March 14, 2022 at 2:40 pmLyladSubscriber
Hi, I am creating a particle flow using DPM I want to figure out the total flow rate of my particles I found on the other forums that the formula is m_dot=# particles per sec [#/s] * mass of particle [kg].
But I just wanted to ask what this part meant # particles per sec [#/s], I understand it's the "strength" and is the reciprocal of the particle time step but how should I determine the particle time step as I understand that the default is 0.001 ?
Also does the particle time step mean the rate of particles being released ?March 14, 2022 at 4:05 pmRobAnsys EmployeeThe flow rate is either taken from the reports or read from the injection panel (out and in respectively). Given we work with parcels that may or may not be of equal mass you need to be little careful.
Particle time step is something you set, in the above it's the same as the flow time step. If you're running a steady flow you can use transient particles so there's a particle time step to consider.
March 14, 2022 at 5:00 pmLyladSubscriberHi rob thank you so much for your reply, if I wanted to calculate the flow rate would I use the formula above ?
And does that mean that the particle time step is equal to the flow time step that you specify in the run calculation page?
Just as context I am running a simulation with a cow coughing and releasing particles therefore I would like to set a rate for the release of particles therefore I would like to set the total flow rate (the rate of the cow releasing particles).
March 15, 2022 at 9:31 amRobAnsys EmployeeFlow rate (entering) is what ever you need it to be: you work out how much mass is entering. For a cow coughing that will be a very small kg/s value. The issue is whether you want to model the cough, and therefore a transient case or steady in which case you want to review the boundary conditions.
March 15, 2022 at 10:32 amLyladSubscriberHi rob I figured out the mass of the particles being 3.6e-14 kg then do I divide it by the time I want the cow coughing for ?
And I am using a transient case to model the transient airflow into the barn in my study, does that seem correct ?
Thanks sorry for all the question :)
March 15, 2022 at 2:15 pmRobAnsys EmployeeYes, so if the cow coughs for 0.5s you need 7.2e-14 kg/s However, have a think about the size of the domain compared to the flow of gas from the cow. How long do you think it'll take for the particles to leave the system, and how much of an effect do you think the cough will have?
March 15, 2022 at 7:25 pmLyladSubscriberHi Rob, okay thats fine I will calculate that I am going to have the cow coughing then respiring out for 10 secs overall so I will have the flow rate as 3.6e-15. So this should be long enough to make an effect on the system.
Also, I have tried to look at modelling droplets for my particles to allow evaporation but once I have run the simulation it says that 0 number of particles have been tracked therefore I am slightly confused why this might be, if not I assume I can just use inert particles to model infectious aerosol ?
Thank you :)
March 16, 2022 at 11:23 amRobAnsys EmployeeProbably safer, and not modelling species will speed up the calculation. Check you are actually adding particles into the system too.
March 16, 2022 at 11:36 amMarch 16, 2022 at 11:52 amRobAnsys EmployeeIs the model transient?
March 16, 2022 at 11:53 amLyladSubscriberYes it is
March 16, 2022 at 1:57 pmRobAnsys EmployeeThe number of tries is to kick trajectories off the mean path when running steady. In a transient run the assumption is that a particle release happens every time step so the changing flow will do that. Turning on Random Walk means the trajectory gets the random kick, but you don't get extra parcels.
March 18, 2022 at 4:56 pmLyladSubscriberHi thank you rob for your answer.
Also I have another question i've been using the droplet function for the particle type however it only seems to show the particle results when the simulation is in steady state.
But I want to run the simulation in transient is there something else I need to enable or another reason for this ?
March 18, 2022 at 8:13 pmDrAmineAnsys EmployeeAdjust stop and start times for the injection as first thing to check.
March 19, 2022 at 11:12 amLyladSubscriberHi thanks for replying my start time is 0 secs and the stop time is 10 secs, should I try to change this to see what happens ?
March 19, 2022 at 12:23 pmLyladSubscriberHi just to confirm these are the boundaries I am using but its not showing any particle tracks in results
Transient: on, gravity y=-9.81
Models- Energy= on, Species transport= on, viscous= k-epsilon/ RNG/Standard Wall functions
Discrete Phase= ON, interaction with continuous phase , unsteady particle tracking, track with fluid flow time step.
Injection= surface, particle type= droplet, material= water liquid, evaporating species= H20, diameter distribution= rosin- rammler.
injection velocity= 10 m/s, temp= 300 K, start time =0 stop time= 10 secs, flow rate= 1e-20, mean diameter= 1e-5, ticked scale flow rate by face area
Then for boundary conditions= inlet= 8.7 m/s and outlet= gauge pressure is 0 (nothing changed for the outlet values)
Run calculation; number of time steps= 1000, time step size= 0.1, max iterations= 20
Bellow I have put a picture of what results it produces when I try to run droplet particles I'm not sure why it's not showing proper particle tracks I would appreciate any help as I want to model droplet infectious aerosol with a transient model.
March 19, 2022 at 1:29 pmDrAmineAnsys EmployeeIf you display the particle summary what do you see in the console?
March 19, 2022 at 2:29 pmMarch 19, 2022 at 3:55 pmDrAmineAnsys EmployeeAlmost all particles have evaporated. So no particles traces can be displayed as they are not there. The other remaining particles are still in domain and you should be able to see them. You scale up the size of displayed particles.
March 19, 2022 at 8:09 pmLyladSubscriberThank you so much DrAmie I've increased the size of the particles and I think thats worked :)
March 20, 2022 at 6:11 pmDrAmineAnsys EmployeeWelcome ƒÖÅ
Viewing 20 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
- 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.