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

Simulation a hydraulic jump

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

Like Tree4Likes
  • 1 Post By ghorrocks
  • 3 Post By Roland R

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 21, 2011, 20:47
Default Simulation a hydraulic jump
  #1
New Member
 
ABDULLA
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, 20:51
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,655
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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, 06:31
Default
  #3
Senior Member
 
Roland Rakos
Join Date: Mar 2009
Posts: 131
Rep Power: 17
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.

Regards;

Roland
BAZAN, Tae Su and aero_head like this.
Roland R is offline   Reply With Quote

Old   November 24, 2011, 09:02
Default
  #4
Member
 
Nirav
Join Date: Jul 2011
Posts: 43
Rep Power: 14
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
Default
  #5
Member
 
Ali Torbaty
Join Date: Jul 2009
Location: Sydney, Australia
Posts: 72
Rep Power: 16
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

Old   March 10, 2016, 06:45
Default
  #6
Senior Member
 
Join Date: Oct 2014
Posts: 124
Rep Power: 11
Ema40 is on a distinguished road
Dear AliTr,

I would like to ask you this. I can use the weir as you suggest, but there is a way to simulate an hydraulic jump without using a weir, but specifying the downstream water depth?? I tried in different ways, but the solution always diverged. The only way was to use a weir, as you said, but I would like to not use a weir.

Thank you
Ema40 is offline   Reply With Quote

Old   March 13, 2016, 17:40
Default
  #7
Member
 
Ali Torbaty
Join Date: Jul 2009
Location: Sydney, Australia
Posts: 72
Rep Power: 16
AliTr is on a distinguished road
Hi Ema40, You can do it without a weir as well, considering the outlet boundary is an open hydrostatic pressure BC (you need a simple CCL for it) , just initiate the model with downstream water level and let it drain. it won't diverge.
AliTr is offline   Reply With Quote

Old   March 14, 2016, 04:37
Default
  #8
Senior Member
 
Join Date: Oct 2014
Posts: 124
Rep Power: 11
Ema40 is on a distinguished road
Thank you!!
Ema40 is offline   Reply With Quote

Old   April 20, 2017, 10:48
Default Simulation a hydraulic jump
  #9
New Member
 
W.N.
Join Date: Apr 2017
Posts: 15
Rep Power: 8
W.N. is on a distinguished road
How to initiate the model with downstream water level?

Last edited by W.N.; April 20, 2017 at 15:11.
W.N. is offline   Reply With Quote

Old   March 8, 2020, 15:23
Lightbulb
  #10
Member
 
Rui
Join Date: Apr 2015
Location: Montreal. CA
Posts: 49
Rep Power: 10
roi247 is on a distinguished road
Quote:
Originally Posted by W.N. View Post
How to initiate the model with downstream water level?
in the 19 version of fluent, we can use the open channel model and pressure outlet boundary condition to specify water surface level
roi247 is offline   Reply With Quote

Old   March 10, 2020, 04:27
Default
  #11
Senior Member
 
karachun's Avatar
 
Join Date: Nov 2015
Posts: 244
Rep Power: 11
karachun is on a distinguished road
Make CFX Tutorial "Free Surface Flow Over a Bump". This tutorial contain a lot of useful information about free surface flow.
karachun 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
Why my simulation not agree with the wind tunnel experiment zhaowei CFX 4 July 11, 2015 04:36
Simulation of a complex wing in solidworks flow simulation niels1900 FloEFD, FloWorks & FloTHERM 6 April 20, 2011 11:44
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 19:57
Please Help ! Pressure Jump of Fan?? Boris FLUENT 0 January 28, 2003 21:26


All times are GMT -4. The time now is 03:09.