Hi all!

I want to build a model of jet flow, and it's water-air two phase model where water eject into air from inlet orifice. I build a rectangle which is big enough to keep it from impacting water jet flow and a inlet orifice with small radius, and these two are connected. As for boundary conditions, I set inlet orifice as Velocity Inlet where volume fraction of water is 1 and that of air is 0, and I also set some parts of the rectangle as Wall. But I don't know how to set the outlet. I think the outlet should allow the water to flow out without affecting it. The air is ideal gas which is compressible. Can somebody help me to tell me how to set the outlet or any hint about building the model? Thank you!

Benny

Hi benny, I am actually doing the exact same simulation 'impinging jet of water into an air domain'. I am using the VOF model and set the oulet BC as outflow. My solution is not completely converged yet . I am actually waiting to know what will happen when the jet will touch the wall. please Let me know what are your results thomas

hello Benny I think that if you set the BC on the outlet faces as pressure outlet then you may have better luck. By doing this you are allowing fluent to determine the pressure at the outlets (maybe ambient) before it begins calculating and therefore saving time in the case.

Justin

hello,

indeed a pressure outlet would give a quicker convergence than an outflow BC. Moreover it should be an unsteady calculation and care should be given to the time step close to the impinging zone in order to meet the convergence criteria.

David

Hi Justin, David and Thomas,

Thank you for your suggestion! I can see that pressure outlet will help the solution converge, but I don't know what the following,'Backflow Volume Fraction', means when I define the air at the Pressure Outlet. Thank you!

Benny

Hi Thomas,

I also use VOF model. Unfortunately, it's difficult for the solution to converge, and the Fluent stop automatically for unknown reason. I think myabe it's because I set wrong BCs. So would you tell me something about your modeling?

Benny

Hi benny,

My simualtion started pretty well to finally diverged. My boundary condition are outflow BC for the side exit and also for part of the doamin top the domain. My doamin is just like you a rectangle with a symmetry with a space on the top part for jet inlet. The problems I encountered are double. My characteristics are : jet diameter = 1.9 mm speed = 0.5 m/s height between wall and jet inlet = 6mm I am using the VOF model, laminar equation because of the folowing of the project, PISO, 1st order, default for convergence criteria and under-relaxation. My cell are quad with a 0.09 cell size. time step = 10^-5 s.

1 - My calculation diverged before my jet has touched the wall down. I have solved that problem by reducing my time step to 10^-5s. A bigger time step catch unphysical unstability at the jet inlet and creates vortex inside the domain and makes my simulation diverge.

2 - After solving that first problem, my fluid gets accumulate along the side exit. The report fluwes do not balance !!!. It is just like if the solver consider a wall BC instead of an outflow BC.

Further idea : I am gonna try maybe further IDEAS A - refine the mesh in the Jet path. B - starting the simulation with an intial jet patch in the domain. C - trying with lower jet velocity. D - Instead initializing the domain with air volume fraction = 1, maybe I will try to intialize with a doamain full of water to limitate the difference of density between the 2 phase at the beginning of the simulation.

This is where I am, i wish to work a bit more on it but I have not a lot of time for it . cheers, thomas

PS: maybe a PSG hooligan can help us ahaha .

Hi Thomas,

Now I got a satisfied result, though it is needed be refined. The solution is converged, but the Report Flux is not balanced, too. Maybe this is because that water flowing from the inlet and need some time to flow out of the outlet, which causes some quantities of water remainding in the domain.

In my case, I enabled Animation before Iterating, so I can exam the process of convergence. During the calculation, I can find that before the water reached the outlet, it converged well; after that, there were some reverse flow on the outlet.

I think if your want to study the effect of impact of water on the wall, you need set your wall wide enough to exam it.

Good luck!

Benny

[Robert@cfd]

Hi Folks!

Old thread, but same problem. I want to simulate water-walljet into an air-domain. I modeled an axisymmetric (2D) and unsteady case. Inlet is 3mm with 10 m/s but I am also trying slower inlet-jets. The outlet and the farfield-air is set to pressure-bc.

My computation converges (while using geo-reconstruct for the VOF-solver is unstable for me, so I work with Modified HRIC) but it seems I got problems with my model. So the hydraulic jump in the water film develops but when the water reaches the outlet the film collaps and in a highly transient behaviour the physics (water impact -> thin film -> hydraulic jump -> thick film) is resetting. The surface of the problem should be pretty constant in a converged solution so I am having big problems in getting a good result.

Hope you get what I mean and can help me. If you need more input-data, I will post it later.

Greetings,
Robert

[Robert@cfd]

Btw I used VOF explicit with kw-SST turbulence model and gravitational force. I use wall adhesion for the phase interaction. For pressure-velocity-coupling I use SIMPLE, but also tried Coupled. For pressure PRESTO!, momentum QUICK and Second Order Upwind for turbulence. Time is modeled with first order implicit (transient).

I did try the VOF plus level-set, but this isn't giving me the hydraulic jump at all. The water is leaving the domain only through the farfield boundary here. Should I try the Open Channel option? I am not really aware of what this changes.

[sdfarahani]

Dear friends
I want to model slot jet in gambit and solve in fluent. for laminar flow, reverse flow is occurred. width nozzle=7mm,H/w=5,target plate is 250mm. have I mistake in modeling ? please, guide me.
Thanks

[Mohawk]

Use pressure outlet boundary condition

[sdfarahani]

Dear Mohwak
I used this condition but reverse flow is occurred. Should I be considered length of impingement plate great then 250mm(for example 1000) for modeling?
Thanks

[sdfarahani]

I have another question. pressure in inlet is 2barg and pressure in outlet is atmospher. How to simulate this condition?
Thanks

[Mohawk]

Which model you have used?

[sdfarahani]

I used velocity inlet.laminar flow

[Mohawk]

My advice is to use k epsilon and put pressure in inlet also I just run a case and everything is okay

[sdfarahani]

okay. length of plate?

[Mohawk]

Doesn't matter