CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

CFX 12.1: y+ value for SST

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree7Likes
  • 1 Post By Jade M
  • 6 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   March 3, 2010, 06:56
Default CFX 12.1: y+ value for SST
  #1
New Member
 
Join Date: Mar 2010
Posts: 2
Rep Power: 0
Aragorn25 is on a distinguished road
Hello

for CFX 11.0 the y+ value has to be set to 1 for SST turbulence model.
is there a change for the new version CFX 12.1 or has y+ still to be set to 1?

Thanks
Aragorn25 is offline   Reply With Quote

Old   March 3, 2010, 17:56
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,828
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I assume you are talking about meshing, that is generating a mesh with an estimated y+ of 1? There has been no change there.
ghorrocks is offline   Reply With Quote

Old   March 10, 2010, 16:35
Default Antwort
  #3
New Member
 
Join Date: Mar 2010
Posts: 2
Rep Power: 0
Aragorn25 is on a distinguished road
Das SST-Model in ANSYS CFX benutzt automatische Wandfunktionen, d.h. Sie können sowohl High-Reynolds Netze mit y+ Werten > 11 rechnen als auch Low-Re Netzt mit y+ < 2. Auch im Übergangsbereich arbeitet das Modell konsistent mit den Gleichungen. Diese Implementierung gibt es seit den ersten ANSYS CFX Versionen und hat sich nicht geändert. Die automatische Wandfunktionen gehen mit allen Turbulenzmodellen, die auf der omega-Gelichung beruhen:
SST
BSL
k-omega
Aragorn25 is offline   Reply With Quote

Old   April 5, 2010, 14:54
Default Confused
  #4
Senior Member
 
Join Date: Feb 2010
Posts: 145
Rep Power: 8
Jade M is on a distinguished road
Aragorn25, I'm curious about your response since I see the number 11. I do not understand German.

I thought that the value of y+ should be 1, also. I see this is the 12.1 manuals in a couple of places.

However, in CFX Tutorials, Release 12.1, November 2009, pp. 109-110, there is the statement "At the lower limit, a value of y+ less than or equal to 11 indicates that the first node is within the laminar sublayer of the boundary flow. Values larger than this indicate that an assumed logarithmic shape of the velocity profile is being used to model the boundary layer portion between the wall and the first node.” I am curious abou this value of 11?

Thanks very much for any clarification from anyone out there. Have a great day.
Jade M is offline   Reply With Quote

Old   April 5, 2010, 18:56
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,828
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The log layer region and the significance of y+=11 is explained in any turbulence text book, or even most general CFD modelling textbooks. Try "Turbulence Modelling for CFD" by Wilcox, for example.
ghorrocks is offline   Reply With Quote

Old   April 6, 2010, 09:16
Default I do not have access to these books
  #6
Senior Member
 
Join Date: Feb 2010
Posts: 145
Rep Power: 8
Jade M is on a distinguished road
but thanks for your reference to general resources. Does anyone have an answer to my questions? Thanks in advance for any assistance.
Jade M is offline   Reply With Quote

Old   April 6, 2010, 18:48
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,828
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You asked a general turbulence question which is not specific to CFX. I am not going to write a turbulence text book to define where the 11 comes from for you. Your question is answered in any turbulence text book so that is where you should look.
ghorrocks is offline   Reply With Quote

Old   April 7, 2010, 09:16
Default LOL at ghorrocks
  #8
Senior Member
 
Join Date: Feb 2010
Posts: 145
Rep Power: 8
Jade M is on a distinguished road
I am truly sorry for the inconvenience I have caused you. I appreciate your stating the obvious that I could find the information in books and then following up with antagonism. I do not think I asked you to write a turbulence model or anything for that matter. Good luck though.

Last edited by Jade M; April 7, 2010 at 11:40.
Jade M is offline   Reply With Quote

Old   April 7, 2010, 09:21
Default y+=11
  #9
Senior Member
 
Join Date: Feb 2010
Posts: 145
Rep Power: 8
Jade M is on a distinguished road
For those who are interested, 11.06 is the y+ value where the linear velocity profile in the sublayer intersects with the logarithmic velocity profile in the log layer.

For the k-e model you should use y+ < 300. If y+ is below about 11 for the k-e model then it still works fine, but it doesn't make use of the fine near wall mesh, so it's a waste of mesh. Essentially the k-e model always uses the wall function approach. The wall function approach is not valid below y+ ~= 11, so we just ignore the mesh below y+ ~= 11.

If you want accurate boundary layer predictions, such as separation prediction, then you should use the SST model with y+ < 2. In this case the SST model will switch to a low-Re formulation near the wall rather than the wall function formulation. SST will still work fine with 11 < y+ < 300, but the results will be fairly similar to the k-e model since it will be using wall functions. For 2 < y+ < 11 it will be a blend between wall functions and low-Re formulations.

In some situations, such as accurate boundary layer heat transfer predictions or when using the transition model, an even lower y+ of about 1 is recommended with the SST model.
adam likes this.
Jade M is offline   Reply With Quote

Old   April 7, 2010, 18:54
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,828
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
No problem - it looks like you have found the answer to your question.

