
[Sponsors] 
October 11, 2001, 09:22 
can any body explain the significance of Y+

#1 
Guest
Posts: n/a

hi friends
can anybody please explain the significance of Y+ in the fluent software, also, is there any ideal value for the Y+ to take into consideration during solution calculations. thanks in advance, madasu. 

October 11, 2001, 11:37 
Re: can any body explain the significance of Y+

#2 
Guest
Posts: n/a

Y+ is a parameter that allows FLUENT to choose the proper way of consider fluid  solid interference ( wall functions ) When you have a turbolent case, after some iterations check the y+ value on the walls : for y+ from 0 to 5 use Two side for y+ from 30 to 60 use wall standard function
for other values of y+ try to adapt the grid so to enter these intervals. I noter that for y+ > 15 wall standard still works. Bye Marc 

October 11, 2001, 12:06 
Re: can any body explain the significance of Y+

#3 
Guest
Posts: n/a

thank you mark,
i read some where that as close as the Y+ value is near to 30, the results are better. is it true? if i get a Y+ value other than 30 how can i bring the solution with a Y+ near to 30. will it give better results or not? thank you once again. 

October 11, 2001, 12:58 
Re: can any body explain the significance of Y+

#4 
Guest
Posts: n/a

Y+ is a dimensionless distance from a given surface.
It used to consider distances within most any boundary layer. If the flow is turbulent, there are 3 relations of y+ to condsider. Nearest the wall there is the laminar sublayer. There is also the log and buffer layer to consider. The near wall treatments have different algorithms/method of solution. Two layer zonal is more accurate when just considering the laminar sublayer(Y+ =< 5), but the other two near wall functions work better when y+ is in the log layer (Y+ is 30 to 60). The question you have to ask yourself is how important is it for you to model that boundary layer? If you are considering seperation of the boundary layer or even convective heat transfer, and the boundary layer is intricate in your analysis, then a finer near wall mesh is required with a smaller y+ value. Beware if you are using roughness height/constant you need to maintain Y+ that is in the log layer. I know my explanation is a bit jumpy, but I will come back and explain it better. In the meanwhile, the User manual explains y+ usage, and Kays and Crawford (convective heat and mass transfer) explain Y+, and the law of the wall. By the way, what problem are you considering? 

October 12, 2001, 11:15 
Re: can any body explain the significance of Y+

#5 
Guest
Posts: n/a

thank you chetan,
i am a new user of cfd as i have started to work on cfd for my masters thesis just one month back. i will describe what i am doing breifly, i am designing a simulation model for heat exchanger pipes through which the hot gases are passed. the flow is turbulent. i took the pipe as a periodic pipe with a specific length. i have used tri/tet mesh in gambit and imported the mesh in fluent. as i am still in a stage of learning basic knowledge of cfd in Fluent, i got to read about Y+ parameter. thats why, i wanted to understand the significance of Y+. i will try to go through the fluent manual and also various books available to me. but if you could please expain little bit more clearly i will be very thankful to you. 

October 15, 2001, 02:02 
Re: can any body explain the significance of Y+

#6 
Guest
Posts: n/a

I had the same probleme one year ago. Try to get the book from Versteeg. It explain the FVM very well.
An introduction to Computational Fluid Dynamics H K Versteeg & W Malalasekera Prentice Hall ISBN 0582218845 www.pearsoneduc.com Yours Armin 

October 15, 2001, 04:31 
Re: can any body explain the significance of Y+

#7 
Guest
Posts: n/a

thank you armin,
fortunately i brought the book specified by you from the library recently, i have`nt gone through it, but i`ll do it right now, once again thank you for your help. bye madasu. 

