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

 November 17, 2005, 10:39 Outlet Boundary Headache #1 Chebeba Guest   Posts: n/a I'm trying to model flow around a yacht hull, but having very little luck in getting water to flow out of my domain in a sensible way. No matter what I do, CFX insists on putting temporary walls in the outlet, to block inflow. I am using homogenous model, standard homogenous free surface model, standard air at 25 degrees and water. Two inlets: one 100% water below y=0, and one 100% air above y=0. Boyancy activated at (0, -9.81, 0), ref density 1.185 (air) and ref location (0,0,0). +Y is up in this model, water surface at y=0. The outlet is static pressure, with a CEL expression pressure profile: pOut = -997[kg m^-3]*g*y*step(-y/1[m]) I have tried using the same pOut as t=0 initial guess for the domain pressure, but that doesn't change anything. Anyone around who's been successful in anything similar? /c

 November 18, 2005, 11:13 Re: Outlet Boundary Headache #2 Jeff Guest   Posts: n/a CFX calculates the buoyancy force using (rho - rho_ref). Without subtracting rho_ref, your pressures will all be just slightly higher than the resulting hydrostatic head resulting in inflow. Try this: pOut = (Water at 25 C.density - Air at STP.density)*g*y*step(-y/1[m]) Using the actual phase densities also ensures you have "exactly" the density that CFX is pulling out of the database. Jeff

 November 18, 2005, 12:32 Re: Outlet Boundary Headache #3 Chebeba Guest   Posts: n/a Thanks a lot! I actually discovered that a reference location of (0,0,0) was not so smart, since that is exactly on the surface. Putting further up in the air solved the major problem, but your tip also made me loose the weird "dip" in the water surface I was getting at the outlet. /c

 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 Saturn CFX 45 February 8, 2016 05:42 mittal OpenFOAM Running, Solving & CFD 2 July 14, 2010 08:59 Pankaj CFX 9 November 23, 2009 05:05 dhananjay Main CFD Forum 2 December 21, 2006 11:03 dhananjay Main CFD Forum 0 December 18, 2006 03:51

All times are GMT -4. The time now is 14:29.