CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Simulation a hydraulic jump (

BAZAN May 21, 2011 19:47

Simulation a hydraulic jump
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.

ghorrocks May 22, 2011 19:51

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.

Roland R May 23, 2011 05:31

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.



niravtm007 November 24, 2011 09:02

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

AliTr November 25, 2011 22:01

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.

Ema40 March 10, 2016 06:45

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

AliTr March 13, 2016 17:40

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.

Ema40 March 14, 2016 04:37

Thank you!!

W.N. April 20, 2017 09:48

Simulation a hydraulic jump
How to initiate the model with downstream water level?

All times are GMT -4. The time now is 12:46.