Impinging Jet Modeling Problem
I am trying to model an impinging jet . There is a nozzle through which air is exiting vertically downwards and hitting the ground. I have two questions about it.
1) what would be the top boundary condition besides (next to) the inlet? Is it pressure or Inlet with zero U and V velocities? If I put Inlet condition bc there with zero U and V , then what values do I put for k and epsilon there ? 2) What are the values of inlet turbulent kinetic energies and dissipation which I need to specify for the inlet jet using kepsilon model? I am using both FLUENT and STARCD for analysis. Thanks 
Re: Impinging Jet Modeling Problem
Hi,
You could read the following two journal papers. Graham L. J. and Bremhorst, K., "Application of the ke turbulence model to the simulation of a fully pulsed free jet", Journal of Fluids Engg., 1993, 115, 7074. Craft, T., Graham, L. J. and Launder, B., " Impinging jet studies for turbulence model assessmentII. An examination of four turbulence models" Int. Journal of Heat and Mass Transfer, 1993, 36, 26852697. Cheers 
Re: Impinging Jet Modeling Problem
Anindya, check out this one: Smooth particle hydrodynamics simulation of surface coating. Reichel et al. (Applied Mathematical Modeling 22 (1998) 10371046. Its not STAR or FLUENT but it is an interesting model for jet impingment using SPH.
All the best. 
Re: Impinging Jet Modeling Problem
The top boundary can be treated as a fixedpressure boundary through which fluid may enter or leave, as dictated by local continuity during the solution. In the event of entrainment, negligible freestream turbulence is usually assumed in the absence of other information.
In the nozzle you can set k and ep values appropriate for fullydeveloped pipe flow (thus k = friction velocity squared and ep=0.1643*k**1.5/Lm), or simply presume a turbulent intensity of say 5% and then specify ep using this intensity and a mixing length Lm of say 10% of the nozzle radius. 
Re: Impinging Jet Modeling Problem
Thanks a lot Mahesh, Christian and Michael for your suggestions.
Michael.. I did try your suggestion. But the problem that I am having is that when I use pressure BC on teh top the horizontal velocities after impinging are much higher compared to the experimental values I have got. Also the normalized the pressure profile(wrt the highest pressure directly under the center of the jet) is not matching the experinetal profile. The computed profile is more than the experimental one. Again when I tried with inlet BC on top with zero U and V velocities, the velocities are little less ( though still not same as the experimental values), but the ground pressures (normalized as before)now are less compared to the experimental ones. I am wondering if it is because of the problem with the top boundary condition or the turbulence model or grid error ? I have checked with different grids and it gives the same result. For the inlet I have used experimental values of Turbulence intensity (about 1.5 %) and used Lm = 0.07D, where D is the dia of my jet. The velocity of my jet is 7 m/s. Thanks 
Re: Impinging Jet Modeling Problem
It is difficult to say what is reponsible for your discrepancies with measurement, as it could be a number of things. I have even known the measurements to be poor as when checked they did not satisfy the momentum balance, although this was for a plane wall jet experiment rather than a radial wall jet.
This flow (conditions as for Cooper experiment with H/D=6 ) was studied at the CFD95 conference in Canada, mainly in respect of the accuracy of the heat transfer predictions. The standard ke model does not perform well in the impingement zone (too much eddy viscosity), and so the Nusselt number distribution along the plate was poor. I used the LaunderYap correction for the nearwall lengthscale, both for a wallfunction and lowRe ke model solution. I used PHOENICS, but I recall that two sets of STAR solutions were reported in the CFD95 workshop report by Andrew Pollard ( Queens University report CFDSC/V/953, 1996). You do not say whether you use a highRe or lowRe model, but the mesh does need to be fine near the wall so as to resolve the radial wall jet, and this can be comprimised by the validity of the wallfunction treatment. I do not know what H/D is for your case, but if it is far enough away I would not have thought it would have a massive impact on the wall region whether a zero flux or zero pressure were prescribed at the top boundary. However, I favour the latter. When specifying the free stream turbulence I usually set ep so that enut=enul for the given very small value of k. There is also the question of securing complete convergence, especially with a lowRe model, as the k and e equations can be rather stiff in the nearwall region where fluid properties vary rapidly. 
Re: Impinging Jet Modeling Problem
(1). I would suggest that you set the Reynolds number at some numbers say Re based on the jet =100, and compute the flow field as a laminar case first. (2). This will eliminate the complication from the turbulence model. And you will be able to focus on the accuracy of the solution first. And also the various B.C. options available, with the impact on the solution. (3). Once you are convinced that the setup is all right, you can move on to the turbulent flow calculation.

