# sloshing

 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 13, 2004, 03:23 sloshing #1 Zaher Guest   Posts: n/a hi all, How can I model sloshing in CFX? thanx in advance

 March 13, 2004, 16:39 Re: sloshing #2 Jeff Guest   Posts: n/a Set up two phases and use the free surface model.

 March 14, 2004, 06:39 Re: sloshing #3 Bob Guest   Posts: n/a 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

 March 14, 2004, 17:33 Re: sloshing #4 Glenn Horrocks Guest   Posts: n/a 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

 March 18, 2004, 07:54 Re: sloshing #5 Bob Guest   Posts: n/a 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

 March 18, 2004, 17:41 Re: sloshing #6 Glenn Horrocks Guest   Posts: n/a 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

 March 19, 2004, 18:29 Re: sloshing #7 Jeff Guest   Posts: n/a 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

 March 22, 2004, 00:26 Re: sloshing #8 Zaher Guest   Posts: n/a but how can I define the volume fraction of water and air inside the tank?? I don't have inlet or outlet.

 March 27, 2004, 18:02 Re: sloshing #9 Jeff Guest   Posts: n/a 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post satellite_control FLOW-3D 0 October 6, 2011 09:04 bearcat Main CFD Forum 7 August 5, 2011 20:13 satellite_control FLOW-3D 0 June 20, 2011 05:34 alastormoody11 STAR-CCM+ 0 January 20, 2011 23:40 D.Martelli Fluent UDF and Scheme Programming 0 December 9, 2009 12:21

All times are GMT -4. The time now is 18:30.