Can someone explain the Y plus value
 

I am a third year engineering student at university currently involved in CFD modeling. could sombody please explain to me the nature of the Y+ value ie. how it is calculated and what it's significance is.

Re: Can someone explain the Y plus value
 

Jeff,

y+ is a non-dimensional distance. It is often used to describe how coarse or fine a mesh is for a particular flow pattern. It is important in turbulence modeling to determine the proper size of the cells near domain walls. The turbulence model wall laws have restrictions on the y+ value at the wall. For instance, the standard K-epsilon model requires a wall y+ value between approximatly 300 and 100. A faster flow near the wall will produce higher values of y+, so the grid size near the wall must be reduced.

The definition of y+ for the K-e model is:

y+ = (((density^2 * Cmu^(1/2) * K)^(1/2))/viscosity) * (distance from wall)

where Cmu is the constant 0.09 and K is the kinetic energy.

If you are interested, I have a study of the effect of y+ on wall heat transfer for various turbulence models in my thesis, at http://bgtibm1.me.uiuc.edu/people/d-...sdownload.html

David Creech CFD Literature CFX User Subroutine Archive

Re: Can someone explain the Y plus value
 

(1). Take a look at the book"Boundary Layer Theory", by Schlichting, McGraw Hill Company. (2). In short, Y+ is a non-dimensional distance derived from Y.

Re: Can someone explain the Y plus value
 

That definition is really for y*, y+ is defined as:

y+ = rho * u* * y / my

where

rho = density, u* = friction velocity, y = distance from wall, my = dynamic viscosity,

y+ and y* are the same in eqilibrium turbulent boundary layers though.

Re: Can someone explain the Y plus value
 

Jeff,

There are two ways of looking at many CFD issues, one from a technical viewpoint or that of a user. The replies I have so far seen are technicl, here is a user viewpoint on Y+.

Y+ is a ratio between turbulent and laminar influences in a cell, if Y+ is big then the cell is turbulent, if it is small it is laminar. The importance in many cases of this concerns wall functions which assume that the laminar sub-layer is within the first cell, if Y+ is small then the cell is totally laminar and the next cell in has some laminar flow in it, the wall functions are not applied to this cell and you make bad modelling assumptions. If Y+ is too big then you are not so bad with the laminar/turb problem but other assumptions are invalidated.

Philip

Re: Can someone explain the Y plus value
 

Well, since this a CFD forum I suppose it's natural that the responses have all been with regards to CFD. However, the origin of y+ arises from solving the boundary layer equations for turbulent flow using matched asymptotic expansions (a method lamentably not taught much these days). In this method, as the others have pointed out, the independent variable is scaled (nondimensionalized) with quantities which dominate the local physics. In the case of y+, it is a scaled y-coordinate in the layer closest to the wall. The boundary layer velocity profile turns out to be linear with y+ in this innermost layer until y+ reaches some matching value with the next layer. Similar criteria is used in the CFD community to select grid point spacing nearest the wall. Hope that helps.

Re: Can someone explain the Y plus value
 

the definition of jonas is correct, but now lets go on: u*=tau_wall*y/mu. is y the first cell-center in the flow-field ? and what is tau_wall and how do you calculate tau_wall ?

Re: Can someone explain the Y plus value
 

(1). It is fairly straightford in finite difference grid. (2). y is the distance measured from the wall. If j=1 is the wall point, y=0 there. (3). For the wall shear stress, one needs another point to calculate the velocity gradient at the wall. In this case, use U(j=2) and y(j=2) to calculate the velocity gradient at the wall. The wall shear stress is equal to mu times the velocity gradient at the wall. (4). For the finite volume formulation, all I can say is it must be consistent with the finite volume approximation used. Sometimes, one can position the first cell center right on the wall. Then y=0, and U=0 at the wall point.

Re: Can someone explain the Y plus value
 

Is this also true for a boundary layer that is only resolved with wall-functions? With wall-functions you can't just use the molecular viscosity mu, can you?

