TAGGED: ansys-fluent, cfd, dpm, fluid-dynamics, transient
February 18, 2021 at 12:44 amharshabharadwaj1Subscriber
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.February 18, 2021 at 3:40 amKarthik RAdministratorHi,nYou 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. nPlease 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.nKarthiknFebruary 24, 2021 at 1:09 amharshabharadwaj1SubscribernHope you are doing well. I am struggling to simulate the droplet deforming inside the plastic. nSo 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. nAlso, 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.nI 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.nAny help with this would be greatly appreciated. Thanks a lot.nFebruary 24, 2021 at 1:21 amYasserSelimaSubscribernAs you are already using a UDF, you can use DEFINE_INIT macro and set the VOF to specific cells to 100% air.nnFebruary 24, 2021 at 1:39 pmRobAnsys EmployeeThe 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. nFebruary 24, 2021 at 5:18 pmharshabharadwaj1SubscriberHello,nThanks for the replies. Here is a detailed run down with images as to what exactly I am doing and what the resultant output is. nI 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. nSince I only care about the phase interaction between the oil and plastic, I setup surface tension there.nn I used the Non-Iterative Time Advancement with Fractional Step but the solution did not converge. So I changed it to SIMPLE.nNow, 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? nnContours 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.nAfter 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. nWhat could be the issues here?nFebruary 25, 2021 at 12:07 pmRobAnsys EmployeeWhat time step are you using?nFebruary 26, 2021 at 5:53 pmharshabharadwaj1SubscribernI 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.nShould I be looking into injections for this rather than just VOF?.nAnd 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. nThanks for the help.nMarch 1, 2021 at 8:05 pmharshabharadwaj1SubscribernI 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.nnNow, the droplet elongates/moves along the channel with the plastic. However, I am still facing some issues. nI 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?nEven if I let the simulation run for a longer time, there still seems to be some plastic where air is supposed to be. nnIs there anything else I can change? Do you happen to know what the reason might be?nMarch 2, 2021 at 4:27 amYasserSelimaSubscriberHello,nFor 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 ... nMarch 2, 2021 at 4:50 amharshabharadwaj1SubscriberHello,nThanks 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) ?nAnd 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.nMarch 2, 2021 at 4:53 pmRobAnsys EmployeeCheck 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. nMarch 3, 2021 at 11:48 pmharshabharadwaj1SubscribernThanks 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.nNow, I changed the backflow for air to be 1. I seem to get good results with this.nI 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?nAlso, I am not specifying operating conditions? Is that vital for a VOF simulation as well? If so, what would be the values?nAnd regarding the mass conservation, I will play around with the mesh size and time step size. nThanks a lot for the help.nMarch 4, 2021 at 9:15 amRobAnsys EmployeeOperating conditions will influence pressure boundaries if gravity is on, but if the system isn't compressible probably won't do much. nYou'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. nMarch 6, 2021 at 3:56 amharshabharadwaj1SubscriberThanks a lot. I just had one more question.nI 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.nIncreasing either ones anymore, will take a long time to compute. Is there anything else I can do about this?nMarch 8, 2021 at 12:35 pmRobAnsys Employee400k 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. nMarch 9, 2021 at 11:05 pmharshabharadwaj1SubscriberThanks 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.nMarch 10, 2021 at 12:36 amMarch 11, 2021 at 6:03 pmRobAnsys EmployeeAh, possibly. You'll need to set them up for the phase pair of interest. nMarch 20, 2021 at 9:58 pmharshabharadwaj1Subscriber,nHello Sir,nI am trying to setup the dynamic meshing for the two phases of interest, but I am not able do it in such a way. nIs there a way I can do this without using UDF?nViewing 19 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.