Dear friend, I am investigating the use of the Volume of fluid method for the simulation of the free surface of flow in a shallow open channel. I have been able to seperate the vel. inlet into two parts to give myself an initial air inlet and then a water inlet at the bottom and am using the PISO function so that the under relaxation factors can be set to one. However, I am having great difficulty in gettin my solution to converge and have found that I am not sure what time step settings to enter.

In this way, any advice or hints that you could give would be greatly appreciated.

Thanks

Hi Nial, Unfortunately Fluent uses an explicit time discretization for the advection of the volume fraction equation. This means that the stability of your solution is mainly determined by the Courant-Number of your problem, i.e. by velocity*timestep/gridspacing. If this number exceeds 1 the algorithm becomes unstable, for practical applications the limit is even lower: ~ 0.5. So usually you will have to use very small timesteps. Hope this helps, there are some remarks in the fluent documentation about this topic too. markus

Use following command in text mode-

(rpsetvar 'md/verbosity 2)

and check the VOF subtimestep should not b more than 4 . If they heigher then reduce the timestep.

Hope this help.

hallo, I am working with VOF model and I get some solutions for wetting of a complex geometry. The folloing suggestions are worthfull:

* mean Cell size 0.2^3 mm to 0.5^3 mm * initial the solution only with 0 values for all variables (also VOF) * use the ddp (double presision version) * body forces weighted, simple and first order upwind for the descritizations: * Geo-reconstruct and Courant No. 0.25, activate solve vof every iteration and implicit body forces. * Multigrid controls, pressure, termination 0.001 instead of 0.1 * hexaherdral cells * reorder domain multitimes and zones one time * time step 0.00005 to 0.00001 * 10 iterations per step and 0.005 residuals for the comtinuity at first then change to 0.0002.

I hope that will help you and good luck

Ataki

Are u using a coupled Solver ?

hi I am using the VOF for tracking the interface between two phase (free flow). It is segregated solver. The coupled solver is not combatible with this multiphase flow model in Fluent. Best wishes Ataki

hallo again, any comment, suggestion or information is wellcome. Thanks