Re: Can someone explain the Y plus value
 

(1). The reason behind using the wall function is the lack of mesh points near the wall. In other word, one is trying to save mesh points by using the wall function approach. (2). We will have to assume that the wall function is a one parameter familar of curves, and the unknown parameter is the wall shear stress (or v*). The function has two sections, near the wall it is linear, and away from the wall it is a log-function. (this definition can be found in Schlichting's Boundary Layer book). (3). Using the finite difference grid as an example, let j=1 is still the wall point, j=2 is the first point away from the wall, and j=3 is the second point away from the wall. If y(j=2) is about 5% of the boundary layer thinkness, then it will be roughly in the log-function region. If y(j=2) is much smaller than that value, it is likely that j=2 point will be in the linear function region. ( this will depend on the actual velocity profile. it is used here to illustrate the order of magnitude.) (4). Now, since we don't have mesh points between j=1 and j=2, there is no way one can compute the velocity profile in the region. But using the wall function approach, one can replace the actual calculation of the profile by a family of wall function curves. The only thing left to be done is to find that particular parameter value. (5). The only way to find that parameter value is through the use of the the velocity information at j=2 and j=3. So, U(j=3) and y(j=3) will be used to find the wall shear stress through the wall function at any time ( or iteration number) of calculation. Remember that j=3 is an interior point and U(j=3) is computed result. (6). With the wall stress determined, the value can be used to determine the new velocity boundary condition at j=2. (j=2 is the boundary condition location, since the region between j=1 and j=2 is not solved. There is a gap between j=1 and j=2.) The new U(j=2) will be used as the new boundary condition for the next iteration. (7). For finite volume approach, in staggered grid, with two-equation model, different approaches have been used. The wall shear stress can be related through other flow field parameters, such as k,...etc indirectly.

Re: Can someone explain the Y plus value
 

Hello Can you give some reference for the basic's of the method you said above. The one related to CFD will be most welcome Thankyou

Re: Can someone explain the Y plus value
 

(1). One final word about the wall function implementation, as long as you are in the non-separated flow region, the results will be reasonable regardless of how the wall stress is derived ( through the velocity profile alone or through the third party ,TKE (k) ). (2). But if you decide to compute the separated flow problem, I would recommand the use of a low Reynolds number model or a simple algebraic model where the whole flow field is covered. This is because it can be very confusing in the separation point region where the flow direction, the sign of the wall stress, and the validity of the wall function are all unknowns. Most published papers did not want to cover this area in details, most of the time, only the formula used are printed. (3). So, for separated flow problems, move on to the low Reynolds number models or the like.

Response to andimiller
 

tau_wall is the shear stress at the wall. This is normally part of the solution. However, depending on your geometry, this could perhaps be estimated with Blasius' solution assuming a flat plate. Try to find an analytical solution or some previous solution that is relevant to your configuration.

Hello David Creech
 

My name is Kiran,I am doing my Maters Thesis in CFD. I am doing CFD simulations on Heat exhangers, I am interested to see how prism layer meshes effect the heat transfer process.

I would like to read your thesis....The link provided by you doesn't work. Can you send me your thesis...Here is my mail id msvkirankumar@gmail.com


thanks in adv.


regards

kiran

The guy you are replying to posted more than 12 years ago. He probably has long forgot about this thread.

y plusssss
 

I have two question related to Y plus.

1- I am trying to have y+<5 while using K-epsilon method (enhanced wall) in a 5 m pipe. My y+ results give a value of less than 5 but the earlier values are about 8 and then it downs to less than 3 severely. Is this ok or not? Y plus value must be less than 5 throughout the geometry wall?

2- My goal is to find pressure drop throughout a pipe. The amount of pressure drop changes with quality of mesh even for the Y plus value less than 5. For example for the y+=3 I have dp=3600 Pa and for y+=0.5 I have dp=3400 Pa. which one is true?
Thank you for your attention to my request

Y+
 

you can take Y+ as small as you want. it will increase the accuracy of your result but program take more time to converge due to more number of grid points...........

What is Y plus?
 

Hello David Creech
I am Manpreet. I am working on project entitled Flow analysis through Rotor 37. I have done meshing by following turbogrid tutorials. In that, does not mention any value for Yplus . It is using standard.Could you please let me know how to calculate Yplus in my case. In addition, I am trying to open link mentioned by you http://bgtibm1.me.uiuc.edu/people/d-...sdownload.html. It's not working showing error server not found. How do I access it.

Thanks and Regards
Manpreet Singh
manpreet_singh_er@yahoo.co.in

;3250]Jeff,

y+ is a non-dimensional distance. It is often used to describe how coarse or fine a mesh is for a particular flow pattern. It is important in turbulence modeling to determine the proper size of the cells near domain walls. The turbulence model wall laws have restrictions on the y+ value at the wall. For instance, the standard K-epsilon model requires a wall y+ value between approximatly 300 and 100. A faster flow near the wall will produce higher values of y+, so the grid size near the wall must be reduced.

The definition of y+ for the K-e model is:

y+ = (((density^2 * Cmu^(1/2) * K)^(1/2))/viscosity) * (distance from wall)

where Cmu is the constant 0.09 and K is the kinetic energy.

If you are interested, I have a study of the effect of y+ on wall heat transfer for various turbulence models in my thesis, at http://bgtibm1.me.uiuc.edu/people/d-...sdownload.html

David Creech CFD Literature CFX User Subroutine Archive[/QUOTE]

First Cell Size in case of laminar flows
 

Hello,

Though the applicability of Y+ is suited for turbulent BL flows what precautions in terms of first cell size should one take while modeling Laminar flows ?

