# y+ value calculation

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

 March 23, 2005, 03:39 y+ value calculation #1 BV Guest   Posts: n/a Dear STAR CD users, How do we calculate the "y+ value" to assign boundary thickness? help me out in this. ----BV

 March 23, 2005, 14:40 Re: y+ value calculation #2 Tom Guest   Posts: n/a I will tell you the way that I do it. I use: y=14*(y+)*(viscosity/(density*velocity)) Then I assume that y+ is about 75 and solve for y, where y will be my first cell layer thickness. This is actually the formula for a flat plate, but gives a pretty good estimate for other geometries also. The thing to remember is that you need to keep units the same. So if you use SI for the fluid properties, then the y value will be in meters, etc. Tom

 March 24, 2005, 06:05 Re: y+ value calculation #3 BV Guest   Posts: n/a Thanks Tom

 March 24, 2005, 12:02 Re: y+ value calculation #4 Amod Kumar Guest   Posts: n/a A more generic approach to calculation of Y+ can be outlined as follows: Step-1: Workout 'k' nased on estimate of local velocity magnitude 'u' and tubulent intensity 'I' (k=1.5*(u*I)**2, I ~ 0.01 Step-2: Esimate turbulent dissipation rate 'epsilon' based on 'k' and turbulent mixing length 'L' (usually of the order of 0.01*Hydraulic Diameter) where epsilon= (0.09)**3/4 X k**1.5/L (0.09 is an empirical constant) Step-3: Work out tubulent coeff of viscosity 'mu_ee' which is equal to 0.09*density*k**2/epsilon Step-4: Estimate wall shear stress (tau_wall) based on assumed velocity profile (appropriate wall law) i.e. tau_wall = (mu_tee + mu_lam)* du/dy Step-5: Work-out u_star Step-6: Finally, estimate Y from definition of Y+ assuming Y+ ~ 3-5 (in case viscous sublayer to be resolved and Y+ 30~50 in case only turbulent zone is to be resolved. (Note that this estimation of Y would be based on CELL-CENTROID location and not cell thickness). Hope this will help! Amod Kumar PS: Some FLUENT tutorials for example such as developing turbulent flow in pipe do suggest empirical formula to calculate Y+. However, I have not come across similar expression in STAR-CD. Has anyone come across ADAPCO recommendation to calculate Y+?

 March 24, 2005, 14:18 Re: y+ value calculation #5 Pauli Guest   Posts: n/a I believe the FAQ section on adapco-online has basically the same explanation.

 March 24, 2005, 23:11 Re: y+ value calculation #6 Amod Kumar Guest   Posts: n/a Yes Pauli, it has been re-phrased (alongwith some recommendation about I & L)from the info available at http://www.adapco-online.com/adapco_...vices/faq.html I forgot to give this link. Amod

 April 11, 2005, 09:05 about y+ #7 ABHAY GUDI Guest   Posts: n/a respected sir i want to get some information about y+. why is this y+ important? how do u define y+ in mixing length CFD solver? why k-e turbulence model is better than mixing length model. explain me clearly about both these models, and y+

 April 13, 2005, 13:11 Re: about y+ #8 Tom Guest   Posts: n/a Not an easy series of questions to answer. Simply, y+ determines which wall boundary conditions exist. Some texts state the near wall boundary is laminar if y+<= 11.63. The analysts have two ways to go - design the mesh to give the y+ to suit your model, or if you can not do that, choose your turbulance model and wall treatment to suit your y+. y+ is defined by the thickness of your subsurface. To determine what y+ is after the run, you must specify that the code print y+ values. Then do a getw,yplus then do a wall plot (wplot). The mixing length for y+ is usually set as one order of magnitude smaller than the hydraulic diameter. I would suggest the text Turbulence Modeling for CFD by David Wilcox. Tom

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Alireza FLUENT 2 May 10, 2006 16:34 Alireza CFX 1 May 9, 2006 08:52 Micaela Demichela FLUENT 2 November 16, 2001 00:40 kvbswamy CFX 0 August 10, 2001 02:36 Mark Render Main CFD Forum 0 May 2, 2001 09:48

All times are GMT -4. The time now is 18:27.