
[Sponsors] 
June 29, 2012, 08:57 

#21  
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,990
Blog Entries: 6
Rep Power: 39 
Quote:


June 29, 2012, 09:01 

#22  
Member
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6 
Quote:
So you mean bigger mesh near the wall gives better results? in my model y+ is varying between 040, so in the region by y+>11 the standard wall function is working well while in the region by y+<11 is giving us wrong results. on the other hand i read in ansys documentation that at least 10 nodes in boundary layer is needed, so we need bigger mesh for the wall function and smaller mesh for accuracy !!!!! 

July 1, 2012, 08:35 

#23 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,045
Rep Power: 86 
Yes, ideally you want all nodes to be y+>11 for standard wall functions. And you are correct in that often contradicts the requirement for sufficient nodes in the boundary layer.
The best solution is usually to use the SST turbulence model with automatic wall functions and it can handle just about any y+. If you still want to stick with standard wall functions then I would do a y+ sensitivity check. You may well find that your simulation is not very sensitive to y+ anyway, and in this case you can run any y+ you like (within reason). 

July 1, 2012, 08:43 

#24 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,990
Blog Entries: 6
Rep Power: 39 
I would like to share my work on turbo machinery. In this case, i tried the Yplus 1, 10 and 60 with scalable wall function and Y+ = 10 with standard wall function. Results clearly show the problem with standard wall function.


July 1, 2012, 08:59 

#25 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,990
Blog Entries: 6
Rep Power: 39 
In case of SST y+ greater than 10 does not produce the good results as shown in this pic: Definitely this is the difficult case for any turbulence model and wall treatment. In simpler cases, you might not find any difference at all


July 1, 2012, 18:22 

#26 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,045
Rep Power: 86 
Nice dataset Far. Shows the wall boundary condition is important in your turbomachinery case.
But do not make the mistake in assuming therefore it is important in all cases. CFD covers a very wide range of applications, and in quite a few of them the wall boundary condition details does not make much difference. For instance HVAC modelling. 

July 2, 2012, 04:50 

#27  
Member
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6 
Quote:
Thanks for nice explanation, one basic question, in the model you usualy have a range of Y+ , when you say y+=1, 10, ... you are talking about the maximum y+ in the model, am i right? 

July 2, 2012, 05:08 

#28  
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,990
Blog Entries: 6
Rep Power: 39 
Quote:
But I want to pointout one important aspect. If you are not solving the equations with integration to the wall approach then you may not be able to predict the quantities accurately e.g. drag on airfoil. So when you are using the wall function you may miss the important flow physics. Obvious fact On the other side as you have pointed out that if you solve the HVAC problem with intergration to wall approach or wall function apporach, it wont make any difference at all. Very true and I agree again. But if you are putting the wrong numerics i.e. using the integration to wall mesh for the standard wall function you are forcing the numerical algorithm for the things it was not designed. So we should keep the wrong numrics and wrong physcis into separate boxes. 

July 2, 2012, 05:15 

#29  
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,990
Blog Entries: 6
Rep Power: 39 
Quote:
I am talking about the average values on the blade surface. I have some how higher values at the leading edge and lower values at separation point( Y + = 120 for Y+ = 10 case). But that portion is not more than 510%. For example for Y+1 mesh, Maximum Y+ is 56. I shall try to post the pic of Y+ values (Y+ and solver Y+) 

July 2, 2012, 05:20 

#30 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,990
Blog Entries: 6
Rep Power: 39 
see Fig. 9 in this reference http://num.math.unigoettingen.de/ba...ings/knopp.pdf for the definition of average Y+
This is also another reference by same author. http://num.math.unigoettingen.de/ba...ngs/alrutz.pdf See Fig 4 Note the difference for the SA and SST model for the range of Y+ values. Knopp recommends the Y+ <=10 for SA model for good results for flow with stagnation, separation etc. And higher values for SST model. 

July 2, 2012, 06:16 

#31 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,990
Blog Entries: 6
Rep Power: 39 
See Fig 1 & 2 http://www.mscsoftware.com/events/ae...pdf/p10201.pdf
Slide 20 http://www.powershow.com/view/b0e25...n#.T_FzQxdKol8 Slide 21 http://www.docstoc.com/docs/10845119...micsUsingCFX General comments about turbulence model and wall treatment with good data from industry. http://www.ansys.com/staticassets/AN...pabilities.pdf Slide 34 clearly states that the Y+ insensitive treatment is availalbe for all turbulence models in ANSYS CFD (CFX+Fluent+other modules) https://www.sharcnet.ca/Software/Flu...bModeMath.html http://www.mathematik.unidortmund.de/~kuzmin/IJCSM.pdf http://nippon.zaidan.info/seikabutsu...okyo_ts059.pdf http://www.idac.co.uk/products/downl...NSYS%20CFX.pdf 

July 2, 2012, 06:59 

#32  
Member
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6 
Quote:
Many Thanks Far ! 

July 6, 2012, 13:53 

#33 
Member
pooyan
Join Date: Nov 2011
Posts: 62
Rep Power: 5 
Hi All,
I was reading your discussion for standard and scalable wall functions. I have a question which may not be related to your discussion, but maybe I can get the answer from you. I do not know where the boundary conditions for U at first grid point is defined in OpenFoam when using wall functions. I expect to see some values for U at the first grid point based on log law equation, but I can not find this implementation through the code. can you please help me on that?! ( I see some implementation for k, epsilon and nut in their corresponding wall functions but nothing for U) So, for the first grid point, do we still solve equations to obtain U?! I will be so appreciated if you can help me with this question. thanks 

July 8, 2012, 07:19 

#34 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,045
Rep Power: 86 
This is the CFX forum, try the Openfoam forum for that question.


March 7, 2015, 11:22 

#35  
Member
Join Date: Aug 2014
Posts: 76
Rep Power: 3 
It's not very clear for me, I wonder if below Y+ = 11.06 mesh points are ignored or below Y+ = 11.06 mesh points are set up to y+ =11.06.
But if it's the last option, this means that we associate a y+ of 11.06 on cell initially too small, do you see what I mean ? Quote:


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
channelFoam for a 3D pipe  AlmostSurelyRob  OpenFOAM  3  June 24, 2011 13:06 
Wall function for velocity?  johnblund  OpenFOAM  0  March 10, 2011 09:50 
BlockMesh FOAM warning  gaottino  OpenFOAM Native Meshers: blockMesh  7  July 19, 2010 14:11 
Need some wall function approaches!  yka8150  Main CFD Forum  0  September 21, 2009 23:08 
Problem with rhoSimpleFoam  matteo_gautero  OpenFOAM Running, Solving & CFD  0  February 28, 2008 07:51 