March 14, 2022 at 10:56 amyyds4092Subscriber
I am currently using Fluent with DDPM and DPM model to simulate particles suspending in the liquid turbulence pipe flow. The pipe diameter is 40 mm and my particles are 2mm, which is quite large. Therefore I used very coarse mesh to ensure the mesh cell is larger than particles.
I had two problems with my simulation. Firstly, as my particles are heavier than the liquid phase, particles are settling at the pipe wall. However, some of these particles get very close to the wall which is less than 1 mm (the radius of the particle) and this is physically not true. I am wondering if there is any method to push the particles out of this 1mm region.
Secondly, as the DDPM model could handle dense volume fraction multiphase flows, I tried to increase particle volume fraction up to 30 vol%. However, I found particles aggregate together at the centre of the pipe (which is validated in the experiment and literature) and the aggregation makes the simulation unstable or diverge sometimes. My initial guess is that the aggregation of particles increased the local solid volume fraction which probably reaches the limitation of the DDPM and causes such issues. I am wondering if anyone has encountered similar problems before and any suggestions for these problems
Thanks in advance!March 14, 2022 at 11:52 amRobForum ModeratorPart of the problem is that DPM doesn't have a packing limit, so particles can pack to a volume fraction exceeding unity. This then causes some problems with the DDPM model. If the whole system is still flowing it's often stable, if a little non physical. However if the particles settle stability becomes a problem.
How big are the cells, especially next to the wall? DPM assumes a point mass, and doesn't even check for wall interactions until it's in the near wall cell.
March 14, 2022 at 2:22 pmyyds4092SubscriberHi Rob
Thank you so much for your quick reply.
The majority of the particles are flowing in a good condition and their velocity and volume distributions are close to the experimental results. However, particles close to the wall are always settling. I used both very fine mesh (first cell high=0.08 mm, y+=0.7) and very coarse mesh at the wall (first cell high=1.5 mm,y+ >30). However, particles will always get too close to the wall (less than the radius). I highly agree with you that since DPM model regards particles as a mass point, particles cannot be stopped from approaching the pipe wall. Therefore, as the particle-liquid flow moves, the cells at the wall trap the particles and lead to instability sometimes. I am wondering if there are any ways of solving this problem? By the way, I notice that a ''DEM collision model'' is inside the DPM, will that help me to create a physical radial boundary for every particle in my system?
Secondly,as for the volume limitation issue for DPM, does it possible to add a volume limitation to it and make it cooperate with DDPM?
Thank you again for your kind reply and I am looking forward to your suggestions
March 14, 2022 at 3:06 pmRobForum ModeratorThe DPM - DDPM model has seen work in 2022R1 so check the notes in that version to address the packing issues.
DEM collision is an interesting model, but tends to require very small time steps to avoid particle overlap (read the theory).
If the near wall cell is large that'll help reduce particle wall proximity. However, it also means the whole cell is in the near wall region so velocity gradients are less well captured: particles entering the cell may get stuck in the boundary layer.
March 18, 2022 at 11:44 amyyds4092SubscriberHi Rob Thank you for your suggestions.
As I cannot give up the accuracy of the velocity field, I decided to try the DEM model. However, the solid particles could still attach to the wall. Therefore, I am wondering does it is possible to stop the Fluent solver to calculate the single-particle DPM trajectory when this particle gets close to the wall?
March 18, 2022 at 1:42 pmRobForum ModeratorYou can set a trap condition, that'll remove anything that hits the wall, so will also remove the high energy "bouncing" particles. Otherwise you need to figure out the particle termination criterion and use a UDF. Altering the maximum number of steps can work, but as with the trap will also remove particles that are just taking their time to pass though the domain.
March 18, 2022 at 3:49 pmyyds4092SubscriberDear Rob
Thank you for your suggestions. I will figure it out. Have a nice week!
