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

wall y+ value

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 21, 2007, 01:17
Default wall y+ value
  #1
Sham
Guest
 
Posts: n/a
Hello all,

I am using Standard Wall Function with k-epsilon model. I understand that wall y+ value should be 30-300 to get a good results. I tend to get y+ around 1-3 which is veru small even after coarsen the mesh. If the valus is less than 30, is my results wrong?

To get 30-300, I really have to make the mesh REALLY coarse and I am not sure as to the appropriateness of this.

Hope someone can clarify.

Thanks. Sham.
  Reply With Quote

Old   August 21, 2007, 02:28
Default Re: wall y+ value
  #2
carno
Guest
 
Posts: n/a
Check the overall Re number and take the appropriate decision of modelling turbulence or not?
  Reply With Quote

Old   August 21, 2007, 02:59
Default Re: wall y+ value
  #3
Razvan
Guest
 
Posts: n/a
Do not change the mesh, use Enhanced Wall Treatment instead of the standard wall functions (this is valid for y+ around 1). Or change the turbulence model (standard or SST k-omega with "transitional flow" option activated).

All the best,

Razvan
  Reply With Quote

Old   August 21, 2007, 03:07
Default Re: wall y+ value
  #4
Sham
Guest
 
Posts: n/a
If I use EWT, will my results be accurate. I read that SWF is well-established and has been used widely.
  Reply With Quote

Old   August 21, 2007, 03:21
Default Re: wall y+ value
  #5
Razvan
Guest
 
Posts: n/a
Well, that depends on what you are trying to model. Describe your problem in detail and I should be able to suggest you an appropriate setup.

Razvan
  Reply With Quote

Old   August 21, 2007, 03:34
Default Re: wall y+ value
  #6
Sham
Guest
 
Posts: n/a
Razvan,

I am modelling a cylinder in free stream with structured mesh. Re=10000. I am interested in Cd, Cl and also vortex shedding. I am using RKE model. Hope you can give some suggestions here.
  Reply With Quote

Old   August 21, 2007, 03:36
Default Re: wall y+ value
  #7
Razvan
Guest
 
Posts: n/a
What FLUENT version are you using?

Razvan
  Reply With Quote

Old   August 21, 2007, 04:33
Default Re: wall y+ value
  #8
Arjun
Guest
 
Posts: n/a
Hey guys,

I am trying to create a model around a car geometry provided in the GAmbit tutorial guide to model the turbulent flow past the simplified sedan. I am thinking of using the standard k-epsilon model for this purpose. Howeevr I do not know hot to create a proper mesh around the car. CAn someone help me on how to create a good mesh. I am using FLUENT 6.3.26

Thanks Regards, Arjun
  Reply With Quote

Old   August 21, 2007, 04:34
Default Re: wall y+ value
  #9
Sham
Guest
 
Posts: n/a
Fluent 6.3.
  Reply With Quote

Old   August 22, 2007, 02:36
Default Re: wall y+ value
  #10
Razvan
Guest
 
Posts: n/a
OK. If you are interested in accuracy, then you MUST use LES. Vortex shedding behind the cylinder is a very difficult case to simulate correctly, and only LES models can give you good results for Re=10000. The LES models I would recommend you are the dynamic Smagorinsky model or the turbulent-kinetic-energy transport model. Of course, all this has to be done in 3D.

If you are not familiar to LES, then a second good approach would be the low-Re omega-based RSM. I personally tested it on a cylinder configuration, and the results were qualitatively good, actually quite similar to LES. Quantitatively, I cannot say, because I did not run the simulation for long enough to be able to apply a time-averaging. But this was also done in 3D, unsteady pressure-based solver.

The simplest way to try this is 2D, with a SST-kw or low-Re omega-based RSM turbulence model, of course using unsteady solver. But I cannot guarantee you that the results will be good. The 3-dimensional effects cannot be neglected. You will obtain vortex shedding, no doubt about that, but Cd and Cl might not be correctly calculated.

Razvan
  Reply With Quote

Old   August 22, 2007, 10:33
Default Re: wall y+ value
  #11
Phil
Guest
 
Posts: n/a
Razvan,

Thanks very much for yourt reply. At the moment though I'm simulating combustion with RANS as a part of research so I don't really have a choice with LES. I am moving onto LES towards the end of my PhD though.

The results are good escept for when I inject the fuel from the wall in question. The fuel seems to stick to it and it causes inaccuracy.

For second order which will give better results in my unstructured tet mesh (fuel injection) segment, when I put it onto EWT it crashes every time.

When injecting from an area far back inside the swirler section, the distribution of fuel in the combustor is largely accurate, so EWT isn't required. It's just this damn wall injection model.

PS - I was thinking of trying to get a much much smoother transition between the dense and coarse areas to see if it helps. IF ANYONE KNOWS IF THES OR A MORE 'STEPWISE' SOLUTION PROCEDURE IS WORTH PURSUING THEN PLEASE LET ME KNOW.

Thanks again Razvan! Phil
  Reply With Quote

Old   August 22, 2007, 10:35
Default Re: wall y+ value
  #12
Phil
Guest
 
Posts: n/a
Sorry for some reason I thought this was a different post. Pleases igonre my message.
  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
Natural convection in a closed domain STILL NEEDING help! Yr0gErG FLUENT 3 June 12, 2013 02:12
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
Fluent3DMeshToFoam simvun OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 48 May 14, 2012 05:20
Errors running allwmake in OpenFOAM141dev with WM_COMPILE_OPTION%3ddebug unoder OpenFOAM Installation 11 January 30, 2008 21:30
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 02:58.