February 21, 2022 at 7:15 amSardarSubscriber
I hope someone would spare a minute to look into my problem.
Tons of particles is going to be volume-injected into the entire domain of a mixing tank with impellers inside.
I am not exactly sure how to proceed from where I have already got. However, I have separately achieved two objectives in two different solution strategies as follows, without success in combining them together.
1. I have solved the single phase flow almost fully in hope of being able to add particles to it. Adding particles seems to stuck as the solver does not procede beyond the first DPM iteration message, even with a flow time step of 0.01 second. However, Fluent user's Guide suggests this method.
2. I have also managed to inject particles (in 1.5 seconds with flow timestep being 1 (s), as suggested by Rob here.) to the unagitated tank (zero angular velocity for impellers) letting water discharge through the tank top using the outlet vent in one modelling (and in another, outflow) BC. After this stage, let alone with rotating the impellers, even letting the particles sediment causes continuity divergence.
Q1 .If either of the two strategies above is correct, which one is that? what am I doing wrong? And can you please take a look at simulation adjusments below, and comment on my questions put beneath them? (images show adjustments for injecting into the unagitated tank in 1.5 seconds as mentioned earlier.)
System Settings (question mark, [?] indicates uncertainty on my side) (p lease see images below for more)
The continuous phase is water. DPM-continuous volume fraction is 20%.
Tank dimensions are diameter 3.8 and height of 5.5 meters.
Transient [?] | Eulerian - DDPM - granular | SST - dispersed multiphase turbulent model | Coupled [?] - all schemes (including transient formulation) being second order upwind except for volume fraction being QUICK | unsteaady particle tracking [?] - tracked with flow timestep [?] - step length factor of 5 [?]February 21, 2022 at 12:38 pmRobAnsys EmployeeHave a look at the DPM theory: what volume will your particles occupy when they settle out?
February 21, 2022 at 1:39 pmSardarSubscriberWell, the volume occupied was monitored in the second strategy mentioned in the original post, being around 15.6 cubic meters. But how does that help, if you don't mind?
Oh, that might be my bad, misusing the term DPM instead of DDPM when pointing to the discrete phase volume fraction above.
Actually I am already using DDPM, as my discrete model, and I guess you mean to refer me to the following in the theory guide:
"The discrete phase formulation used byANSYS FLUENTcontains the assumption that the second phase is sufficiently dilute that particle-particle interactions and the effects of the particle volume fractionon the gas phase are negligible. In practice, these issues imply that the discrete phase must be present at a fairly low volume fraction, usually less than 10-12%. Note that the mass loading of the discrete phase may greatly exceed 10-12%: you may solve problems in which the mass flow of the discrete phase equals or exceeds that of the continuous phase."
So, once again, to clarify, since my DPM volume fraction is 20%, I have chosen DDPM!
By the way, What I overlooked in my original post was to mention that I turned off the flow and turbulence equations in the second strategy.
February 22, 2022 at 5:00 pmRobAnsys EmployeeAt 20% your particles are going to switch from DPM to Eulerian pretty much instantly. Ie the DDPM model is instant. If you turn off the flow equations I'm not sure what will happen as you're now using an Euler phase with some particles over the top: the maths will be a mess as the flow can't update.
Now, with the second approach, the DPM part of DDPM doesn't understand the packing limits so as the particles sediment out the volume fraction can reach a high value, ie well over 1. This isn't physical and again will cause strange things to happen.
For a suspension DPP/DDPM/Euler will be fine, for sedimentation Euler is preferred. Or uncouple DPM where the excessive volume fraction can't cause the fluid phase to diverge as the volume fraction becomes non-physical.
February 23, 2022 at 8:50 amSardarSubscriberIf not mistaken on your comments, I can think of adding particles kind of gradually (via several injections) while rotating the impellers with high enough velocity to keep the powders mixed apart between injections and thus, avoiding volume fraction troubles you mentioned, but low enough to not burden the solver with flow complexities. (Easier said than done!)
I am afraid I can't see your point in "for sedimentation, Euler is fine". Does that mean Eulerian model without DDPM activated? I thought I should be the opposite way around, as sedimentation implies high volume fractions for discrete phase at the tank floor. Doesn't it? And what is DPP? I could not find DPP in the User's/Theory Guide btw :)
Thank you so much, Rob, you have no idea how helpful your comments are on this end of the line, specially if they are a bit more elaborated - just a bit. :)
February 23, 2022 at 2:14 pmRobAnsys EmployeeDPP is DPM, I'd had a long day......
If you read the back ground for the models it'll make more sense. DPM assumes a dispersed particle phase. Eulerian assumes it's not dispersed, but can also be used for low volume fractions. DDPM bridges the gap, but because the particles don't obey packing limits when you get sedimentation the volume fraction can exceed 1. I think there's a correction in 2022R1 but check the documentation.
If I elaborate too much there's no incentive for you to read the manuals and do some of the courses. ;)
February 23, 2022 at 2:41 pmDrAmineAnsys Employee;)
Viewing 6 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
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
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 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.