hi all, How can I model sloshing in CFX?

thanx in advance

Set up two phases and use the free surface model.

You will also need to excite the fluid. To do this you will need to solve the simulation transiently and also need to move the body. The body movement will require the use of user fortran or you could wait till CFX5.7 where I think there is a GUI to do this (not 100% sure though !). Bob

Hi,

Mesh movement was in the 5.7 beta so it should be in the erlease version. You could also excite it by moving the gravity vector and this would not require mesh movement.

Regards, Glenn

Hi Glenn we toyed with this but collegues were convinced that this would not give the same result. However we were looking at the added mass of the water, and I believe by changing the gravity vector, you do not include this ? Alas I'm no expert, and had to go by their advice ! what are your thoughts ? Bob

Hi Bob,

I can't see why for a simple horizontal oscillation changing the gravity vector would not work. You would need to be careful in considering which frame of reference the force/moments/velocity/displacements are in, nut as long as you have got your brain around that I can't see why it would not work.

Just my thoughts.

Glenn

I've solved this very problem for a cylinder of water moving around a corner on a conveyor belt. We simply imparted an additional gravitational accelleration that changed direction with time as the centrifugal force was applied and then removed after the total travel time in the curve.

CFX takes care of the mass for you by imparting the body forces as long as buoyancy is on. You may want to make sure you set your reference density to that of the light phase (air above) which will deliver the appropriate hydrostatic head in the liquid.

I don't think there's a problem with this technique at all. And it is MUCH easier than moving the grid.

Jeff

but how can I define the volume fraction of water and air inside the tank?? I don't have inlet or outlet.

Using your initial conditions.

Use CEL to set the vf for liquid to 1.0 below a specified height (say z level) and 0.0 for everything above. Opposite for gas....

CEL EXPRESSIONS

z_inerface = 5.0 [in] # liquid level height

vf_liquid = step(z_interface-z)*1.0

vf_gas = 1.0 - vf_liquid END END

This sets liquide vol. frac. to 1.0 for all nodes below z_interface and 0.0 above interface. In your Initial Condition for Volume Fraction use the CEL variables vf_liquid and vf_gas.

Hope this helps, Jeff