh adaption refine (and coarsen, this is an additional option) the mesh as it sees fit.

[lennardgoh]

For the case of creating an external wind tunnel control volume over a car body for this case. Should I create a cuboid CV that encapsulates the car body or would it be better to create six surfaces which I would later assign the BC's to. 

Thanks!

[apolo_vanderberg]

Creating an external domain, i would recommend making a volume not just 6 surfaces that meet along their edges.