Drop deformation inside an existing liquid

harshabharadwaj1harshabharadwaj1 Member Posts: 9
edited February 18 in Fluids

Hello,

Hope you guys are doing well. As seen in the image below, I have simulated a flow of plastic (green) onto a build plate. There exists a continuous flow of another liquid (red) in the middle of the plastic.


Where currently the continuous red phase is, I would like to simulate a drop breaking/elongating along the path. Would I be able to do something like this?

I would like to create a drop at the inlet and would like to determine how the drop breaks up and elongates in the channel. I would like to see what the resultant shape will be like at the outlet (plane highlighted in black).

How would I do something like this?

I am using a Laminar model and have neglected the surface tension as of now.

I looked up Injections, but was not able to understand properly as to how to do it. Any help will be greatly appreciated.

Comments

  • KremellaKremella Posts: 2,471Admin

    Hi,

    You should be able to do this in Fluent. You will have two fluids - air and liquid (of interest). You will need to the VoF model in Fluent. Also, surface tension would be important here because you are talking about drops of liquid, and the reason surface tension force generally tends to make these drops round.

    Please have a look at VoF tutorials on YouTube and these might help you get started. Also, there is plenty of literature available on this topic. Please read through the modeling work. This will help you understand if you are making progress in the right direction.

    Karthik

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member

    Hello @Kremella

    Hope you are doing well. I am struggling to simulate the droplet deforming inside the plastic.

    So I looked at lot of videos about VOF models. The best way I could think of was creating a region at the top of the inlet and patching it with the volume of the droplet. The complexity here is that the drop deforms at the centre as the plastic flows.

    Also, to be exact I would be having three phases here. Plastic (green), droplet (as indicated by the continuous red) and air flowing in the direction of the strand deposited.

    I am using the VOF model with surface tension. I am using an UDF to simulate the flow of plastic to get a parabolic profile. As mentioned above I create a region in the shape of a sphere at the top of the inlet and patch it. Not sure what it is I am doing wrong.

    Any help with this would be greatly appreciated. Thanks a lot.

  • YasserSelimaYasserSelima Posts: 931Member

    @harshabharadwaj1

    As you are already using a UDF, you can use DEFINE_INIT macro and set the VOF to specific cells to 100% air.

  • RobRob UKPosts: 8,855Forum Coordinator

    The droplet will deform based on the material properties and local flow field, so it will deform. Pay attention to the solver convergence and mesh: you may need a lot more cells than you realise.

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member
    edited February 24

    Hello,

    Thanks for the replies. Here is a detailed run down with images as to what exactly I am doing and what the resultant output is.

    1. I am using the VOF model with Explicit formulation. The flow is laminar. There are 3 phases. I create three materials: Air, Oil and Plastic with different properties. I go to phases and set air to be the primary and the other two are secondary phases.
    2. Since I only care about the phase interaction between the oil and plastic, I setup surface tension there.


    1. I used the Non-Iterative Time Advancement with Fractional Step but the solution did not converge. So I changed it to SIMPLE.
    2. Now, I create regions for plastic and oil (Images attached). I Initialize and patch the regions. Now if I set the VF of plastic and oil to be 1, it gives me an error (image attached). Should I just set it to be 0.5 each?


    1. Contours of the volumes after patching are attached as well. The VF for air does not make sense to me since air is not supposed to be present in the inlet cylindrical area i.e. the green section (images attached). This can be eradicated by giving VF as 1 for plastic, but doing that I am not sure if I can set the VF for oil as 1.
    1. After running the simulation, I do not see anything at all. The solution converges pretty early and the model remains how it was before. I do not see the flow of the plastic or the drop deforming inside the plastic. The flow of the plastic should be similar to the image attached in my original post.

    What could be the issues here?

  • RobRob UKPosts: 8,855Forum Coordinator

    What time step are you using?

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member
    edited February 26

    Hello @Rob

    I am using Adaptive, Incremental time steps. Number of time steps = 20 because it converges before that itself. Courant number is 2. Initial time step size = 1e-5.

    Should I be looking into injections for this rather than just VOF?.