We can estimate the first cell size height for turbulent flows employing turbulence models but what about the first cell size height in case of laminar flows? ....

Thanks

Hello everyone

I was wondering if there are any thumb rules for deciding the y+ value for the first grid point when standard wall function is used for k-e model. In my area of work, some have considered 30, 50 etc. For my particular case I was thinking of using a higher value of about 100 or even upto 200, otherwise the no of cells become too large even for structured mesh. But i am not able to arrive at any conclusion, not finding any deciding rules. Can anyone please help me out ? Till what extent of y+, the standard wall function takes care of, this is the prime issue. I am not interested in any near wall flow physics, so i would like to use as large a value for y+ as possible with a good soluton for bulk flow characteristics and heat transfer at the walls. The reynolds no is of the order of 10^6.

Thanks in advance
Saurav

if you need to evaluate heat transfer at the wall how can you say that you are not interested in the physics near the wall? Heat transfer at the wall depends on both the thermal and dynamical boundary layer

Thanks for the quick reply. Yes you are right. I misframed my statement. I do have to get proper behaviour of the momentum boundary layer as well in order to capture the thermal boundary layer. It is just that momentum B.L is not directly of my interest. Actually i am carrying out a heat transfer problem in a combustion furnace, which is near rectangular in shape, with air-fuel mixture coming into the furnace from small circular burners. And my purpose is to find the resutant heat transfer at some of the surfaces. Can you plese let me know about my query now ?

Honestly, I doubt you can accurately solve a heat transfer problem at walls without a necessary grid resolution for the boundary layers...Assume you have a decoupled problem, after you solve first the velocity field how can you accurately predict the heat transfer without any information for the velocity near the wall?
In other words, if you disregard the physics near the wall for the momentum, I consider you should simply disregard the details of the heat transfer at the wall (in some sense you have the counterpart of the wall model for the heat transfer)

Yes, the standard wall function also takes care for the solution of thermal boundary layer in the log-law region , just like for the momentum boundary layer. So that seems to work fine to help reduce grid resolution. But what I am worried about is that there must be some higher limit of yplus to which the wall function works. I want to know this limit of yplus.

I would only consider the model for y+<100

https://upload.wikimedia.org/wikiped...glish).svg.png

Yes, from that figure it does look like it would not be good to consider yplus more than 100, because wall function models upto the log law layer. Actually the departure from log layer and beginning of the outer layer depends on Re or more precisely the adverse pressure gradient. Higher it is, the outer layer begins sooner. It can be seen from a plot in the source mentioned below as well. For zero gradient (flat plate) or favourable pressure gradient, the log layer extends upto yplus of 1000, and the outer layer starts beyond that. But again, yes, a maximum value of 100 would be in the safer side.

https://www.euhit.org/infrastructure...nel/facilities

y+, y* and "Law of the Wall" - a comprehensive explanation
 

Y+, Y* and Law of the Wall: https://cfdisraelblog.wordpress.com/...w-of-the-wall/

estimation y +
 

I am a doctoral student at the university. currently I imply CFD modeling in fluent. I spent a year in the mesh , could you help me to choose the best mesh for (y plus) and (dy first cell no mesh) for a turbulent simulation with number of Re = 6000 to 100000 to calculate the constant (B) of the log law logaritmic profile.
Vx / (V *) = 2.5Ln (y / k) + B.
with roughness effect artificial
1. Please explain to me how chosen y +, how chosen turbulence model (k epsilon , k-w, scalable or enhanced RNG or standart ....)
2. Can i use the same mesh to calculate the shear stress and the logarithmic profile and constant B.

Why do you not discuss these issues with your tutor(s)? You need to learn not simply to do ...

if you have an answer tell me if not i don't need any recommendations

The answer is to study. This forum cannot substitute the role of the tutor of a PhD student. A lot of people think that they can write private email for any kind of help as well as they ask for somehow homework.
You do not need recomendation? Well, the answers is that I have some answers but I do not teach here.

Wow, Captain Politeness here, you are going to have a lot of help, especially considering that you also hijacked the thread

y+ in condensing flow
 

Hello everyone,

I am trying to model two-phase upstream flow inside the tube with condensation (film flowing down).

For my understanding there are two regions of shear stress that are of interest: wall - liquid and liquid film surface - 2ph flow.

In this case should I calculate two boundary layers, one considering liquid film velocity and another one considering 2ph flow velocity? Also, the thickens of the liquid film is to be evaluated during simulations, so second boundary layer (l. film surface - 2ph flow) location is not known.

What kind of approach would you suggest? Also, any references to helpful material would be appreciated.

(I am relative new in CFD and planning of using ANSYS CFX)

Thank you in advance. :)