CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   sloshing simulation (http://www.cfd-online.com/Forums/fluent/36373-sloshing-simulation.html)

nabeel mohsin April 13, 2005 11:18

sloshing simulation
 
hi everybody i am doing simulation of sloshing effect of moving cylinder filled 90 percent with water and remaining air can any body help in this regard i am using vof any help no rotational velocity is given in this simulatio can any body tell me thanks in advance and plz answer quickly nabeel mohsin

edi ghirardi April 14, 2005 07:04

Re: sloshing simulation
 
Well,

-solver>unsteady>1st order implicit -multiphase>VOF>implicit body force ON -if you have baffles inside, SLIT THEM! -set the lighter phase as phase-1 OP CONDITIONS -turn on gravity, be careful about the signs of the components -operating density, the one of the lighter phase -pressure location: a point where the lighter phase is. SOLUTION -U-R Factors: pressure 0.6 momentum 0.8, 1 the others. -discretization: body force weighted for pressure, PISO for pressure velocity coupling (PISO parameters: skewness correction 0, neighbor correction 1), first order upwind for momentum.

initialize the flow field, and then

-adapt>region set the coordinates where water is and click mark. -solve>initialize>patch: under phase choose water, under variable volume fraction, under value 1, under registers to patch the region you marked, than patch.

Basically that's what is it.

hope it helps,

Edi.


All times are GMT -4. The time now is 15:35.