
[Sponsors] 
May 25, 2007, 00:12 
plz help,urgent, vof model steady state

#1 
Guest
Posts: n/a

Dear Sir/Madam,
I had a query regarding staedy state solution of the vof_model given as 16 th example in tutorial guide of fluent. I tried it with a different geometry i.e. of a cylinder of radius 2 cm and height 8 cm. I filled it with water till a height of .03 m. I wanted a steady state solution of the problem instead of the unsteady state solution. But the problem what I am facing is that the solution doesnt converges at all even though I reduced the under relaxation parameters to 1/100 th of the initial values given by default.Still it will not converge after some time and there occurs a sharp rise i.e. vertical rise in the residual values and finally it shows an error.THe changes what I made from tutorial problem setting of vof_model of unsteady state to steady state are as follows: 1. unsteady state to steady state under solver 2. ke model to laminar model under viscous as I want to work first with the low rpm/sec i.e. till 2 rad/sec which gives a reynolds no in laminar region for this geometry of mine 3. Under solution controls I took the scheme SIMPLE under pressurevelocity coupling and under Discretization I took the scheme STANDARD 4.Under surface monitors I took Iteration for define instead of flow time Rest everything I kept same But I also tried with the presto scheme only instead of standard , though it gives convergence but it doesnt give any change in the profile of liquid in cylinder after iteration is over its still .03 m filled horizontal line no parabolic shape. Plz guide me I m not able to interpret whats the issue. Regards Garima 

May 25, 2007, 01:51 
Re: plz help,urgent, vof model steady state

#2 
Guest
Posts: n/a

First of all, for VOF you MUST use only Body Force Weighted or PRESTO schemes for pressure discretisation, prefferably BFW because it is more stable, even on tritetra meshes, and you need to activate "Implicit Body Force" option in the Multiphase GUI panel.
Second, unsteady VOF will ALWAYS be much more stable then steady formulation, and there are cases when it is almost impossible to obtain a converged solution using the steady implicit formulation. An example would be the supercritical (Fr>1) Open Channel flow, for which the steady approach is inapplicable, and one must use unsteady solver. There are three possible approaches to a VOF problem:  steady implicit formulation, suited for the cases where there is no interest but for the final state of the solution; difficult to converge, needs low URF, especially for momentum.  unsteady explicit, suited for accurate timedependant solutions, stable up to CFL=5 near the free surface; very timeconsuming, but necessary if you are interested in evolutivetype problems.  unsteady implicit, not as accurate as explicit, but for sufficiently small time steps (CFL no more then 10), applicable to evolutive problems, with some error expected (general evolution of the phenomena is well predicted, but all oscillations are smoothed); very stable, even when using large time steps (CFL>100), which makes it applicable to steadytype problems also. My favorite approach for steady problems is unsteady implicit formulation, because it allows me to obtain a solution much faster then with steady implicit. Example: for a free surface flow around a hull, steady implicit converges in 7000 iterations (2000 for the first order solution, 5000 for the second order solution), unsteady implicit converges in about 1000 iterations (with 5 iterations per timestep, 200 timesteps), ramping CFL from 1 at start to 100 (doubling it every 10 timesteps). I think this is quite an improvement! So my advice is to use unsteady implicit, first order time discretisation, with large timesteps. All the best, Razvan 

May 30, 2007, 04:38 
Re: plz help,urgent, vof model steady state

#3 
Guest
Posts: n/a

I have the same problem as you. In fact to choose a steady state model you have to choose the implicit VOF sheme. Then in solve >controls>solution, choose under relaxation factors between 0.2 and 0.5 chosse a body force weihted pressure and second order upwind for momentum, volume fraction...For pressurevelocity coupling choose PISO. For me it doesn't work with those modifications but I read it in the userguide.
If you find the right solution, please write te me and describe what you did. I will do it also if I find the right solution. faithfully yours, Marion, 

November 13, 2017, 02:35 

#4 
Member
Taiwan,new north city
Join Date: Aug 2017
Location: Taiwan
Posts: 74
Rep Power: 5 
hi guys.
i am doing vof model for water tank simulation in fluent. fluids used : air and water i did the setting according to tutorial. but in cfd post i could not find a phase1 (volume fraction) and phase 2 (Volume fraction). i dont know whats wrong. can somebody tell me whats wrong in cfd post? thanks in advance.. 

March 15, 2018, 12:22 

#5  
Senior Member
Hamed Abdul Majeed
Join Date: May 2012
Location: New Orleans, LA, US
Posts: 147
Rep Power: 10 
Quote:
Solution>Calculation Activities>Create>Solution data Export. Hope it helps. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
vof steady state  bene  FLUENT  1  October 14, 2010 12:11 
Is animation possible for Steady state model???  NI3  CFX  1  November 12, 2008 02:45 
urgent query regarding vof model plz rply  Garima Chaudhary  FLUENT  0  July 13, 2007 02:20 
VOF steady state?  CFD Newbie  Main CFD Forum  3  December 16, 2002 00:23 
About the difference between steady and unsteady problems  Lisa  Main CFD Forum  11  July 5, 2000 14:37 