CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

Outlet Boundary Headache

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

LinkBack Thread Tools Display Modes
Old   November 17, 2005, 10:39
Default Outlet Boundary Headache
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?

  Reply With Quote

Old   November 18, 2005, 11:13
Default Re: Outlet Boundary Headache
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.

  Reply With Quote

Old   November 18, 2005, 12:32
Default Re: Outlet Boundary Headache
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.

  Reply With Quote


Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 49 Today 02:45
Outlet boundary setup for interFoam mittal OpenFOAM Running, Solving & CFD 2 July 14, 2010 08:59
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
Inlet & Outlet Boundary Conditions dhananjay Main CFD Forum 2 December 21, 2006 11:03
Inlet & Outlet Boundary Conditions dhananjay Main CFD Forum 0 December 18, 2006 03:51

All times are GMT -4. The time now is 15:58.