# The length of the first node

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

 February 18, 2000, 15:37 The length of the first node #1 Jennie Guest   Posts: n/a Hi! guys, Could you tell me how to define the length of the first node to the wall, if the flow is laminar or turbulent? Thanks. Jennie

 February 21, 2000, 11:29 Re: The length of the first node #2 Ahmed Hassaneen Guest   Posts: n/a Hi Jennie, What you mean by the "length", I think you mean the length normal to the wall. If this is true, in the laminar flow problems this length is not important but in turbulent flow problems it is very important and it is a different story. Good luck =Ahmed=

 February 22, 2000, 09:24 Re: The length of the first node #3 Volker Pawlik Guest   Posts: n/a Hi Jenny, I think your question is concerning the grid size of first cell adjacent to the wall? Turbulent flows: So for turbulent flow you should have a look to the definition of the y+=(density*u_tau*yp)/dyn.viscosity. u_tau is the so called friction velocity defined by sqrt(tau/density). For a pipe flow there is a relation-ship for u_tau/u=6.99(u_tau*R/kin. viscosity)^1/7 (R=pipe Radius, u=mean velocity) 1/7-Power law which can be generalized to a 1/n-law for different Re-numbers (e.g. see Blevins "Handbook of apllied fluid dynamics" for the relations between the friction coeff. lambda (or. s.t. called f) and n=1/sqrt(f), f=0.316/Re^0.25. So solve for u_tau and put it into the def. of y+. Then you you get an equation for y+ as function of y which is the distance of the cell center (!!!) from the wall. Then you are able to estimate y+ even for non-pipe flows. Just exchange the Radius with the half of the hydr. diameter of your problem. It works fine. The y+-value which suits you fine depends of course on the turbulent model and wall model you want to use. The y+ value is correct only for th full developed flow region. Laminar flows: have a look to the Fluent User's Guide p5-14 (fluent 5) or 5-23 (1996). For a fully developed pipe flow with Radius R choose: y/R<=0.1, for a flow between two plates choose y/H<=0.05 in order to resolve the flow profile correctly, that means that the stepwise linear approximation is not to far from reality. Unless the pressure loss due to shear stresses (or perpendicular momentum transport) will not be ok. Good luck

 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 Ardalan Main CFD Forum 6 April 17, 2010 23:40 rizhang CFX 1 September 10, 2009 06:38 fluentnoob FLUENT 2 July 3, 2009 08:40 Charles FLUENT 0 October 30, 2007 18:48

All times are GMT -4. The time now is 23:36.