CFD Online Logo CFD Online URL
Home > Forums > FLUENT

HELP.......sloshing problem using VOF

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

LinkBack Thread Tools Display Modes
Old   July 26, 2005, 07:04
Default HELP.......sloshing problem using VOF
Posts: n/a
hi guys new to FLUENT ...can any body help me with sloving the "Sloshing Problem" using VOF with regards to the boundary conditions to be used and the relevant input details...... thanks to all who want to help ....bbye
  Reply With Quote

Old   July 27, 2005, 06:29
Default Re: HELP.......sloshing problem using VOF
edi ghirardi
Posts: n/a
On boundary conditions: if you have an outlet or inlet define them as pressure boundaries, but the whole thing works fine even in closed domains (i.e., all walls). I assume that you don't have fluid filling or draining from your tank or whatever. You have to make your slosh motion driven by the gravitational accelerations (in the operating condition panel). If you have to define them as functions of time let me know I can give you a couple of UDFs or a scheme file.

-The solver must be unsteady (1st order implicit)

-the multiphase model is obviously VOF. Turn on the implicit body force option

-set the phases. The primary phase should be the lighter

-if you have baffles, slit em!

-on the operating conditions panel enable gravity and specify the operating density as the one of the lighter phase.

-keep your URFs quite big (0.6 and 0.8 for pressure and momentum respectively, 1 for the other parameters)

-discretization schemes: BODY FORCE WEIGHTED for pressure, PISO for pressure velocity coupling (skewness correction=0, neighbour correction=1, turn off the skewness neighbor coupling), FIRST ORDER UPWIND for momentum.

-once you initialize the flow field create an adaption register for patching the initial fluid location (adapt>region, then patch the liquid volume fraction solve>initialise>patch, select the volume fraction of the liquid as 1)

-keep your time step quite small. On using the NITA algorithm for time advancement there's a little debate...

Hope this helps, let me know if you need more hints

  Reply With Quote

Old   July 29, 2005, 13:33
Default Re: HELP.......sloshing problem using VOF
Posts: n/a
************************************************** *

Hi edi ghirardi

great, if you could help with udfs. In my case a can filled with liquid and 3% air is shaked. This all stands to simulate better heat transfer under shaked (forced) convection.

The can is shaked like a piston-crankshaft mounting. where i have w=omega=angel velocity crankshaft

function for ax is: a= w^2*sin(w*t)

w=17.6 1/s

under fluent support solution 838 i find a nice solution how to solve under time-changing accerleration with *.scm and input.txt files, which works for several accerleration lines. But in my case i have a simulation over 10min whith 200000 acceleration lines. fluent reads them but gets totally this solution is only for a couple of lines

a udf would be much better where every time step x-acceleration is calculated.

would be happy about any help with an udf

regards optixxx
  Reply With Quote

Old   August 11, 2005, 13:32
Default Re: HELP.......sloshing problem using VOF
Posts: n/a
Hi edi ghirardi

if you could help with pressure inlet boundary condition udfs(pressure is increasing with height of the water) and from which zone it has to initialized, from all zones or air zone only. If any idea about simulation of water waves free surface over the hydrofoils. Getting fine result when i take domain as a wall but could not understand about---how to define air and water inlet boundary b'coz water pressure is increasing with height).

Thanks anil
  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
problem in VOF hamid1 FLUENT 7 February 5, 2011 01:32
Multiphase Convergence Problem using VOF in ANSYS 13 FLUENT 1 January 28, 2011 03:22
Turbulent: VOF for reservoir problem prem FLUENT 0 March 30, 2006 10:44
Problem with VOF Jiri Novak FLUENT 1 March 17, 2006 06:13
problem with VOF. Marc FLUENT 1 June 5, 2002 08:17

All times are GMT -4. The time now is 22:55.