October 15, 2001, 14:21 
Re: can any body explain the significance of Y+

#8 
Guest
Posts: n/a

Hallo I want to mention a comment:
Y+ is a nonedimensional quantity which results from the dimensional analysis to describe the behaviour of the Boundary Layer. To perfoem dimensional analysis (DA) one can assume the following relation: U=U(y, rho, mue, Tau_w, epsilon). After performing the DA, we get three nondimensional numbers: U+, Y+ and epsilon+ and the appropriate relation to describe the behaviour in the BL is simply U+=F(y+, epsilon+) So physically, Y+ is a nonedimensional number or quantity which is appropriate to describe and ease the handling, and classification, of the BL rather than the velocity or... The complicated Equations can be get from any textbook! I hope to be able to help. Markus 

October 16, 2001, 02:27 
Stay Away From Commercial CFD Code in School

#9 
Guest
Posts: n/a

(1). Now you see that reason why I kept saying that "stay away from any commercial CFD codes when you are learning CFD at school". (2). You must know at least the boundary layer theory in turbulent flows, including experimental data, before you can understand the Y+. (3). You can only get more confused when trying to use a commercial CFD code at the same time, especially some of the methods are not properly implemented in some commercial codes.


October 16, 2001, 15:50 
Re: Stay Away From Commercial CFD Code in School

#10 
Guest
Posts: n/a

Good point John. Maybe thats where we should have started... with some basics.
Madasu, are you familiar with Boundary layer theory? As you know, due to the shearing effect of a wall, I.e. viscous forces, a boundary layer form along the wall. The velocity at the wall is 0 (assuming the wall does not move), and the velocity far from the wall is some value called the freestream velocity. Within the boundary layer, we move from 0 velocity to freestream velocity. In laminar flow, an easy to understand velocity profile exists in the boundary layer. > freestream velocity > > > > > > > > > wall above i drew a profile of how velocity changes in a lmainar boundary layer. But when the flow is turbulent your boundary layer may look something like this: > > > > > > > > > > This is not exactly how i might draw it by freehand, but the point is that we again see a parabolic shape close to the wall, this is actually a very small region called the laminar sublayer (it is typically much smaller than as drawn in my profile). Still in the boundary layer, but not touching the wall,we have a region where we can see momentum exchange in the boundary layer. In a turbulent flow, the relation of y+ to u+ are either y+ = u+ (near the wall), or outside the laminar sublayer we have a logarithmic relation between y+ and u+. You need to pick up a book and study this relation which will be understood to be law of the wall, and go through the math yourself to see what the significance is. Look at White's Viscous Fluid Flow, Schlicting's Boundary Layer Theory, and/or Kays and Crawford's Advanced Convective Heat and Mass Transfer. Then read throught the manual in regards to y+. 

October 16, 2001, 16:12 
Re: Stay Away From Commercial CFD Code in School

#11 
Guest
Posts: n/a

I guess the profiles i drew did not come out the way i intended... see those books i recommended.


October 16, 2001, 17:46 
Re: Stay Away From Commercial CFD Code in School

#12 
Guest
Posts: n/a

(1). I am glad to see your comments, I think, this is the type of forum we need for CFD. (2). We need to focus on the more fundamental part of fluid mechanics and numerical analysis. If we step into the commercial black box, right away, you will see all sorts of promotions, which have little effect in helping the readers.


October 16, 2001, 18:23 
Re: Stay Away From Commercial CFD Code in School

#13 
Guest
Posts: n/a

Thanks for compliment John.
We must all remember that CFD is only a semiaccurate tool for the study of physics of fluids and heat... I'll be back to add some more on the turbulent boundary layer, law of the wall, and y+. 

October 17, 2001, 03:56 
Re: Stay Away From Commercial CFD Code in School

#14 
Guest
Posts: n/a

I find it is great to disscuss such consepts and help us to understand the physicsical and numericsl aspects of the fluid mechanics.
I have a comment: there is NO LAMINAR sublayer!!!. This is not an appropriate nomenclature. This sublayer ist correctly named VISCOUS sublayer. It was observed, thet there are (turbulent) vortices within this layer. In this Layer, the viscous effects DOMINATE the inertia effects. I will involve once again later. THanks, Markus. 

October 17, 2001, 05:53 
Re: oh,great discussion is going on, thank you all

#15 
Guest
Posts: n/a

hi guys,
its really amaging and interesting to find such a great discussion going on in this thread, it really provides a great knowledge for beginers like me to follow such an active discussion on the fundamentals and laws of fluid dynamics. in fact, now i could get at least some basic idea of what and what is related with boundary layer theory and cfd principles. i need to say thanks to everybody who has participated in such a nice talk. also i hope to get knowledge on these concepts and try to answere the questions posted by others. i`ll do my best. its simply great, keep on going guys, thank you, madasu 

October 17, 2001, 11:38 
Re: Stay Away From Commercial CFD Code in School

#16 
Guest
Posts: n/a

I did not know that the viscous sublayer is not truly laminar, but this seems to be a common mistake in several books. Could you give me the reference of this study? If I restate this comment, I need to back it up.


