# free surface

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

 August 24, 2005, 12:15 free surface #1 Jennifer Haque Guest   Posts: n/a Hi, I am using CFX 5.7. From what I have read in the manual, it seems that the code uses interface capturing oppose to interface tracking. I wondered if anyone knew which interface capturing method it uses. It seems to me it is the scalar equation method. Can anyone confirm this? Jennifer

 August 24, 2005, 12:37 Re: free surface #2 Rui Guest   Posts: n/a Hi, For multiphase (n phases) flows, CFX uses the continuity equation of n-1 phases plus the total continuity equation. For free-surface flows, it uses the total continuity equation and the continuity equation of the primary fluid (the liquid). I suppose this last equation is what you call the scalar equation methodTo keep the interface sharp, as you can read on the Documentation (Solver Theory, Multiphase Theory, Free Surface Flow), CFX uses a compressive advection scheme, a compressive transient scheme and a special treatment of the pressure gradient and gravity terms (but I have no idea what is this special treatment) Regards, Rui

 August 25, 2005, 03:23 Re: free surface #3 test Guest   Posts: n/a The free surface model of CFX-5 is NOT an interface tracking method. No efforts are made in order to track or reconstruct the real interface between the 2 phases. The model in CFX-5 is a surface sharpening algorithm, a so-called "compressive scheme". If you consider the upwind method for the treatment of the convective terms in discretisation, you know that upwinding introduces additional numerical diffusivity to the solution process, commonly leading to a smearing of sharp gradients. The free surface model in CFX-5 is a special discretisation method for the convective terms, which is in contrary anti-diffusive, but with preservation of stability of the flow solver. So it acts against the smearing of sharp gradients as much as possible without loosing stability of the solution process. Free surface is detected everywhere where a grid cell is showing a steep gradient between gas volume fraction of 1.0 and liquid volume fraction of 1.0 in neighboring grid cells. Hope this helps. There are some conference papers which give a fair detail about the modelling approach. Contact your CFX support people to get these. Regards, test