density current-outlet boundary condition
 

I want to simulate an open-channel flow that at the begining of my experience has only water and air. The experience begins with the injection of a mixture of water and sediments into this channel. I have a device that allows the water height to remains constant. I would like to know your opinion about:

-As i am not interested in modeling the air part i am modeling the free surface with a free slip boundary condition. Agree?
-At the outlet boundary condition i am using the option average static pressure, with relative pressure=0 and the pressure profile blend=0.05 (average over whole outlet). Agree?
Best Regards

No. A pressure boundary is better, as the pressure at the free surface is atmospheric (assuming surface tension is insignificant).

As long as it represents what you are trying to model it sounds good.

Hi Glenn.
In what relates my top boundary condition i will try to check your suggestion. CFX is computing a recirculation zone in the top of my domain that was not supposed to be there and I want to check if it´s possible to improve my results in this zone.

In what concerns my outlet boundary condition, in my experimental setup, I have initially an hydrostatic pressure distribution in the outlet (just clean water) but then, when I inject the mixture (water+sediments) the pressure distribution ceases to be hydrostatic...Also the sediments and the water that left the domain are captured by a feedback circuit. I have choosen the option average static pressure, with relative pressure=0 and the pressure profile blend=0.05 (average over whole outlet) because it seemed to be the most appropriate for me.

Do you consider this is the best way of modeling the outlet ? I am having some difficulties with my results so I need to check all details. Thanks.
Regards.

Glenn, in what concerns the top boundary condition, you were referring to a condition of "opening" type?Such as in the free surface over a bump tutorial?

Yes, an opening.

If you are having troubles with your outlet boundary then move it further downstream.

Glenn, but if I put an opening boundary condition it may happen that the fluid goes out of my domain...and in my experience the water level remains constant.Furthermore it could be even harder to get convergence. Do you agree with my comment?
I have tried to implement a symmetry boundary at the top of the domain but i have received a very strange error.

Also, do you think that a no-slip wall will be an option for my top boundary condition. As i have said I am having negative velocities at the top of my domain that should be approximately = zero(at the moment i am using a free slip wall)

If you are happy to run this model as a multiphase free surface model then you can let the simulation sort out the interface. But if the free surface is simple you can simplify your model down to a single phase model with a pressure boundary as the free surface. Why a pressure boundary? Because the best description of a free surface (in most cases) is that it is at atmospheric pressure. This does mean a small amount of flow will probably go in or out of the boundary but this is an approximation of the system so you would expect some deviation. It is up to you to determine whether this simplification is acceptable or not.

The alternative (a free slip boundary) means that the pressure will vary along the interface.

If you want to use the single phase approximation you then need to choose whether the correct pressure but small flow across the interface (ie the pressure approach) or the wrong pressure but no flow across the interface (ie the free slip boundary approach) is best.