# Air Jet Simulation

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

 April 4, 2022, 10:45 Air Jet Simulation #1 New Member   Yaisel Join Date: Nov 2018 Posts: 8 Rep Power: 6 Hello everyone, I'm simulating air injected horizontally via two inlets (spargers) through one side of a water bath. Therefore it would be a multiphase problem (air and water). The bath is a hexahedral tank with dimensions 1 x 0.25 x 0.6 m (Length, Width, Height). The nozzles are velocity inlet. I'm simulating a steady state but I have problems in the convergence of the model. My model is composed of two continuous fluids with a reference pressure of 1 atm. I am considering buoyancy and the chosen reference buoyancy density is that of the less dense fluid (air). Heterogeneous model was considered to simulate the multiphase model, heat transfer was considered as homogeneous and isothermal model and a homogeneous model (k-epsilon) was used for turbulence. The fluid buoyancy model is Density Difference. The surface tension coefficient is 0.073 N m-1 and the interface transfer was simulated by Mixture Model with an Interface Len. Scale of 1 mm. The Drag Coefficient chosen is 0.44. The inlet condition was simulated with a bulk mass flow rate of 5e-4 kg s-1 where air initially enters. An Opening Pressure and Dirn with a Relative Pressure of 0 Pa was simulated at the outlet with a volume fraction of 0 for air. The Advection Scheme used is Upwind and Auto Timescale with the conservative option for the scale length with a factor of 1.0. In addition a consevation target of 0.01 is used. The results I obtain differ from those obtained in the experiments, which is caused by the non-convergence of the model. Does anyone know how I could improve the convergence of my model? Thanks!! Yaisel

 April 4, 2022, 23:00 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,266 Rep Power: 136 The general advice is: * better mesh quality * smaller time steps * double precision numerics * better initial condition If you want more specific comments please post your output file and some images of what you are modelling. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

April 5, 2022, 06:13
#3
New Member

Yaisel
Join Date: Nov 2018
Posts: 8
Rep Power: 6
Hello ghorrocks ,

Thank you for your prompt replay.
I will now work on the mesh quality to see if I can improve the convergence. The model that I'm talking about is steady state, but I have also simulated it as a transient taking the steady state result as initial condition and using a time step of 0.0001 s, the result does converge but sometimes when I have higher velocities the convergence costs a little more. I'm using double precision numeric.
I send you my output file and some images of what I want to model.
Thanks!!
Yaisel
Attached Images
 1.PNG (23.0 KB, 7 views) 2.PNG (12.4 KB, 7 views) 6.PNG (20.7 KB, 7 views) BC.PNG (27.3 KB, 8 views)
Attached Files
 CFX_001.zip (115.7 KB, 1 views)

 April 5, 2022, 06:31 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,266 Rep Power: 136 Some comments: * You should probably define the reference density as the water phase, and then initial and boundary pressure will just be a constant * A domain surrounded by openings is often unstable. Walls are more stable, and you can move them far enough away from the area of interest that they do not affect things. * A degassing boundary on the top face might work better What are you trying to achieve with this model? Won't you just get a stream of air bubbles rising from the inlets? Why do you want to model this? What are you trying to learn? __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 April 5, 2022, 08:37 #5 New Member   Yaisel Join Date: Nov 2018 Posts: 8 Rep Power: 6 Thanks for the comments , I will take them into account for the simulation I'm doing now together with improving the quality of the mesh. The degassing boundary at the outlet would only be available if I consider the air as a dispersed fluid. Is this true? I was simulating it as a continuous fluid both air and water. Do you think it would be better to simulate it as a dispersed and apply the degassing boundary? With this model I want to obtain the behavior of this air jet in water, to validate it given the experimental results we have obtained. Yes, what we get is a stream of air coming out of the outlet. Also with this model the idea is to obtain parameters that are difficult to obtain without applying intrusive methods in the experiments, as is the case of the pressure. Thanks again!!

 April 5, 2022, 13:26 #6 New Member   Yaisel Join Date: Nov 2018 Posts: 8 Rep Power: 6 Thanks for the comments!! I performed a first simulation taking into account all comments and an error occurs at iteration 4 (ENFORCE_BOUNDS), after the previous iterations put: A wall has been placed at portion(s) of an OUTLET boundary condition to prevent fluid from flowing into the domain. If this situation persists, consider switching to an Opening type boundary condition instead. Another point is that the Degassing boundary condition requires that air be assumed to be a dispersed fluid. In my previous simulations I was simulating it as a continuous fluid. Do you think there is any improvement if it is considered as a dispersed fluid? Then let me assume instead of a degassing boundary at the output, an opening, and continue to diverge the simulation. Thanks again!!

 April 5, 2022, 20:16 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,266 Rep Power: 136 There are many different multiphase models in CFX and you should choose the one which best matches the physics of what you are trying to model. So make sure you have read the CFX documentation on multiphase modelling so choose the correct model. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 April 6, 2022, 07:22 #8 New Member   Yaisel Join Date: Nov 2018 Posts: 8 Rep Power: 6 Yes, I know the multiphase models that can be used in CFX, I have used the Mixture Model because it is the one that best suits my conditions. I also used the Particle Model in the first simulations, but in the end I opted for the Mixture Model.

 April 6, 2022, 07:34 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,266 Rep Power: 136 Good to hear you have checked this and I will take your word for it that the mixture model is most appropriate for your case. Does it run better if you have a free surface a short distance down from the top boundary? This will probably be easiest if you make the side boundaries walls and you can make the top boundary an opening with air volume fraction = 1. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

April 6, 2022, 08:04
#10
New Member

Yaisel
Join Date: Nov 2018
Posts: 8
Rep Power: 6
What you are telling me is to use a Headspace Condition? (As show in the figure below)

I have used it before but I could try it with the new comments you made to see if it works better.

Thanks!!
Attached Images
 1.PNG (189.7 KB, 5 views)

 April 6, 2022, 08:25 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,266 Rep Power: 136 Yes, a headspace condition. You might need to add a free surface model as well to capture the interface properly. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 April 6, 2022, 08:30 #12 New Member   Yaisel Join Date: Nov 2018 Posts: 8 Rep Power: 6 Ok, I'll do that then. When I get something I'll let you know. Thank!!

 Tags air + water flows, convergence, jet flows, multiphase