CFD Online Logo CFD Online URL
Home > Forums > CFX

Simulation a hydraulic jump

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

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By Roland R

LinkBack Thread Tools Display Modes
Old   May 21, 2011, 19:47
Default Simulation a hydraulic jump
New Member
Join Date: May 2011
Posts: 1
Rep Power: 0
BAZAN is on a distinguished road
Hi All
I am a PhD student at the University of Plymouth and I am using ANSYS-CFX-12 to simulate a hydraulic jump in an open channel. Is it possible for you to provide me some instruction on how to set up outlet boundary conditions for this case? I would like to use thebulk mass flow rate boundary option for the outlet boundary and am would like advise on whether I need to specify sources and how to do this. I have tried using this boundary condition for free surface flow in an open channel (using the VoF method) and it works well if I select laminar flow, but when I select a turbulence model, such as k-e, then the calculation does not converge.

I will be very grateful for your help with directing me to a suitable tutorial or advising me on what to enter if anything under the boundary condition->outlet->bulk mass flow rate sources tab. If helpful, I would be happy to send you the CFX Pre input file.
BAZAN is offline   Reply With Quote

Old   May 22, 2011, 19:51
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,053
Rep Power: 86
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Strange, it is rare for 2-eqn turbulence models to cause divergence. I suspect you have some problem causing this.

If you are having problems with the boundaries currently defined then move the outlet downstream further. This is especially useful if then you can add features (eg a large pond so the flow settles out) where simpler boundary conditions can be applied at the exit of the pond.
BAZAN likes this.
ghorrocks is offline   Reply With Quote

Old   May 23, 2011, 05:31
Senior Member
Roland Rakos
Join Date: Mar 2009
Posts: 122
Rep Power: 8
Roland R is on a distinguished road
Hello Bazan,

The hydraulic jump is a very interesting theme in terms of CFD simulation. When I was a student I completed a lot of free surface flow simulations which contained hydraulic jump.
During my measurements I measured the deep of the water in the channel from start to end in some points. I measured the main parameters of the hydraulic jump. Finally I validated these datas with simulation. I defined hydrostatic pressure distribution at inlet and outlet (based on the measurements) but it is important that the measurement has to be very exact! If you don't define deep of the water according to the measurements exactly then the simulation will not converge. (Just 1-2mm difference from the measurement and you will meet convergence problem). You have to apply very fine mesh in region of the hydraulic jump, and you have to generate structured haxa mesh (if it's possible). Based on my experience application of the tetra mesh is not suitable in case of free surface flows. I applied SST turbulence model.


BAZAN likes this.
Roland R is offline   Reply With Quote

Old   November 24, 2011, 09:02
Join Date: Jul 2011
Posts: 42
Rep Power: 6
niravtm007 is on a distinguished road
Send a message via Skype™ to niravtm007
thanks ronald, can you send me any of your tutorials how you simulated hydraulic jump presently in my project i need to develop your copy will be of gret guidance. hoping for positive reponse
niravtm007 is offline   Reply With Quote

Old   November 25, 2011, 22:01
Ali Torbaty
Join Date: Jul 2009
Location: Sydney, Australia
Posts: 71
Rep Power: 8
AliTr is on a distinguished road
firstly, to create and control a hydraulic jump you need to define the downstream water level. so put a weir somewhere before the outlet and define the outlet as an Open boundary (I assume you don't care about what happens after the weir)

secondly, Initialize the domain with downstream (subcritical) water level, then run it and let it drain. this prevent that initial numerical divergence in these sort of multiphase models.
AliTr is offline   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
Why my simulation not agree with the wind tunnel experiment zhaowei CFX 4 July 11, 2015 03:36
Simulation of a complex wing in solidworks flow simulation niels1900 FloEFD, FloWorks & FloTHERM 6 April 20, 2011 10:44
GUI crash and simulation engine still running RPJones FLOW-3D 2 November 9, 2010 09:18
velocity profile export from a simulation onto another sudhirlv STAR-CCM+ 1 September 12, 2010 18:57
Please Help ! Pressure Jump of Fan?? Boris FLUENT 0 January 28, 2003 21:26

All times are GMT -4. The time now is 19:59.