Dear Sirs, I want to study an asymmetric water free jet discharging into the air (like the one found in Cross-Flow hydraulic turbine), using CFD codes. In my case, the free jet geometry must came out as a result, since it is unknown at the beginning. There are methods for potential flow analysis, but I never found anything for viscous flow. I don't know if there are any CFD software packages that can handle this kind of problem. I emphasize that we don't know the free jet surface shape. It can be shown that the pressure is constant on the jet surface (and, therefore, the velocity is also constant). Although we know the nozzle geometry, the flow calculation inside this region must take into account the shape of the free jet, which is not known at the start. I thank in advance for any help given.

Dear Norberto

I doubt that the pressure on the interface remains contant when a jet enter into the surrounding atmosphere, even if the air is "at rest".

If the flow is viscous then you will have shear stresses and therefore, a spatial development of Kelvin-Helmholtz instabilities (maybe Rayleigh and Taylor intabilities), which are closely related to a pressure distribution on the inteface.

If you know the geometry of your nozzle just send the water into the computation domain by this arbitrary shape orifice. Track the interface and you will find the shape. That is what we do.

We (our group) works on liquid jets with and without air coflows, but I can't understand your last sentence. "the flow calculation inside this region must take into account the shape of the free jet, which is not known at the start". Please, be more clear if you can, and maybe we can help you a little.

Regards

Kike

Dear Kike, Thanks for your reply. It seems safe to conclude that your answer is based on the implicit suggestion that we should discretize the nozzle and turbine enclosure, and calculate the flow as a two-phase flow in this domain. In this way, it would be possible to study the jet breakdown, due to Kelvin-Helmholtz instabilities. However, this approach seems to be wasteful in terms of computational resources, since the jet would only occupy a small fraction of the entire computational space. Besides that, I am only interested in the region near the nozzle exit (where the rotor may be placed), which is a region where the jet has sharp boundaries, easily defined. The jet breakdown and the calculation of the air velocities have no interest at all for me. Therefore, if I follow your advice, I may end up with a lot of information which have no use for my purposes. My original question was motivated by my feeling that an alternative strategy may give better results. In this alternative approach, I would only discretize the region occupied by the water. This way of solving the problem raises the question that the boundaries of the free jet are not known during the discretization stage. These boundaries of the jet are determined by the condition that the pressure is constant throughout. In fact, the static pressure is constant in all the regions occupied by the air, to a very good approximation, since the air velocities are low (of the order of a few m/s). Since the boundary, by virtue of its definition, is in contact with the air it follows that its pressure must be constant. Returning to my original question, I was wondering whether, with a viscous CFD code, there is a simple way of imposing constant pressure along a boundary, and using this condition calculate the physical shape of the boundary. I thank in advance any help given by you about this topic.

(1). Most applications using Navier-Stokes code require the specification of the boundary conditions and the corresponding locations. (2). In your case, a model must be developed first to take the constant pressure as the boundary condition and the boundary location must be the part of the solution. (3). So, a method has to be developed first to do that. I don't know whether current commercial code can handle it or not. A code which can handle free surface might be a good place to start.

The commercial code FLOW-3D was originally developed for this kind of application. The company, Flow Science, is a sponser of this web site.

It's antecedents, SOLA-VOF, NASA-VOF/2D and NASA-VOF/3D also have a free service capability.

I have no relationship to this company.

Dear Norberto

OK, I thought you were interested in atomization, but I have not assumed at all you want to discretize all the turbine geometry to study the liquid jet dynamic. In your first message you had written "Although we know the nozzle geometry, the flow calculation inside this region must take into account the shape of the free jet, ...", and I suppose you want to study the same thing I studied in my PhD.: liquid sheets behind thick wall injectors.

Unfortunately, I will can't help you because I don't know how to handle a "constant pressure dynamical liquid-gas interface"; but I would like you help me to understand what is the instability-atomization mechanism you have in your turbine. It is just for professional curiosity.

As far as I know there are several atomization (I know, you had said you are not interested on it): high pressure jets, coflow assited, rotatory, ultrasound resonants systems. In all of them the pressure distribution on the interface is not constant.

