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

y+ for given turbulence model

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

Like Tree4Likes
  • 2 Post By ghorrocks
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   May 16, 2017, 19:17
Default y+ for given turbulence model
  #1
Member
 
Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 85
Rep Power: 3
frossi is on a distinguished road
Hi,

I am trying to solve flow over a 3D wing and struggling to find the right turbulence model.

I am finding the right height of my first inflation layer using this link:
https://www.computationalfluiddynami...t-cell-height/

1) What is y+? I know it's a non dimensional distance, but it would be awesome if someone could give a more detailed explanation. What does y+ correspond to exactly?

2) Since I am using a 3D geometry and Re = 1,000,000 I think I do not need to solve the viscous and buffer layers (would require to many elements). So I want a y+ >1 to solve for the log law layer. So, since I won't solve for the viscous and buffer sublayers, I will need wall functions. Is my reasoning right so far?

3) Since I need wall functions, I chose realizable k-epsilon model. With this model, what should be my target y+? I researched and I saw that it needs to be 30<y+<60. But other sources says between 30 and 200. I am confused on which value I should aim for. Or should I use another turbulence model? I am looking for quick convergence.

4) Is it wrong if I use Spalart-allmaras? Since this model doesn't have wall functions, it looks to me like i can never use it. What's its purpose then? But when I researched, I found this:
Spalart-Allmaras:
Economical for large meshes. Performs poorly for 3D flows, free shear flows, flows with strong separation. Suitable for mildly complex (quasi-2D) external/internal flows and boundary layer flows under pressure gradient (e.g. airfoils, wings, airplane fuselages, missiles, ship hulls).

So should I use spalart-allmaras? but if it doesnt have wall functions, do I even need to consider the y+ with this turbulence model?

5) How do I check Y+ after i run my simulation? I was told to use CFD post and plot it, but I dont understand how to plot it, since i always received vague instructions. I really dont know where to look. Could someone please list the steps to plot y+?



Thank you so much everybody.
frossi is offline   Reply With Quote

Old   May 16, 2017, 22:07
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,639
Rep Power: 105
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
1) y+ gives you a position in the usual turbulent boundary layer profile for the first node. So it is a normalised position in the turbulent boundary layer profile.

2) You are probably correct. Friction is well predicted by wall functions in many cases. Heat transfer less so, and separations can be problematic. If turbulence transition is important then you must use y+ = ~1.

3) y+ between 11 and about 100 is normal, but you should find out for your case by a mesh sensitivity study.

4) Your quote looks like a good summary of the models benefits and deficiencies. So as long as your airfoil is in the normal operating range (ie not stalled) then it should be close. But why not check a few models and see how they go against each other?

5) CFD-Post has y+ as an available variable by default. Have a look under the puzzlingly labelld "..." button. Note that y+ only exists on surfaces, not the volume mesh, so only plot it on wall boundary surfaces.
frossi and AnnaF like this.
ghorrocks is offline   Reply With Quote

Old   May 17, 2017, 15:22
Default
  #3
Member
 
Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 85
Rep Power: 3
frossi is on a distinguished road
got it, thank you so much!
I was finally able to plot y+! (see picture)


Now, as I said before I wanna stay out of the viscous and buffer layer, and just focus on the log-law layer. So I aim at a y+ between 80 and 60.

1) In the graph you can see the y+ values for both surfaces of the wing (top and bottom surfaces). As you can see from the graph, I get regions where the y+ is too low (leading and trailing edge) and goes into the buffer layer (y+ around 10). At the same time, these places in which the y+ is too low have very short x-distances (less than 0.025 m at the leading edge). Are these low y+ regions a problem? Or they aren't, since they appear over a very short distance? But since the leading edge is very important part for the wing, should i try to get my ideal y+ there as well?

2) I am using Spalart-Allmaras model. But I saw that this model doesn't use wall functions. So how can it be a good model if it doesn't use wall function? I thought that the goal of wall functions was to approximate the viscous and buffer layers that would otherwise be ignored by a large y+ choice. Could you please clarify this?

3) I saw that enhanced wall treatment means that wall functions are used in the right way regardless of the y+ value i use. Is this true? Also, if it's true, how can i tell if the turbulence model has enhanced wall treatment? I can't see any option that mentions this in the pre-solver set up. Or Spalart-Allmaras and the other models are all enhanced by default?


