Hi, I'm fairly new to CFD, but have embarked on a university project so I'm having to take things on trust rather than develop a full understanding behind the theory, so I'd really appreciate so help, in laymans terms!

I'm trying to model a free surface (water:air) flow in an open channel, over a cylinder. I'm using Volume of Fluid. Dimensions are of the order 1m, and flow rate approx 1m/s.

The boundary conditions are: velocity inlet, pressure outlet, walls top and bottom and initial volume fraction 0.5:0.5.

time step 0.01s (and also 0.001s) and 200 iterations per timestep. Residuals converge after about 100 iterations.

The problems I've encountered are wierd reflecting waves off the rear boundary, and, more importantly, a very dissipative water-air interface. The distance between pure air and pure water is about 0.4m, whereas I had expected it to be just one element width.

Any suggestions?

200 it per time step? I have never needed such a number. It is to much. Better to decrease timestep.By the way, sorry, but I didnot undestand your geometry and flow character.

Bye, John

OK, I will decrease the number of iterations. What timestep would you recommend? 0.001s?

The problem is 2-D, and models a horizontal cylinder of diameter 0.24m in a flow, 0.06m above the bottom. The domain extends 1m upstream, 4m downstream, and 1m high. I'd like the free surface to be about 0.5m above the cylinder.

Thanks

Gareth

Hi, I think there should be no problem. Your task sounds quite easily. (are you using Geo-reconstruct scheme? are you sure about your boundary conditions? gravity? etc.) A width of interface also depends on mesh quality. Are cells fine enough? Anyway, I still cannot understand your task. If you wanted, you would send me description in more details (bohacek.jan@gmail.com) (figure,dimensions, BC,..) Otherwise, Good Luck!! John

Hello again, I'm still having some problems with this. I have tried all sorts of boundary conditions, but i think the problem is in the solver rather than the conditions. Even with a timestep 1e-5 the air-water interface still is not a thin line but is very dissipative. Are there any particular settings to be made in the solver options? thanks Gareth

for sharpener interface choose modified HRIC discretization for volume fraction eq.

Perhaps you should change your initial condition for the volume fraction of water. 0.5 is not a physical value but only a way to model the interface between air and water. For the initialization, you should only affect 0 or 1 for the volume fraction of water, not 0.5. It may be necessary to change your mesh in Gambit to define the initial volume of water and the initial volume of air. Then, you can affect in Fleunt the value 1 for the volume of water, and 0 for the volume of air.

If it does not change anything, you can decrease the under-relaxation factor of the VOF equation. For my own experience, the under-relaxation factors must be small when the VOF model is used: generally 0.1.

It sounds like you are solving a nano-scale problem...

If you still have the problem you could check if the scale in Fluent is the same as in Gambit.

(Grid -> Scale -> Grid was created in … )

The blurring is somewhat unavoidable numerical diffusion of the phase. mHRIC works well but will may give you some blurring still if the mesh is poorly aligned for the interface/flow and/or contains lots of unstrucutred regions. Try CICSAM if georeconstruct is giving you issues - or if looking for a s.state solution solve to convergence using HRIC then run georeconstruct with low # interations per cycle and small time step to sharpen.