Near the outlet, even at zero air velocity, you will have a pressure distribution along the axial coordinate. It allows the die-swel problem (low liquid velocity or high viscosities) in which the shape of the interface depends on liquid outlet velocity and contact angle dynamic. If the liquid outgoing velocity is high enough (I am sorry not to give an order of magnitude) the pressure have a singular behaivour behind the thick wall injector (your nozzle) and that is explained by a tripple-deck structure of the flow at the outlet.

I have studied the liquid sheet instability under the action of coflows with velocities between 5 and 100 m/s. with good agreement with experimental observations. I can confirm you that for low air velocities (and liquid outlet velocity of 1m/s) the pressure distribution on the interface (just behind the nozzle) is soft (low variations) but a sinusoidal function of the dowstream coordinate and, at a length about 10*sheet_thickness, the nonlinear effects turns this distribution into a very complex function.

"Dynamics of thin planar viscous liquid sheet in the presence of viscous gas coflows behind thick wall injectors"; C. Dopazo, E. Lopez-Pagés, N. Fueyo; Session of FN Interfacial and Thin-Film Instabilities III; 52nd. Annual Meeting of the Division of Flow Dynamics APS; New Orleans 1999.

"The instability of a thin liquid sheet between two parallel high-speed gas streams"; E. Lopez-Pagés, C. Dopazo and N Fueyo; V Latin American and Caribbean Congress on Fluid Mechanics; Caracas 2001.

To (maybe) ansuwer your first questions I had used PHOENICS, which is a well know powerfull and accurate commercial code (despite some people in this FORUM think). You can add to it your specific requirements via a wide-purpose subroutine. I can give you more details if you decide for this option.

Besides this, I think any CFD comercial code (FLUENT, CFX) can handle your problem with adaptative grids and high order schemes if you need them. The problem is that they ere expensive in most cases.

Dear colleague, I am sorry if I missunderstood your problem, I was trying to help.

Regards

Kike

dear Norberto,

Instead of knowing this phenomenon of asymmetric flow, I started with an experiment in which I evaluated the cross-sectional velocity-outflow distribution of a vertical vessel/scrubber with a horizontal internal vane type inlet separator. An airflow was injected sideways in the middle of the vessel through a pipe and was streaming through the inlet separator and diverted into the open air through the outlet of the vessel. Results showed that this flow distribution was asymmetric. For comparison with this result I used a CFD-code named FLUENT and the results showed the exact same outcome. The flow is considered only gas because the multi-phase flow which is normally inserted (oil, gas, water, solids) can be considered one-phase when the gas flow is flowing out of the vessel (particles that are not separated by the inlet separator and the gravity are still inside the gas stream but are negligible for the properties of this flow). You have to use a geometry (Which you can make in AUTOCAD, RHINOCEROS, or GAMBIT a.o.) and grid (make it in GAMBIT) and make sure that you have enough cells at the places where you expect a change in velocity. So make sure your grid is dense enough and smooth enough (in GAMBIT you can check your grid and mesh if it is suitable, use tetrahedical cells for your convenience) After this, make use of FLUENT to process your meshed grid. Set your boundary conditions, like inlet velocity, hydraulic diameter and turbulence intensity and pressure at the outflow level (use a pressure outlet). Make sure you use the right solver model for your flow...the standard k-epsilon model is proven accurate but not for all turbulent flows, when you have a strongly curved flow, and flow close to the wall you might consider LES (or Latice-Boltzman, but that model is not used in FLUENT). Remember however that the more cells you use in your grid and the more complex the solver model, the more time it takes to reach convergence and a good solution. My model consisted of 600,000 cells and it took 36 hours to reach convergence in FLUENT with the standard k-epsilon model. After solving the model, it is possible to substract many results, you can display the contours/vectors of the pressure for example and many more of each region or point in this region that you desire. See www.fluent.com for more information.

I hope that this elaborate discussion of my results can help you with your problem,

Regards, Marko van der Smitte

ps. do you have information about the origination of this asymmetric phenomenon? I suppose that it has to do with a difference in pressure gradients, but do not know the full story.

I have used (FIDAP) code to handle a Free Surface problem like this when I was simulating the fluid flow and heat transfer characteristics of a free liquid jet impinging on a hot plate.