July 3, 2019 at 12:44 pmPrashankSubscriberI am injecting 64 particles from a inlet using the surface option . I have three outlets & I need to know how many particles escaped from each outlet .
1.is there any option to calculate that?
2 . I am also facing an another problem. My no of incomplete particles keep on fluctuating with the no of iteration . Like on 289th iteration
no of tracked particles= 64, escaped = 63 , incomplete = 1
But the on 300th iteration
No of tracked particles = 64, escaped =56, incomplete= 8
I don't why is this happening.( My model contains vortex formations , if that helps)
July 3, 2019 at 2:37 pmRobAnsys Employee
Have a look at the results & particle positions: are any particles stuck in the recirculation/vortex zones? 64 is also quite low for statistical purposes: read up on stochastic tracking in the manual(s).
Have a look in the reporting options (monitors) and you should find a DPM Mass Escape. Assuming all the particles are the same size that should give you enough information. Alternatively use DPM Summary and review the data either as a histogram (Fluent) or via Excel or similar.
July 4, 2019 at 8:51 amhjubaerSubscriber
My understanding is, the problem you (@Prashank) mentioned is not unusual. The number of incomplete particles will depend on how many steps with what step length factor/length scale Fluent is tracking your particles. If your particle is still trapped inside your domain (e.g. due to vortex formation) after the longest possible tracked length is reached, it will be declared incomplete. As your iteration progresses, there must be some fluctuations in the solution of the flowfield which will lead to fluctuations in the residence time of particles. Therefore, your number of incomplete particles will naturally vary as well, I suppose.
I would suggest that, you try increasing tracking parameters (e.g. Max Number of Steps) under your DPM settings, in order to let fluent track your incomplete particles to the end. This way you can account for the definite fate for all your injected particles.
I hope that helps.
July 4, 2019 at 5:17 pmPrashankSubscriberThanks mate for your valuable suggestion..I have tried looking into monitors but I couldn't find dpm mass escape ( can you tell me it's location ).I found some mass concentration but it's report only mass concentration not the count of particles.
2.Also the summary option in report is unavailable....
3. I did increase the max no of steps. It seems that the particles are trapped in between the vortex before their trajectories could complete. Is there any option I can found about the location of those particles..
July 5, 2019 at 2:58 amhjubaerSubscriber
My guess is, you are running a steady-state simulation? If you are, then of course you are missing the particle current positions in your particle track summary.
If transient: Go to Particle tracks>Reporting>Current position and then you can add or remove variables that you want Fluent to report.
If steady state: Try Particle Tracks>Reporting>Step by step and then write the variables in a file
Either way, import the written file in excel and look at the residence time column first (column 1). May be sort the whole sheet according to decreasing residence time. So you now can see your culprits at the top. Column 2 through 4 should give you the particle positions (if the default order was not changed).
- 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.
- 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.