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

Thought of turbulence model used in automotive

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

Like Tree1Likes
  • 1 Post By Ravindra Shende

Reply
 
LinkBack Thread Tools Display Modes
Old   November 24, 2017, 04:34
Default Thought of turbulence model used in automotive
  #1
Member
 
Join Date: Nov 2014
Posts: 61
Rep Power: 6
hokhay is on a distinguished road
Hi,

I am working in an electric sport car company as a CFD engineer. My job is to analysis drag and lift of our car under different configurations. Currently, I am using OpenFOAM for this jobs.

The numerical setup for the simulations are as follow:
Turbulence model: k-OmegaSST
Gradient scheme: cellLimited leastSquares 1
Divergence scheme (U): linearUpwind
Divergence scheme (others): upwind
Cell number: 40~60 millions
Average y+: 20~30

We have recently consulted with a aerodynamic professor who has worked in the automotive industry for more than 30 years. He has some comments on my CFD settings.

His first comment is to use k-Epsilon or SA model instead of K-Omega model. The second comment is y+ should be 1~5. These two suggestions seem to be counter-intuitive to me, especially the first one. In my understanding, k-Epsilon and SA are the worst turbulence model that would have been picked for vehicle simulation. They are well known for under predicting separation at the rear window which will result in under estimate drag and lift. The second comment is more of a practical reason rather than a technical one. It is almost impossible to achieve such small y+ in real car simulations.

Could you guys give me comment on this topic whether you agree on the professor comment or not please? I am a bit confuse.

Thank you very much
Jason
hokhay is offline   Reply With Quote

Old   November 24, 2017, 10:26
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 4,309
Rep Power: 46
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
I think that try to evaluate the viscous drag by using the first cell at y+=20 is the main reason for the negative comments you received.
This way you have to work with wall-modelled BC.s, that is you are somehow already prescribing the drag as a BC instead of trying evaluating it by the solution.
FMDenaro is offline   Reply With Quote

Old   November 24, 2017, 13:36
Default
  #3
Member
 
Join Date: Nov 2014
Posts: 61
Rep Power: 6
hokhay is on a distinguished road
Thanks for your reply. If I am not getting you, you mean y+ 20 is too large to solve the boundary layer, right? If that is the case then I have another question. Is the wall shear stress or viscous drag important to a bluff body like a car? What is the typical viscous drag value? I have calculated the viscous drag of our car at 30m/s and the value is just less than 20N when using wall model. Is this value sounds reasonable?
hokhay is offline   Reply With Quote

Old   November 24, 2017, 14:09
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 4,309
Rep Power: 46
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by hokhay View Post
Thanks for your reply. If I am not getting you, you mean y+ 20 is too large to solve the boundary layer, right? If that is the case then I have another question. Is the wall shear stress or viscous drag important to a bluff body like a car? What is the typical viscous drag value? I have calculated the viscous drag of our car at 30m/s and the value is just less than 20N when using wall model. Is this value sounds reasonable?
Yes, it is to large to compute the stresses at the wall accurately and for this reason one adopts some wall-modelled BC instead of using the no-slip condition. However, that introduces a model on to the drag evaluation.
FMDenaro is offline   Reply With Quote

Old   December 6, 2017, 00:17
Default
  #5
Member
 
Join Date: Nov 2014
Posts: 61
Rep Power: 6
hokhay is on a distinguished road
Thanks very much for your advice Filippo. Is there any comment on the turbulence model or numerical scheme too?
hokhay is offline   Reply With Quote

Old   December 6, 2017, 02:38
Default
  #6
Member
 
Ravindra Shende
Join Date: Feb 2011
Location: Pune, India
Posts: 45
Rep Power: 9
Ravindra Shende is on a distinguished road
Hi hokhay,

Your mesh size is too large and still you are not able to achieve the y+ values needed by the k-omega SST model (between 1 and 5). This means the viscous drag is not correctly predicted and may be the separation point also.

If you wish to continue using this model then you will have to increase your mesh size, which will make your simulations more expensive.

Using the k-epsilon model with wall functions you will get results of similar quality and you might get some margin to reduce the mesh size.

PS: The SA model also requires wall y+ between 1 and 5.
hokhay likes this.
Ravindra Shende is offline   Reply With Quote

Old   December 6, 2017, 22:45
Default
  #7
Member
 
Join Date: Nov 2014
Posts: 61
Rep Power: 6
hokhay is on a distinguished road
Thanks a lot for your reply, Ravindra. I also feel strange to I still cannot achieve smaller y+ with such mesh size. Some researchers can achieve y+<1 even with 20M cells on a DriVaer model at the same speed as mine. My first mesh is at 510-4m from the wall. If I goto y+=1, the first cell will be 510-5m which seems unreasonably small. This makes me confusing of the definition of y+. Actually the y+ various from 0.001 to 98 on the whole car and the average y+ is 19. In this case, should I say my case has a y+ of 19?

