CFD Online Logo CFD Online URL
Home > Forums > FLUENT

The length of the first node

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

LinkBack Thread Tools Display Modes
Old   February 18, 2000, 15:37
Default The length of the first node
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?


  Reply With Quote

Old   February 21, 2000, 11:29
Default Re: The length of the first node
Ahmed Hassaneen
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=
  Reply With Quote

Old   February 22, 2000, 09:24
Default Re: The length of the first node
Volker Pawlik
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
  Reply With Quote


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
mesh file for flow over a circular cylinder Ardalan Main CFD Forum 6 April 17, 2010 23:40
Turbulence length scale and integral length scale rizhang CFX 1 September 10, 2009 06:38
Turbulent Characteristic Length/Turbulent Length Scale fluentnoob FLUENT 2 July 3, 2009 08:40
License server not visible from master node Charles FLUENT 0 October 30, 2007 18:48

All times are GMT -4. The time now is 02:13.