May 5, 2022 at 6:59 amNargesSubscriber
I'm trying to calculate DPM erosion Rate, but no matter what method I use, I just get zero as the result! can anyone help about what the problem is from?
System: fluid + nanoparticles are injected from the inlet of the microchannel
I used: 3D-dp-pbns-steady state flow
viscose model: SST k-omega
DPM: 2-way coupled, injection type: surface-inlet
BC: velocity-inlet, pressure-outlet, reflect-wallMay 5, 2022 at 7:03 amDrAmineAnsys EmployeeAre you using the Boundary Trap for DPM at the walls?
May 5, 2022 at 7:07 amNargesSubscriberI have used "reflect" and "wall-jet" and also "trap" and even UDF! not only Erosion rate, but also the "DPM wall force" and "DPM wall normal pressure" are zero!
my fluid is Water. I resimulated my system with air and it worked! how can I solve it?
May 5, 2022 at 7:39 amDrAmineAnsys EmployeePlease first focus on using Trap and check if any particles are declared to be trapped? Which version area you using?
May 5, 2022 at 7:43 amNargesSubscriberI'm using Student version. when I change my fluid from "liquid water" to "air" I can get non-zero value. but I don't know how to do it with liquid Water.
May 5, 2022 at 7:50 amDrAmineAnsys EmployeeThe same way as with air: your particles are not hitting any wall perhaps..
May 5, 2022 at 7:57 amMay 5, 2022 at 8:04 amDrAmineAnsys EmployeeAlso again: if you set the wall to be a trapping wall: do you see the particle trapped there Yes or No?
May 5, 2022 at 8:07 amNargesSubscriberwhen I use water as fluid there is no trapped particle.
when I use Air as fluid, less than a third of particles are trapped and else escaped.
May 5, 2022 at 8:56 amDrAmineAnsys EmployeeIf you do not have any trapped particles then you won't see any erosion rate as your particles are not toughing the wall. Please add a screenshot of particle tracks and screenshot of particle DPM Summary.
May 6, 2022 at 1:28 amMay 6, 2022 at 9:22 amDrAmineAnsys EmployeeThe mesh does not look good for me but it is my flavor as I prefer uniform mesh and boundary layer resolved meshes. Moreover your particles are all escaping so your erosion rate will be zero. You said at it was air particles are trapped on the wall. Water has higher viscosity and this will affect the particle relaxation time. Can you estimate the Stokes number based on the properties you have?
Consider changing the position of the outlet to avoid any numerical backflow which you are now just "avoiding" via artificial wall creation.
May 6, 2022 at 9:41 amNargesSubscriberDr. Amine, thank you for your answer. the Stocks number is 1.8575e-6 for this system.
sorry, but I didn't get the "changing the position of the outlet". how can I do that?
May 6, 2022 at 9:44 amDrAmineAnsys Employeeyou place your outlet bit more downstream to avoid any numerical backflow. Sometimes backflow will also happen due to the physics. Please disable the "prevent backflow" option and try to figure out why you have a backflow.
Your Stokes number is very low so the particles will be like passive tracers and travel with the flow.
May 6, 2022 at 10:43 amNargesSubscriberThank you very much for your help. with increasing the particle relaxation time I can get non-zero wall force. I also I removed the "prevent backflow" option.
would you please suggest me a method to improve my meshing?
May 6, 2022 at 11:08 amRobForum Moderatorlikes inflation and hex, alternatively have a look at Fluent Meshing and use inflation with polyhedral cells.
With a Stokes Number that low I'd be surprised if the particles hit anything: they'll follow the flow.
May 6, 2022 at 12:23 pmDrAmineAnsys EmployeeAssess some inflations layers :)
May 10, 2022 at 1:31 amNargesSubscriberthank you . sure, I will do that
Viewing 17 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
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- Suppress Fluent to open with GUI while performing in journal file
- error: Received signal SIGSEGV
- Using GPU in FLUENT
© 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.