CFD Online Logo CFD Online URL
Home > Forums > General Forums > Main CFD Forum

initial condition of DNS

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

LinkBack Thread Tools Display Modes
Old   June 6, 2001, 09:42
Default initial condition of DNS
Posts: n/a
Dear all. I'm going to perform direct numeriacl simulation of the fully developed turbulent flow through square duct. I want to make efficient initial condition of velocity field in order to get fully developed turbulent profile faster. Could you tell me how to make initial velocity of turbulent flow.

  Reply With Quote

Old   June 6, 2001, 11:33
Default Re: initial condition of DNS
Frederic Felten
Posts: n/a
Hi there,

A way of initializing the field would be to superimpose some random fluctuation to the typical turbulent average velocity profile for channel flow. you would get something like (in fortran):

flct= 0.1 u= uaverage(y) + flct*( rand(0) - rand(0) ) v= flct*( rand(0) - rand(0) ) w= flct*( rand(0) - rand(0) )

Where the expression for uaverage(y) is known and can easily be found in the litterature. Check the book: "Viscous Fluid Flow" by Frank M. White, McGraw-Hill, 1991.


Frederic Felten.
  Reply With Quote

Old   June 6, 2001, 14:17
Default Re: initial condition of DNS
John C. Chien
Posts: n/a
(1). There was some discussions here, long time ago. So, you may want to do the old messages search for the related topics.
  Reply With Quote

Old   June 8, 2001, 11:32
Default Re: initial condition of DNS
Posts: n/a
You can temporally evolve the solution using a pressure-driven periodic flow in a square duct. They are a couple of points to note.

i) You can not estimate the pressure gradient needed to evolve the flow to the Reynolds number you want unless you know the wall shear stress distribution (in the fully developed state) in the cross-sectional plane. You would know the stress distribution if you know the velocity profiles (at least near the walls). If you already know the velocity profile, you might not want to solve the problem unless you want the turbulence characteristics. To solve this problem, assume a pressure gradient, solve the periodic problem and if the bulk flow Re is lower than what you need, increase the pressure gradient or else decrease it. You can use Newtons method to arrive at the pressure gradient at each step (or every few time steps). Once you have the Re you want, you also have at hand the pressure gradient that is needed to drive the flow.

ii) When you solve the periodic problem, you need to make sure that length of the domain in the periodic direction is much larger than the longitudinal integral length scale and the size of the largest longitudinal structure you want.

iii) Temporal evolution to a fully developed state might take a long time when using DNS. So use coarser resolution (about four times coarser along each direction than the DNS) ans use LES to obtain a quick approximate solution. Then map this LES solution to the fine mesh and then start the DNS.
  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
Low Mach number Compressible jet flow using LES ankgupta8um OpenFOAM Running, Solving & CFD 7 January 15, 2011 14:38
MRFSimpleFOAM goes divergenced! renyun0511 OpenFOAM Running, Solving & CFD 0 November 19, 2009 03:11
Computational time sunnysun OpenFOAM Running, Solving & CFD 5 March 16, 2009 04:32
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09
Modeling in micron scale using icoFoam m9819348 OpenFOAM Running, Solving & CFD 7 October 27, 2007 00:36

All times are GMT -4. The time now is 12:49.