    And about the volume fraction error I get above, can you suggest what I can do about this?. Because the oil drop and the plastic exist in the same region, and I cannot set both to 1.

    Thanks for the help.

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member
    edited March 1

    Hello @Rob

    I created two different zones so that I could assign the volume fraction of air to that zone, instead of assigning the VF for plastic. I was able to solve the VF error from above.


    Now, the droplet elongates/moves along the channel with the plastic. However, I am still facing some issues.

    I am playing around with different time steps. The one attached below has a time step of 0.0005. As you can see from the image there is some plastic present at the outlet. This is incorrect and should not happen. I do not know the reason for this. Also, the results do not converge even after a very long time. And as the oil droplets moves, its volume keeps on decreasing. Is that supposed to happen?

    Even if I let the simulation run for a longer time, there still seems to be some plastic where air is supposed to be.


    Is there anything else I can change? Do you happen to know what the reason might be?

  • YasserSelimaYasserSelima Posts: 931Member

    Hello,

    For batching, instead of creating zones and interface, you can used Define_init macro .. loop through all threads and cells, assign the VOF based on coordinates ...

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member

    Hello,

    Thanks for the reply. I am not too sure how to do that. Also, does it make any difference in the final results either way (creating separate zones OR using a UDF to do it) ?

    And also for the air geometry, highlighted in blue in the last figure, I am not too sure as to how I can specify using co-ordinates. It it were a cylindrical block, I could have done it easily. This, I am not too sure.

  • RobRob UKPosts: 8,855Forum Coordinator

    Check the backflow phase setting re the outlet. You won't be the first person to have the wrong phase set. If you're losing mass from the blob it's usually either the mesh being too coarse or the time step is too big: you're not conserving mass sufficiently.

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member

    Hello @Rob ,

    Thanks for all the help sir. It was indeed the backflow that was giving me issues with the flow. Since it is a three phase setup, the backflow for both the secondary phases was set to 0.

    Now, I changed the backflow for air to be 1. I seem to get good results with this.

    I did read up some stuff about the backflow. Either I have to increase the length of the cylinder in the outlet direction or use prevent back flow option. Will it make any difference if I change the Volume Fraction Specification Method?

    Also, I am not specifying operating conditions? Is that vital for a VOF simulation as well? If so, what would be the values?

    And regarding the mass conservation, I will play around with the mesh size and time step size.

    Thanks a lot for the help.

  • RobRob UKPosts: 8,855Forum Coordinator

    Operating conditions will influence pressure boundaries if gravity is on, but if the system isn't compressible probably won't do much.

    You're right about the back flow, but it only needs correcting if it's altering the flow: you need to judge that. We recommend extending the model, but unless the air alters the temperature or flow of the polymer it may be less critical, but you may need to defend the assumption in your report.

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member

    @Rob Thanks a lot. I just had one more question.

    I am currently running the simulation with 400K nodes and elements. And the time step size is 5E-5. Even with this, there seems to be a significant loss of volume of the oil. Although. the VF of air and plastic is very well consumed.

    Increasing either ones anymore, will take a long time to compute. Is there anything else I can do about this?

  • RobRob UKPosts: 8,855Forum Coordinator

    400k cells may or may not be enough. Have a look at dynamic adaption and the pre-set refinement & coarsening options. Also, check the convergence for each time step and use a monitor to check for mass of the oil.

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member

    @Rob Thanks for all the help sir. I got to know a lot from these conversations. I will get back to you if I have any more questions.

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member
    edited March 10

    @Rob Is Adaption Controls not available for 3 phase VOF simulation?. When clicked on Predefined Criteria, nothing pops up and I cannot select Volume-of-fluid.

    But I can do when there are 2 phases. Am I doing something wrong here?.


  • RobRob UKPosts: 8,855Forum Coordinator

    Ah, possibly. You'll need to set them up for the phase pair of interest.

  • harshabharadwaj1harshabharadwaj1 Posts: 41Member

    @Rob ,

    Hello Sir,

    I am trying to setup the dynamic meshing for the two phases of interest, but I am not able do it in such a way.

    Is there a way I can do this without using UDF?

Sign In or Register to comment.