
[Sponsors] 
May 16, 2017, 19:17 
y+ for given turbulence model

#1 
Member
Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 85
Rep Power: 3 
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...tcellheight/ 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 kepsilon 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 Spalartallmaras? 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: SpalartAllmaras: Economical for large meshes. Performs poorly for 3D flows, free shear flows, flows with strong separation. Suitable for mildly complex (quasi2D) external/internal flows and boundary layer flows under pressure gradient (e.g. airfoils, wings, airplane fuselages, missiles, ship hulls). So should I use spalartallmaras? 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. 

May 16, 2017, 22:07 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,639
Rep Power: 105 
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) CFDPost 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. 

May 17, 2017, 15:22 

#3 
Member
Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 85
Rep Power: 3 
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 loglaw 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 xdistances (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 SpalartAllmaras 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 presolver set up. Or SpalartAllmaras and the other models are all enhanced by default? Thank you Last edited by frossi; May 17, 2017 at 18:07. 

May 17, 2017, 21:12 

#4  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,639
Rep Power: 105 
Quote:
Quote:
Quote:
Quote:
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 kw 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). 

May 17, 2017, 21:30 

#5  
Member
Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 85
Rep Power: 3 
Ok, thank you. I have one last point where I am confused:
Quote:
1) So from where does SA start analyzing the physics? Does it start from the loglaw 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 SA 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 SA doesn't have wall functions, then I can use the SA model with any value of y+ that is >0? 

May 17, 2017, 21:35 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,639
Rep Power: 105 
These questions are getting beyond my knowledge of SA.
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. 

May 17, 2017, 21:41 

#7 
Member
Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 85
Rep Power: 3 
Thank you so much,
your comments were extremely helpful. Best regards. 

Thread Tools  
Display Modes  


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 