October 20, 2018 at 3:25 pmalmulhem_900Subscriber
I'm trying to model the flow of water and sand in 3D pipe with three side openings ( perforations) as shown in the following picture. The three holes are marked with the letters (A,B,C) and the other side of the pipe near hole C is plugged. The first objective is to estimate how much sand will escape from each hole.
Inlet (velocity-inlet B.C) with velocity = 8.617 ft/sec and reflect DPM B.C
outlet (pressure outlet B.C) with 0 gauge pressure and escape DPM B.C
Sand Injection is at the inlet face at the same velocity of the fluid (8.617 ft/sec) at flow rate of (22.4 lb/sec)
I'm having difficulty to get a converged solution using DPM without DEM collision and with steady particle tracking. Allowing DEM collision and tracking the particle in unsteady mode seems to be easier to get a converged solution but I have not gotten any yet.
Here are some questions I have:
- With such dense particle concentration will the DPM work ? or it is still considered to be a dilute fluid ?
- How can I model this problem using DDPM-DEM ? is the right model to handle such case ?
- Any tips to reach a convergence ( particle time step size, number of time steps, tracking parameters, Parcels, etc.... )
Thanks for your help
October 21, 2018 at 1:45 pmKarthik RAdministrator
To answer your question in general terms - DPM generally works well when your dispersed phase is dilute (volume loading ~ 10%). In case of DDPM, this volume loading is much larger and the model is preferred for modeling particulate flows. A note of caution - DDPM takes into account particle-particle collision and there are really two different approaches - 1. using kinetic theory of grannular flow (KTGF), and 2. Discrete element modeling. KTGF models particle-particle interaction using an approximate grannular theory while DEM explicitly resolves these particle-particle interactions.
Regarding steady vs. unsteady particle tracking, please take a look at this screenshot below (ref - Fluent Users Guide, R18.2, Chapter 23: Modeling Discrete Phase).
Please use this information to select a modeling approach based on the problem you are attempting to solve.
October 21, 2018 at 10:42 pmalmulhem_900Subscriber
Thanks Karthik for the reply.
I'm currently trying to run DEM with interaction between fluid and particles and it automatically switches to unsteady tracking. The question is how can I tell Fluent to simulate particles using DDPM? is there any specific button/window to enable it or DDPM is active when DEM collision model is selected? .
Please see below snapshots of an attempt to run DEM for the above problem.It is a very slow simulation. Is that normal for the case parameters? any suggestions/tips to make the case faster and reach convergence ? this case has been running for around 6 hours so far.
Thanks again for your help
October 22, 2018 at 5:55 amDrAmineAnsys Employee
To use DDPM you need to enable it under Multiphase Panel (as It a hybrid approach). Then in the injection panel check if the "Discrete Phase Domain" corresponds to the DDPM (secondary) phase
October 22, 2018 at 6:31 am
October 22, 2018 at 3:10 pm
October 22, 2018 at 5:03 pmDrAmineAnsys Employee
Either KTGF or DEM for particle particle interactions within the DDPM framework. The particles are tracked by solving ODE's as you want.
October 22, 2018 at 5:31 pmalmulhem_900Subscriber
Are both KTGF and DEM with DDPM framework you are referring to are using Lagrangian ? Can you show me where can I specify those models?
October 22, 2018 at 6:55 pmKarthik RAdministrator
Yes, both are lagrangian. If you are interested in the difference, please refer to my previous post.
Enabling KTGF: This can be done from the secondary phase. Please see the screenshot below.
Enabling DEM: DEM can be enabled from the Discrete phase options under Models. Select DEM collisions from Physical Models. Please see the attached screenshot.
I hope this helps.
October 27, 2018 at 5:29 pmalmulhem_900Subscriber
Here is a DPM case that I'm trying to solve.
I get a convergence when I use a 0.15 lb/sec mass flow rate as shown below:
When I increase the mass flow rate to 1.5 lb/sec (at iteration 1500), the solution does not converge and I get "floating point exception" as shown below:
This is the way I setup the DPM:
Can someone help me with solving this issue ?
October 28, 2018 at 10:57 amDrAmineAnsys Employee
Switch on update DPM source every iteration, increase number of continuous iterations per DPM and reduce DPM Underrelaxation and run for much more iterations: first steps to sort problems out.
ps: even the case at low loading the run is not converging at all from residual perspective
October 29, 2018 at 12:54 amalmulhem_900Subscriber
This is the status of an ongoing re-run of the high loading particles (1lb/sec) with the parameters you suggested. I'm using a 0.3 underrelaxation for DPM.
it is now around 35k iterations and still there is no convergence. Do you think it needs more iterations to converge ?
The following snapshot is for the early time. 0.15 lb/sec particle flow rate until 2000 iterations. is this still not converged for the low loading using 1e-3 residual criteria ?
Thanks again and best regards,
October 29, 2018 at 6:31 amDrAmineAnsys Employee
That is kind of non-converging case. Can you please describe a bit your case and share with us all information regarding boundaries, settings and co?
October 29, 2018 at 2:30 pmalmulhem_900Subscriber
The case tries to simulate the flow of water + sand along a pipe that is plugged from the outlet side and perforated on the sides as shown below:
Pipe length: 1 ft
Pipe diameter: 4.3 in
Perforation diameter: 0.38 in
Quadratic Meshing (400k nodes) with program controlled inflation layer as shown below:
Inlet: velocity inlet with 2 ft/sec. DPM BC: reflect
Holes: outlet vent with 0 gauge pressure . DPM BC: escape
Plug: stationary wall DPM BC: reflect
DPM as shown below:
Let me know if you need additional info
October 29, 2018 at 2:45 pmDrAmineAnsys Employee
How big is the particulate volume fraction? Can you make any estimation? Can you obtain a converged case without DPM?
October 29, 2018 at 2:49 pmalmulhem_900SubscriberIt is around 7% volume fraction
I did obtain convergence without introducing particles
October 29, 2018 at 3:03 pmDrAmineAnsys Employee
So you need to find now a biasing between the DPM Source Terms URF and number of update.
You can run transient for enhanced stability. 7% Volume fraction at high mass loading requires the resolution of particle-particle interaction but you can tackle that stage after you are able to run a fine DPM run.
Are you accounting for buoyancy effects?
October 29, 2018 at 3:45 pmalmulhem_900Subscriber
I'm eventually will use either DEM or DDPM to include particle-particle interaction.
Do you mean transient fluid flow or transient particle tracking ?
I think I'm not accounting for buoyancy yet.
October 29, 2018 at 3:50 pmDrAmineAnsys Employee
Both: Transient flow with transient particle tracking. I guess your continuous flow implies a sort of swirl which affect the particles and the latter start consuming the TKE of the continuous flow and the mean energy.
- 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.
- 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.