
[Sponsors] 
January 5, 2018, 13:27 
yplus value openfoam turbulent analysis

#1 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
Learning CFD analysis through tutorials and came across this problem:
I am performing a pipe ( radius = 0.07m) flow analysis with Reynolds number >9500 using OpenFOAM. To find the best mesh configuration, I am using the results of yplus. i calculated yplus value using equation and for a y=5mm i get a yplus=3.18 I am increasing the cells near the wall and correspondingly observing the yplus values. when i plot a yplus vs length of the pipe graph i get the following plots for different mesh configuration. yplus.png yplus plots Interestingly 1) the graph gets stabilized and falls back to zero in both the cases. what can be the reason ? 2) with few cells i get more yplus value. why is this. What value of yplus i should be looking at for kepsilon model. 

January 5, 2018, 14:24 

#2 
Senior Member
Join Date: Dec 2017
Posts: 153
Rep Power: 8 
Hi,
In order to calculate the yplus you should know the value of the friction velocity for your pipe flow (in your case i think you can use some existing correlation for the friction coef to exitimate the wall friction). How do you calculate the quantity in your plots? If you use a rans/ urans approach with wall function, then yplus should be larger than 30. If you would like to simulate the boundary layer, then you should know that you will found it at yplus<5 so much more resolution is required. 

January 5, 2018, 17:34 

#3 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
I calculated yplus analytically using the formula : density *friction velocity*y/dynamic viscosity. At y=5mm i am getting yplus as 3.18.
I am using Kepsilon wall function ... values for plot ( yplus) are obtained from yplusRAS utility in openfoam after running the simulation. To get 30 as yplus i need to look at y=3cm from the wall which is more than the boundary layer thickness ( 7.86mm). Then in such a case will i not miss the flow properties near the wall ? 

January 5, 2018, 20:00 

#4  
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,680
Rep Power: 66 
Quote:
A y+ of 30 is still well within the BL (it's just outside the viscous sublayer and roughly 3% of the BL thickness). There's no way you can be at 3cm, which is much more than the BL thickness of 7.86mm and get a y+ of 30. Your y+ would be in the tenthousands at 3cm. If you tell me your BL thickness is 7.86 mm, then I would roughly guess that y+ of 30 is at .02 mm or near that order of magnitude. 

January 5, 2018, 20:09 

#5 
Senior Member
Join Date: Dec 2017
Posts: 153
Rep Power: 8 
No, the wall function is used to model the boundary layer region which for high Re flows requires a huge resolution (e. g kim moin moser 1987 performed dns of a channel flow at Re=2800 and their yplus was 0.05 with 4 million mesh points)... So if you use the wall function, your first mesh point has to be located far enougth the viscous sublayer and yplus=30 is a standard choice.


January 5, 2018, 20:23 

#6 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
I am calculating yplus as :
WhatsApp Image 20180106 at 1.19.55 AM.jpg I am using yplusras utility in openfoam to generate yplus data. As i am refining mesh near the wall the yplus gets small. It went to 0.5 too. I never crossed the value of 2.5 till now. Where do you think i am going wrong. Thanks for the support 

January 5, 2018, 20:33 

#7 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
But i read that to obtain accurate flow properties the first mesh point should be within the viscous sublayer and yplus value should be less. Isnt it so ?


January 6, 2018, 03:41 

#8  
Senior Member
Join Date: Dec 2017
Posts: 153
Rep Power: 8 
Quote:
Yes it is, if you do not use the wall function. However, as pointed out in the previous posts, the wall function model the viscous sublayer itself and you do not need resolution there. If you do not use it, then you must put points within the viscous sublayer. Regarding your plots, they look strange to me. Since both utau and viscosity are constant, then they should scale directly with the wall distance... 

January 6, 2018, 10:37 

#9 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
Using analytical formula i am getting very less yplus value at y=2mm . Why is that .
Moreover why is the yplus plot decreasing back to zero after becoming steady. Any ideas ?? 

January 6, 2018, 10:59 

#10 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,782
Rep Power: 71 
y+=u_tau*y/ni is just a local Reynolds number measured from the position y=0 at the wall. The key is in the value u_tau=sqrt(tau_wall/rho). You need to compute tau_wall from the final numerical solution


January 6, 2018, 11:08 

#11 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
but i get a yplus value generated after the last simulation from openfoam and i plotted the graph yplus vs Length of pipe . you can see them in the above posts.


January 6, 2018, 11:12 

#12 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
i get yplus value generated after the simulation from openfoam and it is around 2.5  0.7. When i increase the mesh near the wall the yplus value still decreases.


January 6, 2018, 12:43 

#13 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,782
Rep Power: 71 
Yes, what you can plot along the streamwise direction is the values y+(h_first_cell). That gives the grid resolution in terms of the BL quantities. You need a value lesser than 1 for a resolving BL (actually, 34 cells within y+=1).
However, u_tau depends on the solution so that when you compute it from a coarse grid or a finer grid, the value can change. Check the way in which u_tau is computed in OF. 

January 6, 2018, 13:11 

#14 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
Okay so is it okay to have yplus around 0.7 . can i treat the mesh as good one ?


January 6, 2018, 13:21 

#15 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,782
Rep Power: 71 
well, as I wrote, if you want to resolve the BL you need that at least 34 cells are within y+=1. If your first point is at 0.7, I suppose you get higher values for the next points layers That depends on your stretching law.


January 6, 2018, 13:28 

#16 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
I read that having yplus>=30 is considered a good mesh. Currently i have a yplus=0.7 how do i get yplus>30 because when i refine the mesh the yplus is still decreasing to lower values .
One more thing as i increase the stretching factor yplus value will go up right ? Last edited by massakimi; January 6, 2018 at 13:30. Reason: added comments 

January 6, 2018, 13:31 

#17  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,782
Rep Power: 71 
Quote:
This is a totally different issue! if you have the first point at y+>30 you do not resolve the BL! Therefore, you need special modelling at the wall, a fact that is implemented only in some turbulence models. I suggest to read the basics of that in the book of Wilcox 

January 6, 2018, 14:04 

#18 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
Okay. Thanks a lot for all the answers


January 6, 2018, 15:18 

#19 
New Member
Arjun
Join Date: Feb 2014
Posts: 20
Rep Power: 12 
Please make this clear .
If i choose kepsilon model and wall fucntion approach i need not add more meshing near the wall of the pipe. ( less cells in wall normal direction ). But if i do not use wall function approach like in other turbulence models then i need to refine the mesh near the walls ( more cells in wall normal direction ). Am i right ?? 

January 6, 2018, 15:33 

#20  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,782
Rep Power: 71 
Quote:
yes, correct 

Tags 
openfoam 2.0.1, pipeflow, turbulent boundary layer, yplusras 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
modeling a turbulent flow over an obstacle using OpenFOAM  Daniel_Khazaei  OpenFOAM Running, Solving & CFD  2  June 4, 2020 05:21 
Problem with divergence  TDK  FLUENT  13  December 14, 2018 06:00 
OpenFOAM v3.0.1 Training, London, Houston, Berlin, JanMar 2016  cfd.direct  OpenFOAM Announcements from Other Sources  0  January 5, 2016 03:18 
OpenFOAM Training, London, Chicago, Munich, SepOct 2015  cfd.direct  OpenFOAM Announcements from Other Sources  2  August 31, 2015 13:36 
implementation of the technique for turbulent flows DES in openFOAM  Ferdinand  OpenFOAM Running, Solving & CFD  1  July 20, 2015 19:11 