Thank you
Attached Images
File Type: png 1.PNG (51.1 KB, 19 views)

Last edited by frossi; May 17, 2017 at 18:07.
frossi is offline   Reply With Quote

Old   May 17, 2017, 21:12
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,639
Rep Power: 105
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
Now, as I said before I wanna stay out of the viscous and buffer layer, and just focus on the log-law layer. So I aim at a y+ between 80 and 60.
No, this is not the usual approach. Wall functions are designed to work from y+= ~11. So they should be fine from 11 upwards. The upper limit is determined by mesh resolution. So your target should be above 11, and below whatever limit a mesh sensitivity check tells you is needed for good boundary layer accuracy.

Quote:
Are these low y+ regions a problem?
Yes and no. At separations, flow reversals and leading/trailing edges y+ goes to zero. This means the wall function approach is not valid in these regions as it is not possible to get y+>11. But if these regions are a small proportion of your flow then overall accuracy will not suffer too much and it is fine. If they are a significant proportion of the flow you could consider remeshing, but more likely it is suggesting that wall functions are not a good approach in that simulation.

Quote:
So how can it be a good model if it doesn't use wall function?
S-A does not attempt to model the boundary layer. If the detailed structure of the boundary layer is not important then S-A is fine. If it is then S-A is not an appropriate turbulence model.

Quote:
I saw that enhanced wall treatment means that wall functions are used in the right way regardless of the y+ value i use.
There are two approaches used here if I recall (it has been a while since I looked into this in detail):
1) Enhanced wall functions put the first node at around y+=11 regardless of where it actually is. In effect this just assumes that there is the boundary layer below it to give y+=11, regardless of what the distance below it actually is. This has the effect of mimicing if the wall boundary was a little closer or further away than it actually is. As long as this variation is small the error is minimal.

2) Automatic wall functions on k-w and SST turbulence models automatically transition from wall functions when y+>11 to integration to the wall when y+<11. So this approach is very nice with few simplifying assumptions. It is quite a general approach (and is a key reason why I recommend the SST turbulence model as the default turbulence model).
frossi likes this.
ghorrocks is offline   Reply With Quote

Old   May 17, 2017, 21:30
Default
  #5
Member
 
Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 85
Rep Power: 3
frossi is on a distinguished road
Ok, thank you. I have one last point where I am confused:


Quote:
Originally Posted by ghorrocks View Post
S-A does not attempt to model the boundary layer. If the detailed structure of the boundary layer is not important then S-A is fine. If it is then S-A is not an appropriate turbulence model.
So what I understand from this is that S-A doesn't solve the boundary layer because it doesn't have wall functions.
1) So from where does S-A start analyzing the physics? Does it start from the log-law layer, or it doesn't even take this part into account and it completely skips the boundary layer as a whole?
2) At this point my question is: if S-A completely skips the boundary layer, how can it be widely used for aerospace applications? It would mean that boundary layer effects on aircraft wings are totally overlooked?
3) If S-A doesn't have wall functions, then I can use the S-A model with any value of y+ that is >0?
frossi is offline   Reply With Quote

Old   May 17, 2017, 21:35
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,639
Rep Power: 105
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
These questions are getting beyond my knowledge of S-A.

I think I will have to refer you to https://en.wikipedia.org/wiki/Spalar...rbulence_model

And even better, a turbulence modelling textbook like "Turbulence Modelling for CFD" by Wilcox.
frossi likes this.
ghorrocks is offline   Reply With Quote

Old   May 17, 2017, 21:41
Default
  #7
Member
 
Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 85
Rep Power: 3
frossi is on a distinguished road
Thank you so much,

your comments were extremely helpful.




Best regards.
frossi 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
Question about matching of solver and turbulence model louistse OpenFOAM Running, Solving & CFD 1 February 1, 2017 22:36
Error in Two phase (condensation) modeling adilsyyed CFX 15 June 24, 2015 19:42
Overflow Error in Multiphase Modelling with Two Continuous Fluids ashtonJ CFX 6 August 11, 2014 14:32
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
Wrong calculation of nut in the kOmegaSST turbulence model FelixL OpenFOAM Bugs 27 March 27, 2012 09:02


All times are GMT -4. The time now is 18:04.