CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

precise water / air boundary

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 19, 2012, 10:16
Default precise water / air boundary
  #1
New Member
 
Heinz Mutzner
Join Date: Jul 2012
Posts: 6
Rep Power: 4
heinz is on a distinguished road
I just succeeded in doing the 2d bump tutorial.

Now, I would like to calculate a more precise water / air boundary. At the moment, it looks like a continuum over 4 mm height.

I would appreciate some hints on the relevant parameters. I already increased the max number of refinement steps in the mesh adaption menu of cfx pre. This didn't give any significant change.

Cheers

Heinz
heinz is offline   Reply With Quote

Old   August 19, 2012, 19:20
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,434
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The best way to improve resolution of the free surface is to use a finer mesh in the region of the free surface. I prefer a fine fixed mesh and adaptive mesh refinement has never worked for me with free surfaces very well.
ghorrocks is offline   Reply With Quote

Old   August 21, 2012, 21:41
Default
  #3
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 439
Rep Power: 8
evcelica is on a distinguished road
Not sure on this, but I seem to remember using a specified blend factor of 1 will aid in separating the two fluids more precisely (less smearing) since it is true second order; feel free to call my bluff anyone.....
Glenn is absolutely correct though, as usual, a finer mesh will of course give you finer resolution.
evcelica is offline   Reply With Quote

Old   August 22, 2012, 04:04
Default
  #4
Member
 
Dynampally Pavitran
Join Date: Mar 2010
Location: India
Posts: 72
Rep Power: 6
pavitran is on a distinguished road
Quote:
Originally Posted by evcelica View Post
Not sure on this, but I seem to remember using a specified blend factor of 1 will aid in separating the two fluids more precisely (less smearing) since it is true second order; feel free to call my bluff anyone.....
Glenn is absolutely correct though, as usual, a finer mesh will of course give you finer resolution.
The volume fraction equation uses high resolution scheme, unless the global advection scheme is set to upwind.

More information on this can be found in CFX Modeling guide --> Advection scheme.


I would like to know, What is the effect, when the partition (while solving in parallel mode) lies along the Free surface?

Sometimes, I have observed that the solver crashes due to build up of unphysical values of Eddy viscosity at the partition zone.
pavitran is offline   Reply With Quote

Old   August 22, 2012, 06:45
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,434
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I'll call your bluff Erik

For free surface models you should use the default compressive scheme for the volume fraction equation. This scheme is specifically designed to capture sharp interfaces and no other schemes will work well at all. For the momentum equations use whatever scheme is sensible - hybrid (with a large blend factor) or high res are the normal choices.

You should try to avoid havign partition boundaries lying along the free surface. This can cause convergence difficulties. You might need to define a partitioning algorithm to avoid this happening.
ghorrocks is offline   Reply With Quote

Old   August 23, 2012, 22:40
Default
  #6
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 439
Rep Power: 8
evcelica is on a distinguished road
Yeah, I don't know where I heard that. I thought a read it somewhere but it was a long time ago. Thanks for correcting me.
evcelica is offline   Reply With Quote

Reply

Tags
cfx, free surface flow, open channel flow

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
Water subcooled boiling Attesz CFX 7 January 5, 2013 03:32
Simulating A water bubble in air with periodic boundary condition cubicmatrixist Main CFD Forum 0 October 14, 2010 12:26
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05
Solver error message!!! IoSa CFX 1 September 14, 2006 04:48
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 15:55


All times are GMT -4. The time now is 23:04.