Community
CFD Forum
Welcome to Autodesk’s CFD Forums. Share your knowledge, ask questions, and explore popular CFD topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

2D vs 3D Undertray CFD

16 REPLIES 16
Reply
Message 1 of 17
andrew.lesiecki
1922 Views, 16 Replies

2D vs 3D Undertray CFD

Hello,

 

 I am currently trying to do CFD on the undertray/diffuser of a race car. I have been switching between 2D and 3D. Both have their pro's and con's and I am looking for  happy medium that will be most realistic. I have attached static images of both results. The 2D shows the ground/venturri effect well but does not keep flow attached (even when I lowered the diffuser angle to 3deg.)  The 3D does not show the ground effect but it does show attached flow, which I realize some of this has to do with the vortices coming around the side that helps keep flow attached. I would like to be able to do all of my tunnel and diffuser iterations in 2D then finalize in 3D so I can see the interaction between the flat body, tunnel, wings, etc. 

 

Both have the same settings Velocity inlet, floor velocity, slip symmetry on walls(obviously only in 3D),slip symmetry on top,  and 0 pressure outlet.  Mesh regions along the bottom of the undertray and in the diffuser/ following area. Turb model RNG ratio 10. Intelligent solution control off in 2D... I know the first suggestion will be longer inlet/outlet and more iteration, I have tried these did not change the result just he time.

 

What can I do different on either of them to get ground effect and attached flow?

 

 

Thanks,

AJ

16 REPLIES 16
Message 2 of 17
Jon.Wilde
in reply to: andrew.lesiecki

I have a few thoughts:

 

  1. Why is ISC off in the 2D model, I would leave it on
  2. You could try with the SST model and also ADV5 may help
  3. What does the mesh quality look like?

Kind regards,

Jon

Message 3 of 17
andrew.lesiecki
in reply to: Jon.Wilde

1. ISC is turned off because I had been informed in a previous post that it would help because it was stopping the simulation before it was done because there was so much mesh.

 

2. Sorry ADV 5 is being used, forgot to mention that. 

I tried one run with the SST k-omega and they looked almost identical

 

3. I attached a screenshot of the mesh regions

 

 

-AJ

Message 4 of 17
Jon.Wilde
in reply to: andrew.lesiecki

You can leave ISC on but turn off the Auto Convergence Assessment within 'Advanced'

 

The mesh looks fine to me - you could test the mesh adaption in 3D but really it looks like it should be sufficient.

 

Kind regards,

Jon

Message 5 of 17
andrew.lesiecki
in reply to: Jon.Wilde

I ran it with the ISC on but Auto convergence off. Looks the same as before, it ran 10,000 iterations but prettty mucgh everything leveled off around 5,000.

Message 6 of 17
Jon.Wilde
in reply to: andrew.lesiecki

Hi Andrew,

 

Would you be able to attach the CFZ (support) file?

Also an image would be cool, for anyone else to see.

 

Thanks,

Jon

Message 7 of 17

Attached is the support file and an image of the result (velocity).  If any other files or images would be helpful let me know.

 

The quick responses are greatly appreciated!

Message 8 of 17
Jon.Wilde
in reply to: andrew.lesiecki

Hi Andrew,

 

So the issue we think we have is that the flow is not remaining attached beneath the structure towards the outlet, correct? It might just be that we are not accouting for something with this 2D analysis but let me have look and see. It does seem strange that it works OK in 3D but not in 2D.

 

Kind regards,

Jon

Message 9 of 17
Jon.Wilde
in reply to: Jon.Wilde

Hi Andrew,

 

Running this here I notice that the mesh is pretty coarse towards the outlet, where we also want to be capturing what is occurring.

 

Outlet Mesh.png

 

It is also wise to avoid any recirculation over the outlet boundary. Extending this here would be sensible.

 

Kind regards,

Jon

Message 10 of 17

What would a proper mesh be in that region? My process has been using the Automesh and then adding regions where I feel it is most needed while trying to keep it reasonable so my computer can still handle it.

