I tried with different injection velocities from 0.1 m/s to 1.5 m/s. However, there was no effect on droplet shape.

Perhaps the surface tension is not properly represented. In the case of jet figure, varicose instabilities act and are magnified by the surface tension.

Let me ask, what is the criteria of breakup you add?

It seems to me that you have two phase flow without breakup.

@ Maestri

As i am using the water and air as my fluids so i added the value of standard surface tension of 72.1 mN/m.

@Elwardany

I followed the standard procedure given in the Fluent tutorial guide. If i continue to run this simulation, the drop gets break up. But still it did not attains a spherical shape. It has a elongated droplet like only.

Kindly see the shape of droplet which i got upon running the simulation for 30 micro-seconds. It has a elongated drop shape which i mentioned earlier. Can anybody suggest something as of where i am doing wrong? Because in actual practice we would always observe a spherical water-droplet due to its 180 deg contact angle with air.

Hi Harpreet - a couple of things that occurred to me.

The first is whether the total simulation time and vertical domain length are long enough. It could be that there are some physical oscillations of the shape of the droplet before it stabilizes into a sphere, due to the large mismatch between air and water, density and viscosity.

Even the horizontal width of the domain could have an influence - are these walls? Are they far enough away from the droplet to have negligible effect on the free surface?

Another possibility that occurred to me was numerical in nature, are you using a fine enough mesh, and a small enough time step.

Hello Lavery

Thank you for your response.

In response to your second and third comment i would like to add that the spacing between the outer walls is three times the nozzle diameter. I checked the pressure and velocity distribution also but i think they were not influenced by the wall spacing. I used a small enough time step of 1e-8 seconds and mesh was adapted before the final simulation.

I think the possibility could be there for the point you highlighted in your first comment. However, as i and most of you might have seen practically that when liquid comes out of out small opening upon being pushed at very small velocity it will directly attain a spherical. My confusion is that what could be the reason for it not to be attaining that perfect shape.

Hi Harpreet,

I would consider taking the wall up to 5 times or more of the width of the nozzle. The lower droplet in the image above seems to be big enough that if it did become spherical, because of surface tension, its surface would be very close to the walls. Even small pressure differences in a confined tube could overcome the surface tension forces and elongate the droplet.

Certainly it would be interesting to see what happened with a longer domain. Would the first droplet become spherical? Would the second droplet break up into a third?

Are you working in double precision? Certainly the very small time step you are using would be further away from round-off in double precision.

Finally, there are different models for the geometric reconstruction of VOF which may or not be more appropriate. In the VOF model are you using implicit body forces? Also, FLUENT has two different models for the surface tension, the Continuum Surface Stress (CSS) and Continuum Surface Force (CSF), you might have greater control on the tangential forces with the CSF.

Hello Lavery

I will try to work out with your suggestions and will update here.

Thanks for the help.

.

Harpreet, the comments by Nick are extremely appropriate because there is a true experimental "magic" number 5:1 ratio of the inner diameter of the conduit diameter and from this body that there is no influence of the walls. As soon testing to verify diameters greater sensitivity.

.

Another tip you could try is to vary the surface tension. Your value is correct, but do not know what level of sensitivity of the program.

.

But what is surprising because I do not varicose display modes prior to the formation of the bubble, the figure showing might not be. Check the shape before formation of the drop.

.

You must also work with the hypothesis of small bugs in the program! As my academic origin is essentially physics simulation always have some suspicion of numerical models!

.

Comsol maybe one good choice.

@ Maestri

Thank you for your comments.

As suggested Nick and you i have re-modeled my geometry and am running the simulations. I will update once i have the results.

Try to repeat the simulation with ~ equal sized mesh in both x and y directions...if it is not already so....

Thank you Sijoy, but mesh is already equi-sized.

@Navamani

I am using 175 deg as the contact angle value. Kindly suggest if i should modify this value.

Dear All,

Thank you for your suggestions.

As suggested by Nick Lavery and Rogerio Maestri, i modified my geometry and now the droplet forming is almost spherical in shape after travelling almost 40 mm distance. The shape was bit distorted after getting detached from the needle; however, after some oscillation it attains a spherical shape.

Thank you all for sharing your experiences and knowledge.

.

Harpreet

.

Depending on the type of oscillation that occurs it may be representing exactly what occurs in nature. Look look at some photos or videos, because maybe your simulation is better than you're thinking.

.

Thank you for presenting a good problem for us to exercise our mind, congratulations.

.

Harpreet,

Rarely I encounter such questions ending with better solution after meaningful discussion. Why don't you post a picture of the last simulation where you got near spherical shape droplet.

@Navamani

Dear Navamani, I too have the experimental data with me. However, one needs to consider that what value one should opt for while doing simulations as also suggested by Prof. Maestri in above discussions.

make sure you have given proper value of surafce tension (interaction of phases)

Dear Harpreet Singh Grewal ,

 I would like to see your final contour  and short description how you resolve this issue.·

Harpreet Singh Grewal Could you please provide me with the tutorial guide because I am trying to work on a similar project.

Best

Adetayo