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

Free Surface Flow: Length of Interface?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 29, 2005, 16:45
Default Free Surface Flow: Length of Interface?
  #1
Chebeba
Guest
 
Posts: n/a
I am playing around with analyzing performance of a sailboat hull using the homogenous free surface model. I've gotten grips on most things, but one thing bothers me: The Water/Air interface is more than a meter wide, even where there is no turbulence at all. (I am using "Interface Compression = 2").

Anyone here with experience on how this influences the accuracy of my results?

/C

  Reply With Quote

Old   November 30, 2005, 03:40
Default Re: Free Surface Flow: Length of Interface?
  #2
Charles
Guest
 
Posts: n/a
You are never going to do it with a grid like that. You need very fine resolution normal to the water surface, something like 10 mm or so. It won't work with a tetrahedral grid. You might make it work with prism layers, but the answer is to use a hexahedral grid.

Charles

  Reply With Quote

Old   November 30, 2005, 06:13
Default Re: Free Surface Flow: Length of Interface?
  #3
Chebeba
Guest
 
Posts: n/a
Well I could feel that comment coming, that's why I included the mesh in the picture ;-)

The next question then is how to create such a mesh? I am using an inflated boundary around the hull regions to create the boundary mesh needed by the SST turbulence model. This boundary is very thin (resolution ~1mm). So I can't apply the same inflation to the water surface region. But it seems not to be possible to specify two different sets of Inflation parameters, only several surfacegroups using one set of parameters.

/C
  Reply With Quote

Old   November 30, 2005, 09:57
Default Re: Free Surface Flow: Length of Interface?
  #4
Rui
Guest
 
Posts: n/a
Hi,

Perhaps you could use mesh adaption as in Tutorial 7 (Free Surface Flow Over a Bump)

By the way, what actually is "Interface Compression"? I think it wasn't available in CFX-5.7.1. Does it have something to do with the compressive advection scheme?

Regards,

Rui
  Reply With Quote

Old   November 30, 2005, 16:56
Default Re: Free Surface Flow: Length of Interface?
  #5
Chebeba
Guest
 
Posts: n/a
No idea, but the manual says to set it = 2 if the fluid interface is too spread out It did improve...
  Reply With Quote

Old   December 1, 2005, 00:30
Default Re: Free Surface Flow: Length of Interface?
  #6
Neale
Guest
 
Posts: n/a
To improve your mesh you could put a subdomain boundary "around" the region you expect the free surface to be located. Then inflate off of that in both directions. Inflation does not have to be off of no-slip wall boundary conditions only.

This is only really useful though if the free surface ultimately conforms to an expected shape.

Neale.
  Reply With Quote

Reply

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
Free surface flow settubg boundary conditions and plotting velocity profiles prashanthreddyh FLUENT 1 December 2, 2009 12:06
Multiphase flow. Dispersed and free surface model Luis CFX 8 May 29, 2007 18:13
How to determine delta t for free surface flow phsieh2005 Main CFD Forum 0 September 14, 2005 11:52
incompressible free surface flow past cylinder vineet FLUENT 2 April 1, 2002 05:56
CFX4.3 -build analysis form Chie Min CFX 5 July 12, 2001 23:19


All times are GMT -4. The time now is 04:42.