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

Residence time in VoF-model

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 7, 2008, 10:32
Default Residence time in VoF-model
  #1
Andreas
Guest
 
Posts: n/a
Hello everybody,

I've got a vof-model of a zylinder filled with water and air. There is a velocity inlet at the bottom (water), a pressure inlet at the top(air) and a pressure outlet.

I want to study the displacement of "old" water by "new" water.

Species dosen't work with VoF and defining two water-phases (old and new) is no option as well, because VoF-phases may not be interpenetrating.

One workaround I thought of, was to create a new one-phase model with the previously optained water-air-interface-contour as a frictionless wall.

If anybody has some solution to my problem or could advice some link/literature/...

Thanks, Andreas

  Reply With Quote

Old   February 8, 2008, 17:46
Default Re: Residence time in VoF-model
  #2
KW
Guest
 
Posts: n/a
You can use a user-defined scalar as described below. From Fluent tech support, also in Fluent UDF archive on User Service Center.

==================== Solution 619 Fluid residence time

Problem: Compute fluid residence time.

Problem solved via UDF using user-defined scalars. Source code for UDF is below.

1. Compile udf 2. Read case.... set # UDS > 0 3. At inlet, set UDS (value) = 0 4. Set diffusivity of UDS to a small value 5. Set source term of UDS to "rt_source" in the appropriat fluid zones 6. Iterate.

Values of UDS represent the length of time fluid has been in the domain since it entered the inlet (in seconds).

Resolution: ------------- #include "udf.h"

/* * UDF to compute fluid residence time * * by William Wangard, Ph.D. * Fluent, Inc. * */

/* * This UDF requires at least 1 UDS to be defined * At inlet, define UDS (value) = 0 * UDS will have units of time and represent approximate residence time * of fluid in domain * * Diffusivity of scalar should be small to reduce diffusion i.e. 1E-5 * */

DEFINE_SOURCE(rt_source,c,t,dS,eqn) { real source = C_R(c,t); dS[eqn] = 0.0; return source; }

  Reply With Quote

Old   February 15, 2008, 07:47
Default Re: Residence time in VoF-model
  #3
Andreas
Guest
 
Posts: n/a
Thank you very much!

Andreas
  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
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 bookie56 OpenFOAM Installation 8 August 13, 2011 04:03
air bubble is disappear increasing time using vof xujjun CFX 9 June 9, 2009 07:59
urgent query regarding vof model plz rply Garima Chaudhary FLUENT 0 July 13, 2007 02:20
residence time Sugen Chetty Main CFD Forum 0 January 28, 2002 10:50


All times are GMT -4. The time now is 04:52.