Regarding to the turbulence model, from your explanation, the k-Omega SST advantage of better separation prediction does not hold if y+>5? Will it still better then k-Epsilon when both using wall function at the buffer zone, y+=19?

Thanks very much
hokhay is offline   Reply With Quote

Old   December 7, 2017, 10:56
Default
  #8
Member
 
Ravindra Shende
Join Date: Feb 2011
Location: Pune, India
Posts: 45
Rep Power: 9
Ravindra Shende is on a distinguished road
Hi hokhay,

I gather that you have maintained first cell height of 0.5 mm everywhere on the surface of your car and with that you are getting wall y+ in the range of 0.001 to 98.

In that case, instead of talking about average y+, you should say that the velocity gradients and hence the friction force is correctly predicted in the regions where the y+ is less than 5 and incorrectly elsewhere.

About the mesh, fine mesh is required only in the boundary layer and wake regions. Elsewhere the mesh can be coarse since the flow is essentially inviscid there. If you have already done this then you can increase surface mesh size in the regions where y+ is less than 1 and use higher first cell heights in these regions. This will be a very tedious and time consuming task.

From an engineering perspective, I would suggest you to do the following.
In your simulations with k-omega SST model, check the wall y+ values in the vicinity of the separation point. If y+ is below 5 for some distance ahead, at and after the separation point then you can safely say that the separation point and hence the total drag is predicted fairly accurately. If not then try to achieve y+ < 5 in that region. The total drag will still have some error due to wrong prediction of the skin friction drag but, as you correctly said in one of your previous posts, it does not contribute significantly to the total drag of a bluff body like a car.
Ravindra Shende is offline   Reply With Quote

Old   December 7, 2017, 15:25
Default
  #9
New Member
 
Arnie
Join Date: Mar 2017
Posts: 4
Rep Power: 3
arnie333 is on a distinguished road
Hockhay,

Are you also considering the aspect ratio of your inflation layer (prism) cells ?

You have to realise that by increasing their aspect ratio, you can decrease the number of cells in your model ! Obviously, the aspect ratio needs to be within acceptable limits and you need to investigate this a little more.

My limited knowledge leads me to understand that the aspect ratio can be quite large as long as the flow is parallel to the long edge of the cell.

Furthermore, increasing cell size sufficiently downstream and upstream from the area of interest also helps to reduce number of cells.

This way, you can use the k-w SST solver with Y+ ~1 on a DrivAer model with less than 10M nodes.

PS. If you want to use k-e turbulence model, then a Y+ from 60 and 300 is ideal.

Regards
arnie333 is offline   Reply With Quote

Old   December 11, 2017, 00:56
Default
  #10
Member
 
Join Date: Nov 2014
Posts: 61
Rep Power: 6
hokhay is on a distinguished road
Thanks for your reply Ravindra and Arnie. I got it now, so make sure y+<5 at critical region.
Arnie, the high aspect ratio and the small area are the main difficulties I am facing when making the boundary layer mesh. I am using SnappyHexMesh for meshing. I am only able to get a nice mesh for the first cell height of 0.1mm, equivalent to y+=8. Further reduce the height will result a collapse of the mesh because of bad mesh quality, otherwise I will need to reduce the mesh size further more.

P.S. Which meshing software you guys use?
hokhay is offline   Reply With Quote

Old   December 11, 2017, 12:18
Default
  #11
Member
 
Ravindra Shende
Join Date: Feb 2011
Location: Pune, India
Posts: 45
Rep Power: 9
Ravindra Shende is on a distinguished road
Glad to know that I was able to help. Good luck for your project.

PS: I use ICEM CFD for meshing. It allows one to set different first cell heights of prism cells over different surfaces of the car.
Ravindra Shende 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
Wrong multiphase flow at rotating interface Sanyo CFX 14 February 7, 2017 18:19
Question about matching of solver and turbulence model louistse OpenFOAM Running, Solving & CFD 1 February 1, 2017 22:36
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 07:20
Error in Two phase (condensation) modeling adilsyyed CFX 15 June 24, 2015 20:42
Overflow Error in Multiphase Modelling with Two Continuous Fluids ashtonJ CFX 6 August 11, 2014 15:32


All times are GMT -4. The time now is 07:43.