October 17, 2001, 14:36 
Re: Stay Away From Commercial CFD Code in School

#17 
Guest
Posts: n/a

(1). Well, he is touching a very sensitive part of the near wall turbulence. (2). I think, this layer was originally named laminar sublayer. (3). It is valid to use that name, because as you see that the velocity profile is also U+ = Y+, which means the velocity profile is linear. (4). But experimental evidence shows that this layer is not absolutely laminar, and there are some turbulence activities initiated from the surface. I guess, that's the reason why "laminar" was dropped and was replaced by "viscous". (5). But since the boundary layer is everywhere viscous, the name of "viscous sublayer" really is not giving out more information when compared with "laminar sublayer". (6). So, we are facing this paradox. My personal interest lies in the fact that the velocity profile is linear in turbulent flows. Laminar flow can produce linear velocity profile like in simple shear flow. If the turbulent flow can also have linear velocity profile, then it is saying that, in some way, the laminar flow equation can also be used for turbulent flows as long as the viscosity is properly modelled.


October 17, 2001, 14:54 
Re: Stay Away From (Blackbox) Commercial CFD

#18 
Guest
Posts: n/a

Hallo,
John means that the MEANvelocty profil is linear in the viscous sublayer! This confuses as if the flow laminar and flows PARALLEL in layers parallel to the wall. Here are some litarature: Cantwell, B.J., Coles, D. and Dimotakis, P. "Structure and entrainment in the plane of symmetry", Journal of Flluid Mechanics, Vol. 87, 1978; pp. 641672. Javier Jimenez "The largest scales of turbulent wall flows", Center of turbulence research, Annual Research Briefs, 1998. Landhal, M. T. "On Sublayer Streaks," J. Fluid Mech. 212, 593614, 1990. Hope to help. Markus. 

October 17, 2001, 17:31 
Re: Stay Away From Commercial CFD Code in School

#19 
Guest
Posts: n/a

Hi John,
Funny, I have to completely agree with you on this. In fact I think I have also stated this on the Forum previously. There is no place in graduate school for a commericial CFD code, especially if you are trying to learn CFD. I think that CFD software can teach fluid dynamics and how to interpret what is happening from a physical standpoint, but you won't learn anything about numerics and how numerical treatments differ in their behaviour. When I graduated I had never even touched a commercial CFD code. People in my department would come ask me questions thinking I would have all the answers because I was working on "CFD". What the hell... I didn't write their software, call them. Now I am a flow solver developer for a CFD company. Go figure. Dan. 

October 17, 2001, 21:14 
Re: Stay Away From Commercial CFD Code in School

#20 
Guest
Posts: n/a

(1). It is all right to write codes. (2). It is all right to write commercial codes. (3). It is all right to sell commercial codes. Well, when you start selling the code, it becomes commercial. (4). But a code in the computer system, regardless of the size of the company, regardless of the reputation of the company, is not going to jump out and hand over the right answer to the user. (5). The user has to know how to use a black box to get the right answer. And that is very challenging task for a student. On the top of it, most commercial codes are designed to make it harder for the user to break in. So, there are always the socalled "leftover bugs from the last generations". (6). Even in your case, working for a developer, I don't think you will be able to understand every bit of the code with the source code given.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
6DOF with floating body bounce back.  paka  FLUENT  4  June 6, 2013 11:32 
Remeshing a deformable solid body in a fluid  brashear  CFX  6  December 12, 2011 12:13 
Body in windtunnel  high preassure behind the body?  Andyjoe  OpenFOAM  4  February 16, 2010 11:57 
Body force at the cell face  Souviktor  Fluent UDF and Scheme Programming  0  March 31, 2009 08:54 
Inquiry, post results on airflow over auto body  Roland  CFX  1  July 1, 2006 14:16 