
[Sponsors] 
Is the solution trusted if Y plus is not located in the suggest value 

LinkBack  Thread Tools  Display Modes 
March 21, 2009, 23:57 
Is the solution acceptable if Y plus is not in the suggested range

#1 
Member
^_^
Join Date: Mar 2009
Posts: 36
Rep Power: 9 
Hi guys,
I am using keplson turbulence model with scale wall function in CFX. I can not figure out how to make sure the Y+ is 30~100 as suggested by CFX. My y+ is 1 ~106.8. How should I do with it? Is the solution ok or not? Thanks a lot Last edited by Jasmine; March 22, 2009 at 04:07. 

March 22, 2009, 18:10 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,403
Rep Power: 97 
Hi,
Do a mesh sensitivity study and work out whether the wonky y+ is affecting results. To do this generate a mesh with half and/or double the element edge length and see how much an important output parameter changes. Glenn Horrocks 

March 24, 2009, 12:12 

#3 
New Member
Join Date: Mar 2009
Posts: 9
Rep Power: 9 
Hi Jasmine,
The Y+ range is only a suggestion. Generally you need 5 to 15 nodes to be within the boundary layer in order to accurately predict the shear stress at the wall with a mesh expansion factor of 1.15 to 1.30. But the actual Y+ is Reynolds number dependant. If you have a very high Reynolds number, such as flow around a ship, a Y+ of greater than 1000 will suffice, whereas very low Reynolds numbers, such as a very small compressor blade, may require Y+ of 1 or 2. Special "Low Reynolds Number" turbulence models were developed for these applications because it was difficult to have 5 nodes within the boundary layer and a Y+ greater than 11 (the lower limit for wall functions). So, you can check visually to see whether you are capturing the boundary layer and also check, as Glenn suggested, that your solution is not affected by further refinement. CycLone 

March 24, 2009, 17:06 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,403
Rep Power: 97 
Hi,
To expand on my previous comment  I mean to say that the boundary layer is not important for all types of simulations. For instance if you want the lift from an airfoil running nicely and well away from separations your lift result will be within a few percent regardless of what you do with the boundary layer. The drag would need accurate boundary layer modelling but the lift would not. Glenn Horrocks 

March 24, 2009, 18:25 

#5 
Member
^_^
Join Date: Mar 2009
Posts: 36
Rep Power: 9 
Hi ghorrocks and CycLone,
Thanks you so much for your kindly explaination~ Jasmine 

April 3, 2009, 04:56 

#6 
New Member
Join Date: Apr 2009
Posts: 3
Rep Power: 9 
hello,
i am quite new to cfx. i want to simulate the flow around an airfoil, c=1600mm, v=2070m/s (so Re=1.87.8*10^6). now i am creating the mesh, wondering how big the first cell at the airfoil has to be. i read about this y+ value and found a calculator to calculate the first cell size, but therefore i need to define y+. i am interested in drag, so the boundary layer should be computed very well. what are appropriate values for y+ for my calculations? or where can i find out more about y+? i use ansys cfx, and i have not finally decided which turbulence model to use. most likely the SST (shear stress transport) model. can anyone help? 

April 3, 2009, 07:16 

#7 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,403
Rep Power: 97 
Hi Anneh,
As a starting point I would use traditional wall functions. Unless you can show they are not appropriate they are the best place to start. For traditional wall functions you should aim for 30>y+>100 approx, and the SST turbulence model is a good general purpose turbulence model to use. Glenn Horrocks 

April 3, 2009, 07:49 

#8 
New Member
Join Date: Apr 2009
Posts: 3
Rep Power: 9 
Hey Glenn,
thanks for your reply. i will try these wall functions. on a later point of my investigation i want to examine gurney flaps (their size is about 12%c), so i think i have to use a finer mesh. what would be a reasonable y+ value if i do not use wall functions? Anne 

April 5, 2009, 17:10 

#9  
Member
^_^
Join Date: Mar 2009
Posts: 36
Rep Power: 9 
Not sure if my understanding is right or not.
There are two ways for wall treatment. One is wall function method which uses the logorithmic law. In this case, 30<Y+<100. One is LowRe method which uses laminar equations in region close to the wall. In this case, 1<Y+<5. Quote:


April 5, 2009, 19:38 

#10 
Senior Member
Join Date: Apr 2009
Posts: 530
Rep Power: 13 
That's pretty much correct. For traditional wall functions 30 < y+ < 100 (or < 300, or , 1000, depending on your case). However, CFX doesn't use traditional wall functions, it uses scalable wall functions for the ke model. This basically removes the lower limit, so you don't need to worry if y+<30, the wall functions will still work OK. Scalable wall functions will not switch over to a lowRe formulation, they essentially just "ignore" the near wall nodes when y+ gets too small.
The omega based models (komega, SST) use an automatic wall treatment that will switch between wall functions and a lowRe formulation depending on the y+. These models are valid for y+ < 100 (or 300, 1000 etc), but to take full advantage of the lowRe formulation (e.g predicting separation) you need y+<=2. Mike 

April 6, 2009, 03:11 

#11 
New Member
Join Date: Apr 2009
Posts: 3
Rep Power: 9 
Hey Jasmine and Mike,
thanks for your answers. this is very helpful information :) Anne 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
grid dependancy  gueynard a.  Main CFD Forum  19  June 27, 2014 21:22 
IcoFoam parallel woes  msrinath80  OpenFOAM Running, Solving & CFD  9  July 22, 2007 02:58 
Could anybody help me see this error and give help  liugx212  OpenFOAM Running, Solving & CFD  3  January 4, 2006 19:07 
Discussion about Mesh independant solution  Seb  Main CFD Forum  13  May 22, 2001 13:37 
Wall functions  Abhijit Tilak  Main CFD Forum  6  February 5, 1999 02:16 