CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT > Fluent Multiphase

VOF: Sharp Interface

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 12, 2014, 06:58
Default VOF: Sharp Interface
  #1
New Member
 
Jan Galijasevic
Join Date: Mar 2014
Posts: 5
Rep Power: 8
Jan90 is on a distinguished road
Hello,

I am simulating in 2D an injection of water in a tank filled with oil through a circle on the left (velocity inlet). The right circle is producing just oil (negative velocity inlet).

My questions: Why am I missing a sharpt interface while using the VOF method? There should not be a green zone. (red is oil and blue is water)

Thanks

Jan90 is offline   Reply With Quote

Old   May 21, 2014, 20:29
Default
  #2
New Member
 
Sean Delfel
Join Date: Aug 2009
Posts: 27
Rep Power: 13
delfel is on a distinguished road
Quote:
Originally Posted by Jan90 View Post
Hello,

I am simulating in 2D an injection of water in a tank filled with oil through a circle on the left (velocity inlet). The right circle is producing just oil (negative velocity inlet).

My questions: Why am I missing a sharpt interface while using the VOF method? There should not be a green zone. (red is oil and blue is water)

Thanks

Hi there,

Do you have any more details on the schemes you are using? In general, my recommendations would be to a) use a better volume fraction scheme to reduce numerical diffusion (I tend to prefer compressive or BGM for sharp interfaces), b) adapt and improve the grid resolution at the interface, c) run the simulation transient as your jet may be causing entrainment between the two fluids.

Hope that helps.
delfel is offline   Reply With Quote

Old   May 29, 2014, 23:02
Default
  #3
New Member
 
赵后剑
Join Date: May 2014
Posts: 1
Rep Power: 0
Bob-zhao is on a distinguished road
Quote:
Originally Posted by Jan90 View Post
Hello,

I am simulating in 2D an injection of water in a tank filled with oil through a circle on the left (velocity inlet). The right circle is producing just oil (negative velocity inlet).

My questions: Why am I missing a sharpt interface while using the VOF method? There should not be a green zone. (red is oil and blue is water)

Thanks

Hi,here:
Could you tell me when you are setting the VOF model,you choose the explicit or the implicit? In my opinion, if you want to see the sharp interface,
choose the "explicit".
Bob-zhao is offline   Reply With Quote

Old   May 29, 2014, 23:13
Default
  #4
New Member
 
Sean Delfel
Join Date: Aug 2009
Posts: 27
Rep Power: 13
delfel is on a distinguished road
Quote:
Originally Posted by Bob-zhao View Post
Hi,here:
Could you tell me when you are setting the VOF model,you choose the explicit or the implicit? In my opinion, if you want to see the sharp interface,
choose the "explicit".
Yes, I agree with Bob. Explicit geo reconstruct will ensure that you capture a sharp interface. It requires a small time step, however, and you may be able to get adequate results with an implicit scheme.
delfel is offline   Reply With Quote

Old   June 20, 2014, 09:36
Default
  #5
New Member
 
Jan Galijasevic
Join Date: Mar 2014
Posts: 5
Rep Power: 8
Jan90 is on a distinguished road
Thank you very much for the reply.

I am using VOF, Implicit Scheme and PISO Scheme, Least Squares Cell Based Gradient, PRESTO! Pressure, Second Order Upwind Momentum, Compressive Volume Fraction and First Order Upwind Turbulent Kinetic Energy.

I will try it with an explicit scheme.

Regards,

Jan
Jan90 is offline   Reply With Quote

Old   June 20, 2014, 23:48
Default
  #6
Member
 
Christopher Hershey
Join Date: Feb 2012
Location: East Lansing, Michigan
Posts: 41
Rep Power: 10
Hershey is on a distinguished road
If the viscosity of your two phases are also significantly different (an order of magnitude or more) then CICSAM is recommended with an explicit VOF model. Also, as delle pointed out, the sharpness of the interface is also a function of the mesh cell size. Make sure your mesh is refined in the area near the interface.
Hershey is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 58 July 3, 2020 02:13
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 11:53
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 07:28
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 08:00
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05


All times are GMT -4. The time now is 02:42.