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

lowering y+ on surfaces...

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 22, 2002, 15:51
Default lowering y+ on surfaces...
  #1
Dimitrios
Guest
 
Posts: n/a
Hi I just started using CFX5.5 (CFX4 before) but I have a problem. With CFX4 I could build a block next to a wall and make a fine mesh and in that way keep low y+ values (around 11) but I don't know which parameter I should "play" with in CFX5. I've tried the mesh control and inflated boundary (were I adjusted the geometric progression on the relevant boundaries) but still my y+ values are too high. Does anyone have a good idea of what I can play around with in the Mesh menu? Every advice is welcome!!!

Dimitris

  Reply With Quote

Old   March 22, 2002, 17:33
Default Re: lowering y+ on surfaces...
  #2
Astrid
Guest
 
Posts: n/a
Dimitros

What is high?

CFX 5.5 provides two values: 1)SOLVER YPLUS and 2) YPLUS. Forget SOLVER YPLUS. Just look at YPLUS which should be between 11 and 100, provided you use a turbulence model with waal functions. If you use a sublayer model, it should be below 2.

Improving your YPLUS can be established using an inflation layer with 10 elements with a progression of 1.3. You need at least 10 elements in your boundary layer. If YPLUS is too high, just increase the progression factor to 1.4 or 1.5. With a simple Excel-sheet you should be able to calculate your smallest element and estimate the expected YPLUS.

Astrid
  Reply With Quote

Old   March 23, 2002, 12:36
Default Re: lowering y+ on surfaces...
  #3
Dimitris
Guest
 
Posts: n/a
Thank you very much Astrid....it works great!!!
  Reply With Quote

Old   March 23, 2002, 20:29
Default Re: lowering y+ on surfaces...
  #4
Neale
Guest
 
Posts: n/a
Also note that the fixed y-plus (scalable) wall functions in CFX-5.5 are the default when running k-epsilon. You can't get y-plus below 11 with these because the code is assuming that the first control volume at the wall is at the boundary of the viscous sub-layer, not inside it.

You might try running SST instead of k-epsilon which automatically integrates to the wall where it can (i.e., you have enough grid to resolve the boundary layer), and automatically uses scalable where you don't have enough grid.

Either way though, Astrid is right. You should use inflation and try and get some control volumes into your boundary layer if resolving the boundary layer is important for your application.

Neale
  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
how to get forces on Iso-Clip Surfaces and How to get forces in cylindrical coordinat CFD XUE FLUENT 3 March 18, 2015 04:28
snappyHexMesh not refining surfaces Hydro1004 OpenFOAM 3 August 29, 2012 11:56
problemes modelling surfaces with snappyhexmesh gija79 OpenFOAM 5 June 30, 2010 13:50
Faceted surfaces in ICEM Chriss Main CFD Forum 1 May 6, 2008 15:18
Surfaces Mark FLUENT 2 February 9, 2004 11:41


All times are GMT -4. The time now is 18:03.