 

Same question with the length, I have read it should be as much as 10-20 times the length of the part, but I tried one that long and it didn't seem to help (which very well could be the mesh is not fine enough), so I went back to the shorter outlet to save on elements.

 

P.S. In no way am I trying to argue that what your saying is incorrect just explaining what I have tried. I am open to try anything that is why i put my question on here.

 

Thanks,

Andrew

Message 11 of 17

The bulk of this will be due to meshing differences between 2D and 3D.

 

You might not have a simliar mesh quality between the two runs.

 

Taking your 2D file and assigning a more consistent mesh (as Jon was referring to) throught he domain and towards the outlet that he highlighted, you can see that the run on my end does maintain attachment much better than the image youhad posted

 

Also, the images you posted between 2D and 3D were not apples to appels as in 3D you were using Traces to look at the flow pattern. I would add a Plane in the 3D model such that you are slicing the geometry down the centerline and then compare flow patterns.

 

Velocity.png

Message 12 of 17

Thank you Jon and Apolo,

 

I added a plane down the middle of my 3D and I see what you are saying about comparing the two.

Could you attach a CFZ file so I could get a better idea of proper meshing throughout the whole box in 2D?

 

Sorry for the two question post, but is the ground effect (well lack of) in the 3D a result of insufficient mesh as well? I have attached the CSV file of the 3D I took screen shots of.

 

-Andrew

Message 13 of 17

Essentially all i did was to use your largest mesh refinement region and extend it all the way back to the outlet.

I did not use your smaller 2 regions (and removed them)

 

When comparing 2D vs 3D it is possible at times that your 3D model was not mesh independent and therefore you were seeing some mesh influence in to the solution itself. It is much easier to get a better quality mesh in 2D than 3D at times, which is why many people leverage 2D before going to 3D. And even then sometimes will run a 1/2 Symmetry 3D model to save elements and foxus them where they are needed

Message 14 of 17

So in the 3D would I be better off doing the 1/2 scale and also just using one mesh region all the way back? Or still add an additional region in the ground effect area?

Message 15 of 17

1/2 Symmetry is always a good time saver.

 

As far as the mesh regions, you can use multiple if you like, but at the end of the day you want to have a similar mesh quality between the two.

 What i mean by that is if you have ~5elements from the ground plane to the floor of the car in 2D we would want a similar mesh quality in 3D to be able to get similar fidelity of results.

This can be difficult in 3D as the mesh sizes can easily grow in to millions of elements so people will make compromises and minimize the amount of mesh in non-critical areas (for example the region towards the ceiling of the domain).

 

Apolo

Message 16 of 17

Andrew,

If you are going to compare results you must maintain some minimum level of consistency between the two models.

 

Taking a small look at your 3D geometry shows that not only are you not using the same profile between 2D and 3D but you are also operating at different ground clearances between the two.

 

Take a look at the image:

in 3D i'm calling out the features that do not exist in the 2D model as the 3D version has a sharp angle in the under-tray

And the lowest point is roughly 0.3ft off the moving ground

 

Compare that with the 2D image that has a number of bends as it goes to the diffuser section and that its lowest section is roughly 0.2ft off the ground.

 

As I called out previously, once you get the geometry the same, from there its a matter of matching mesh quality and ensuring we are running this out to convergence.

2D.png

 

3D.png

Message 17 of 17

Apolo,

 

The difference in geometry was from my countless iterations of trying to see what I wanted to. The 3D is the actual drawing of what was on the vehicle. The 2D radius was something I added trying to keep the flow attached in the 2D CFD, which come to find out was not the problem. The difference in height I believe was just a mistake on my part.

 

You have answered my question, the solution is that with my computing power I am unable to compare my 2D and 3D directly to each other. I can not run the same amount of mesh in my 3D, even using a half scale, because of that I am unable to see ground effect in 3D. I am currently running all my design changes in 2D like recommended.

 

 

Thank you and the rest of the Autodesk team for your help!

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report