Your explanation is not quite correct. Here are some points:

There is no real upper limit on the y+ value you can use in the wall function approach. The real upper limit is set by a mesh convergence study - as you coarsen the mesh you will loose boundary layer accuracy and eventually simulation accuracy will suffer. But which y+ value this occurs on will depend on the simulation.

k-e, when using a wall function approach does not "ignore" mesh with y+<11. What it does is to blindly apply the wall function approach to the first node assuming it is in the log layer, but when y+<11 it is not in the log layer but in or near to the laminar sublayer. This means you will be applying the wrong physical model and your boundary layer profile will be wrong.

The wall function approach is accurate providing you are only interested in the log layer and beyond.

In general, integrating to the wall will give more accurate separation predictions then the wall function approach, but not universally. If a separation is off a sharp corner then wall functions work fine.

When integrating to the wall, yes you will need y+<2. But the exact value of y+ required for accuracy is problem dependant and again you need to do a sensitivity study to find out. Generalisations are dangerous.
D.B, joy2000, goyz515 and 3 others like this.
ghorrocks is offline   Reply With Quote

Old   May 6, 2012, 06:25
Default
  #11
New Member
 
Muhammad K
Join Date: Apr 2012
Location: Sydney, Australia
Posts: 10
Rep Power: 5
MuhammadK is on a distinguished road
Hi

I have looked at the Ansys Help document in the wall boundary condition, but still could not find anything with 'Y+'. As a new user, I believe its in the help document, but its just that I could not find it.
Can anyone point clearly where should I look for?

Are there any books/pdf/whatever online of which will help me understand it better?

Thanks

Muhammad
MuhammadK is offline   Reply With Quote

Old   May 6, 2012, 06:38
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,828
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You are looking for the CFX theory manual. The section on near wall modelling of turbuelnt flows.

Just about any CFD textbook will describe basic turbulence model application and wall functions. If you want a mode detailed/advanced textbook "Turbulence modelling for CFD" by Wilcox is a good textbook.
ghorrocks is offline   Reply With Quote

Old   May 8, 2012, 21:17
Default
  #13
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 486
Rep Power: 9
evcelica is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
when y+<11 it is not in the log layer but in or near to the laminar sublayer. This means you will be applying the wrong physical model and your boundary layer profile will be wrong.

I was under the impression CFX uses scalable wall functions to overcome the problem of too small of a Y+ for the k-e turbulence model.
evcelica is offline   Reply With Quote

Old   May 9, 2012, 03:54
Default
  #14
New Member
 
Muhammad K
Join Date: Apr 2012
Location: Sydney, Australia
Posts: 10
Rep Power: 5
MuhammadK is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You are looking for the CFX theory manual. The section on near wall modelling of turbuelnt flows.

Just about any CFD textbook will describe basic turbulence model application and wall functions. If you want a mode detailed/advanced textbook "Turbulence modelling for CFD" by Wilcox is a good textbook.
Thanks Glenn. got the book from the library.

Cheers
MuhammadK is offline   Reply With Quote

Old   January 23, 2015, 05:17
Default
  #15
spl
New Member
 
spl
Join Date: Nov 2014
Posts: 24
Rep Power: 2
spl is on a distinguished road
Hi,

Sorry to bring up such an old post but I have a question the statement -

Quote:
The real upper limit is set by a mesh convergence study - as you coarsen the mesh you will loose boundary layer accuracy and eventually simulation accuracy will suffer. But which y+ value this occurs on will depend on the simulation.
Does this mean through your mesh convergence study you would keep a constant initial cell height and overall boundary layer mesh height or change them with mesh density? If you do change these parameters how do you determine if the change in your results is due to the change in boundary layer resolution or the change free stream resolution? Alternately, would you conduct separate boundary layer and free stream refinement studies?
spl is offline   Reply With Quote

Old   January 23, 2015, 06:33
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,828
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If the boundary layer and free stream are separable then it is easier to do them separately. Often they are not, so you have to do it all together.

More advanced mesh convergence studies (see the references in the FAQ) require a mesh refinement parameter to use for optimisation. It is best if that single parameter controls the entire mesh size. But the technique still works as long as the parameter changes the most significant part of the mesh on the output.
ghorrocks is offline   Reply With Quote

Old   January 23, 2015, 06:40
Default
  #17
spl
New Member
 
spl
Join Date: Nov 2014
Posts: 24
Rep Power: 2
spl is on a distinguished road
Thank you very much Glenn.

Regards

Last edited by spl; February 5, 2015 at 04:29.
spl is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Pros and Cons for CFX, CFdesign, COMSOL Val Main CFD Forum 3 June 10, 2011 02:20
Importing solutions in CFX. Alphonso CFX 1 August 1, 2008 14:01
PhD using CFX Rui CFX 9 May 28, 2007 05:59
CFX 10 VS CFX 11 for combustion Jonathan Lemay CFX 2 May 9, 2007 11:58
CFX 4.4 installation problem Pandu Sattvika CFX 1 December 1, 2001 05:07


All times are GMT -4. The time now is 20:27.