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. k-e 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 pressure-velocity 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

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 tri-tetra 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 time-dependant solutions, stable up to CFL=5 near the free surface; very time-consuming, but necessary if you are interested in evolutive-type 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 steady-type 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

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 pressure-velocity coupling choose PISO. For me it doesn't work with those modifications but I read it in the user-guide.

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,

[Rajaero]

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..

[hamed.majeed]

Originally Posted by Rajaero

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..

Probably you didn't export those variables for CFD post.
Solution>Calculation Activities>Create>Solution data Export.

Hope it helps.