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

y+ and y* issue

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

Like Tree2Likes
  • 1 Post By Ahmed
  • 1 Post By pUl|

Reply
 
LinkBack Thread Tools Display Modes
Old   October 23, 2005, 11:20
Default y+ and y* issue
  #1
Freeman
Guest
 
Posts: n/a
Hi all!

I am just starting using fluent for my simulations and in many bibliography the y+ and y* appears to be very important to make a right mesh, but the fact is that i still don't understant the meaning of these dimensionless parameters and their implications/utility for meshing?

Can someone explain them to me in plain english please?

Thanxs in advance!
  Reply With Quote

Old   October 23, 2005, 22:08
Default Re: y+ and y* issue
  #2
Ahmed
Guest
 
Posts: n/a
Panton book "Incompressible Flow" develops the Law of the wall. In short, we cannot generate a mesh to accuratley capture the flow details inside a boundary layer, instead all CFD programmes represent the boundary layer by a single wall layer. The thickness of this layer is selected so that the law of the wall is valid. This is important because the pressure drop along the flow path depends on the skin friction which is calculaed from the Law of the wall.
  Reply With Quote

Old   October 24, 2005, 15:07
Default Re: y+ and y* issue
  #3
Freeman
Guest
 
Posts: n/a
Thanxs Ahmed. That was really helpfull.

So, from your reply I understand that near the wall CFD soft calculates flow fields following the law of the wall and not only the RANS, don't them?

The only think that I don't know is which is the interval of y+ in what the Yplus Plot must be limited by, depending on the model I use to solve the problem. Can you or anyone highlight me in this? For example, I've read that for the Spallart-Allmaras the Yplus must be grater than 30 or near 1 but not in the 1-30 region? Is that right? And for the other RANS models?

Many thanxs!

  Reply With Quote

Old   October 24, 2005, 17:27
Default Re: y+ and y* issue
  #4
pUl|
Guest
 
Posts: n/a
Once more:

http://university.fluent.com/blog/in...&pb=1#comments

The fourth comment in the above link to be precise.
  Reply With Quote

Old   October 25, 2005, 06:23
Default Re: y+ and y* issue
  #5
Ahmed
Guest
 
Posts: n/a
Yes, the shear stress at the wall (Skin friction) is calculated from the Law of the Wall in all CFD programmes that I am familiar with. If you want to gain experience, insight about the acceptable values of Y+ (Y*) It will be helpful if you have the Law of the Wall plotted before you, most CFD/Fluid Mechanics books have that plot, just keep in mind that these published plots are taken from experimental data at zero pressure gradient, and because of this simple fact, CFD vendors advice (Recommend) lower values than those published (if you do not have access to such a plot drop me an email and I will scan the one I have and email it to you). Since you posted your question on this FLUENT Forum, I am going to assume that you are using this software, if so, you have no problem at all, if after carrying your analysis you find the values of Y+ to be high you can adapt the wall layer by going to [Adapt] -> Boundary and follow the instructions(Fluent will break each wall cell that you have selected into four smaller cells). Cheers and good luck with what you are doing.

Marsoup likes this.
  Reply With Quote

Old   October 25, 2005, 13:17
Default Re: y+ and y* issue
  #6
Freeman
Guest
 
Posts: n/a
Wow! Nice link pUl|: I didn't notice about this little Fluent forum. Thanxs, that was helpfull!

Ahmed: in point 11.9.1 of Fluent's users guide there's one plot of the law of the wall. And I've also found it in "Prandtl's Essentials of Fluid Mechanics" book. Know in this post I've realized about the importance of Y+ plot. With this, I conclude that I have to avoid the y+ located in the buffer layer, but new questions come to me:

1. In Fluent's users guide, it is said that Fluent makes calculations with the law of the wall for mean velocity when mesh is such that y*>11.225 and when it's lower than this value, it aplies the laminar stress-strain relationship U*=y*. So, this means that although Fluent makes this calculations, they would be not very reliable if I get a mesh with y+ values less than 30?

2. Which is the difference between y* and y+? Does Fluent always use y* for its calculations? In which manner does this affect in the recommended interval of [30,300] of y+?

3. When using Near-wall models (instead of wall functions), is still valid all the methodology done with y+ as we do when using wall functions? I mean, if plotting y+ makes still sense or I have to revise my meshes with other techniques?

I know the above was quite long Thanxs a lot!
  Reply With Quote

Old   October 25, 2005, 17:09
Default Re: y+ and y* issue
  #7
pUl|
Guest
 
Posts: n/a
I can answer the thrid question quickly and so here it is:

When you use Enhanced Wall Treatment (EWT), you're really resolving the flow all the way down to the wall (actually the turbulence models are modified to work that way when you use EWT). Ergo, you need to maintain a very low Y+ value near the wall. The recommended range is (1 to 5) although a value around 1 is usually recommended. Creating a mesh with such resolutions is often tricky as one also needs to ensure that cell aspect ratios (ratio of one edge of a cell to the other) greater than 1:5 are best avoided. So plotting the variation of Y+ along the wall is still useful as you can check if your resolution is within prescribed limits. However, bear in mind that the turbulent reynolds number has to be below 200 or some such for the first 10 odd cells. This is mentioned in the Fluent Users Guide.

Good Luck!
Marsoup likes this.
  Reply With Quote

Old   October 26, 2005, 10:19
Default Re: y+ and y* issue
  #8
Freeman
Guest
 
Posts: n/a
Ok pUl|, many thanks. These days I am reading point 11 of fluent's users guide intensively to take care about all these things about the mesh size near walls. I hope I could answer the othr questions for myself in the following days, but those have came to me reading the user's manual xD. Specially the fact that fluent does not work directlly with y+, as he makes calculations with y* and that in some cases,it uses the linear equation U*=y* (I imagine that it is to have a solution "at any cost", knowing that the mesh is not fine enough to use standard wall-equations and the result may be not accurate)

I will keep working on that (and reading/searching the forum for new answers). Thanxs again!
  Reply With Quote

Old   December 7, 2013, 16:23
Question
  #9
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 7
Anna Tian is on a distinguished road
Quote:
Originally Posted by Freeman
;125537
Ok pUl|, many thanks. These days I am reading point 11 of fluent's users guide intensively to take care about all these things about the mesh size near walls. I hope I could answer the othr questions for myself in the following days, but those have came to me reading the user's manual xD. Specially the fact that fluent does not work directlly with y+, as he makes calculations with y* and that in some cases,it uses the linear equation U*=y* (I imagine that it is to have a solution "at any cost", knowing that the mesh is not fine enough to use standard wall-equations and the result may be not accurate)

I will keep working on that (and reading/searching the forum for new answers). Thanxs again!

If that is true, why do we still need to know Y+? Y* is already enough to make sure that the first line is inside the subviscous layer.
__________________
Best regards,
Meimei

Last edited by Anna Tian; December 9, 2013 at 05:20.
Anna Tian 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
Issue installation OpenFOAM - libopen-rte.so.0 Voyage_gui OpenFOAM 1 August 12, 2011 03:46
Meshing related issue in Flow EFD appu FloEFD, FloWorks & FloTHERM 1 May 22, 2011 08:27
snappyHexMesh Issue thomasnwalshiii OpenFOAM 3 March 15, 2011 14:49
Simple Frustrating Meshing Issue in Gambit (w/pics) Dylan ANSYS Meshing & Geometry 6 March 23, 2009 17:14
STAR-CD Dynamics issue 16 CD adapco Group Marketing CD-adapco 0 November 30, 2001 11:25


All times are GMT -4. The time now is 09:59.