July 1, 2021 at 10:42 amPhilxyzSubscriber
I'm currently simulating a multiphase flow in 2 phases with pbm. phase 1 is gasoline and phase 2 is water. The goal is to simulate an emulsification process with water as the dispersed phase.
As my multiphase model I'm using the Euler and Mixture model to compare them. (see attached screenshots)
In the beginning I was simulating the flow without any PBM activated, just So I know that it is running stable. The Problem is that as soon as I activate the PBM my flow pattern changes completely, while it is still running stable and converging.
So the question is if anybody knows why the flow pattern changes or how to fix it.
Thank youJuly 1, 2021 at 2:50 pmDrAmineAnsys EmployeeFirst of all you need to pay attention the kernels you want to use: almost none of them have been calibrated for your flow system. Check the references in the Guide and do a literature review. Second: now you have a polydisperse flow with changing diameter-> affects Interfacial area, drag force and non-drag forces. I won't use surface tension force for this kind of subjects. Cheers!
July 1, 2021 at 2:52 pmDrAmineAnsys EmployeeBit looks more weird than just my explanation: please check the boundary condition if something went wrong. Also check without any breakage and coalescence and just use a dummy polydisperse by just initializing and using a 1 for certain bin size at inlet. Debuging will help to understand!
July 1, 2021 at 2:52 pmDrAmineAnsys EmployeeAnd Report back!
July 1, 2021 at 3:40 pmRobAnsys EmployeeAnother question, which way is up in your model?
July 2, 2021 at 8:29 amJuly 2, 2021 at 10:10 amRobAnsys EmployeeHmm, if you plot phase fraction on the walls what do you see.
July 2, 2021 at 10:27 amJuly 2, 2021 at 10:34 amRobAnsys EmployeePerfect. Now look at the droplet sizes in the two cases.
July 2, 2021 at 11:01 amDrAmineAnsys EmployeeGo through what we have shared yesterday with the debugging and check the diameter predicted with your current model. Also share residuals and convergence behavior of both runs.
July 2, 2021 at 3:44 pmDrAmineAnsys EmployeeCheck the size Check the Size Check the Size :) :) small droplets are swept away.. Large droplets have more resistance and they accumulate...
July 2, 2021 at 6:28 pmPhilxyzSubscriberI don't have any droplet size in the model without PBM except the default value (1e-05), but I think I'm getting what you mean. The flow of the individual droplets looks suspiciously close to the flow of water without PBM. Meaning that fluent is tracking the flow of the individual droplet and depicting it as the actual phase (water). I hope I make sense right now :)
Disabling the surface tension force seems to do the trick. The flow looks to the one without the PBM (the simulation isn't completely done yet). Also I'm letting in just 1 BIN size at the moment.
July 3, 2021 at 10:56 amDrAmineAnsys EmployeeGood progress.
July 5, 2021 at 6:34 pmPhilxyzSubscriberLittle Update: The last simulation is run through without any problems and without any change in the flow pattern.
What I got from different simulations is as stated before: depending on the BIN size I set up at the inlet my flow pattern changes.
The changing diameter, or rather a different diameter than before, changes drag and non-drag forces and the interfacial area of the droplets as DrAmine already pointed out.
So basically if I have a flow in which I want to track droplets via PBM I can't compare flow patterns of simulations with different inlet droplet sizes.
July 6, 2021 at 6:14 amDrAmineAnsys EmployeeBecause as mentioned from the beginning: you need to "review" the kernels used for breakup and coalescence which have not been calibrated for this kind of system. So actually either you set a limit for the bin sizes (Top), adjust the kernels or you stick to a monodisperse formulation. There is another model which try's to enforce a special treatment where the secondary phase accumulates. Is is the GENTOP approach, relies , however, on the PBE and so on the kernels you are using.
July 6, 2021 at 6:58 amPhilxyzSubscriberThank you for all the advice
July 6, 2021 at 9:24 amDrAmineAnsys EmployeeWelcome!
Viewing 16 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- The solver failed with a non-zero exit code of : 2
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
Top Rated Tags
© 2022 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.