CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   HELP.......sloshing problem using VOF (

suryakant July 26, 2005 07:04

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

edi ghirardi July 27, 2005 06:29

Re: HELP.......sloshing problem using VOF
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


Optixxx July 29, 2005 13:33

Re: HELP.......sloshing problem using VOF
************************************************** *

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

anil August 11, 2005 13:32

Re: HELP.......sloshing problem using VOF
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

All times are GMT -4. The time now is 06:15.