Re: Impinging Jet Modeling Problem
Hi Michael... The Dia of my jet is 14 Inches and the height is 24 Inches. I used the High Re model. I ma having a pretty fine mesh near the impinging wall.

Re: Impinging Jet Modeling Problem
(1). Always try to duplicate the experimental B.C. first. (2). If the measurement requires zero U,V there, then set U,V to zero. (3). If the measurement requires constant pressure then use constant pressure there. (4). If in the experiment, the wall is located further back behind the jet exit plane, then simulate it there. (5). If you want to get accurate result, you may have to compute the nozzle internal flow as well, with inlet further upstream of the jet exit. (6). So, keep the boundary condition identical to the experiment setup, or keep inlet and exit further away from the point of interest.

Re: Impinging Jet Modeling Problem
The top horizontal boundary next to the inlet is just free air. No walls, etc . So I am in a dilemma as to what to choose ... another inlet with zero U and V or just pressure ? again both of these needs some value of k and e. I do know what values to substitute for them. Also for the vertical boundary on the right (left vertical bc is symmetry), I am using pressure as a bc. Again for this bc also, Fluent asks me to input some value of k and e about which I have no idea also.
I can only put the values of k and e for the top inlet as from experimental values I know turbulence intensity and knowing the dia of the jet I can choose a hydraulic diameter for the length scale. 
Re: Impinging Jet Modeling Problem
(1). You can not specify the boundary condition at the jet exit plane, because that is too close to the point of interest. (2). You can consider another case of a long vertical pipe in a large room. The top wall is very far away from the jet exit, and the room wall is far away from the centerline. for example, the top wall is 10feet from the jet exit, and the side wall is also 10feet from the centerline. on the side wall, you can have the exit duct with 5feet height. (3). In this way, the air enter the pipe from the ceiling of the wall and exit at the jet exit. and the room is confined by the walls, with a side exit on the side wall. (4). In this way, you can apply the downstream B.C. at the end of the exit duct. The jet exit(inlet condition) remain the same (you could move it further upstream in the pipe). The rest is just the wall boundary condition. This should give you a free jet impinging condition. And you no longer have to worry about the jet exit plane top boundary condition. (it is too close to the bottom wall, and should be the part of the unknown solution rather than the boundary condition itself.) (5). So, you problem is very simple. (6). On the other hand, you can place a solid wall at the jet exit plane(top wall), and run the calculation and the test. There is nothing wrong this way. (7). When you move the inlet upstream of the jet exit in the pipe, you will capture the real jet exit velocity profile, which is nonuniform and is important in the subsequent wakejet flow development before impingement .

Re: Impinging Jet Modeling Problem
If the mesh is very fine near the wall and you are using wall functions, then you are probably violating the wallfunction formulae. What is the value of y+ near the wall? If it is less than 11.5, then the b.c.'s used for k and e by the wall functions are invalid.
However, more influential is probably the tendency for the ke model to overestimate the eddy viscosity in the impingement zone. This is likely to influence the pressure distribution along the plate. The LaunderYap or KatoLaunder variants of the ke model do much better for impinging flows. If you are using Fluent or star, surely they have other suitable variants of the ke model as options. All this presumes your present solution is fully converged. For example, for each momentum equation, are the absolute wholefield sum of the residual errors below say 1% of the incoming jet momentum? As long as the entrained values of k and e are small at the free boundaries, then their precise values should not matter as long as they are small and imply a small eddy viscosity. This comment presumes, of course, that there was negligible free stream turbulence in the experiments. You might consider benchmarking against a case (Cooper experiment H/D=6 ) where the results of the standard ke model are known, or even for a laminar case as suggested by John Chien. 
Re: Impinging Jet Modeling Problem
Thanks John and Michael. I think John your suggestion is good . I will try that , ie, to move the top boundary higher up. I will also try the benchamarking with coopers case as you suggested Michael.
Thanks a lot both of your for your helpful suggestions. I will get back to you guys after I run the new simulations. 
Re: Impinging Jet Modeling Problem
It seems to me that moving the boundary away from the nozzle somewhat would help to reduce the velocity at the boundary. then I would use a total pressure/ total temperture bc. If you're putting the boundary right up on the nozzle an use ambient static pressure then your total pressure is higer than ambient right? That seems fishy. You want to as closely model the idea of 'quiescent air' as possible. So I think moving the boundary away from the nozzle and using a total pressure BC are two things that could help.

All times are GMT 4. The time now is 14:00. 