March 22, 2022 at 12:41 pmyyds4092SubscriberHi Rob I tried the trap wall condition but it makes my simulation diverge. When some particles were trapped by the wall, the pressure term was diverging and the solver failed to stabilize the system. The possible reason for this might be because of the solid pressure considered in the DDPM model is imbalanced as particles get trapped. And if I try to stop calculating particle trajectories by altering the maximum number, a similar error occurred. Therefore, I think in order to balance the pressure term of the whole system, I cannot give up particles attaching to the wall. Thus, does it possible to keep particles away from the pipe wall? For example, use a UDF code to reflect the particles away from the pipe wall when the distance from the centre of particles to the pipe wall reaches 1 mm (the radius of the particle). I read the reflect boundary condition in the Fluent UDF Manual. However, I found it does not use the distance to justify the reflection, in other words, the reflection UDF is still worked on the physical pipe wall boundary. I am wondering if it is possible to use the radial distance away from the wall as a reflection condition by UDF in Fluent?
March 24, 2022 at 4:38 pmRobForum ModeratorYou can trigger a direction change using a UDF, you're looking to alter the momentum. How high is the particle loading? Ie do you really need DDPM to be on? You really need to explain what you're modelling here: we can answer the questions but I suspect you're not asking the right ones.
March 24, 2022 at 7:40 pmDrAmineAnsys Employee.
March 24, 2022 at 7:41 pmDrAmineAnsys EmployeeTry please with High Resolution Tracking. And explain more
March 24, 2022 at 7:42 pmDrAmineAnsys EmployeeHow many particles do you have?
March 29, 2022 at 1:21 pmyyds4092SubscriberDear Rob and Dr Amine Sorry for the late reply. I was dealing with the coding of DPM_SCALAR_UPDATE and didn't check the question forum. But thank you very much for your replies.
Basically, I am modelling particles flowing in a horizontal pipe by Lagrangian-Eulerian tracking. Currently, the volume fraction of the particles inside the pipe is 20 vol% and I need to inject 47000 particles per second. The solid loading would go higher if I manage to achieve 20 vol% cases.
Therefore, I use DPM and DDPM to achieve my target. However, for DPM, particles are regarded as massless points and they will get into the inflation laminar mesh layers that are close to the pipe wall. Particles are trapped there. Thus, I am now trying to reflect the particles by changing their velocity directions using DPM_SCALAR_UPDATE.
The basic code is like this:
/* calculate the radial position of the particle, x is the flow direction and YZ plane is the cross-section of the pipe*/
real R = sqrt(TP_POS(tp)*TP_POS(tp) +TP_POS(tp)*TP_POS(tp));
/* define the true physical boundary, pipe radius=0.02, particle radius=0.001 m, so physically, particle should never get into the R>0.019 region*/
if (R >= 0.019)
/* if the movement of the particle is towards the boundary, then reflect it by turn that velocity to the opposite side*/
if (TP_POS(tp) > 0 && TP_POS(tp) > 0)
if (TP_VEL(tp) > 0 )
TP_VEL(tp) = -TP_VEL(tp) ;
if (TP_VEL(tp) > 0 )
TP_VEL(tp) = -TP_VEL(tp);
/* for other quadrants, the same*/
if (TP_POS(tp) >= 0 && TP_POS(tp) <= 0)
The code does reflect most of the particles away from the boundary but some of them still break the boundary and get into the laminar layer(0.019
March 29, 2022 at 2:44 pmRobForum ModeratorAre you trying to model dune formation and saltation? From what you've described I'd be using the Eulerian granular model.
March 29, 2022 at 5:07 pmyyds4092SubscriberHi Rob I am modelling the solid velocity profile and particle volume distribution in the pipe fluid. I tried the Eulerian granular model simulation and managed to work it out. However, as I got the lagrangian data from experiments, I am now more interested in comparing simulation and experiment data and looking into the solid-liquid multiphase flow system to investigate particle-particle and particle-wall interactions, where the E-E simulation does not provide this kind of information. From your professional perspective, I am wondering if I am on the right way to solving my issue (in my last post)?
March 29, 2022 at 6:31 pmDrAmineAnsys EmployeeYour particles are quite big and I assume in certain regions the mesh is smaller than the particles. At the same time you have many particles so macroscopic particlescwill be expensive. Please consider other approaches.
You can create an interior surface of revolution on which you define a dpm bc to reflect particles.
March 30, 2022 at 9:16 amyyds4092SubscriberHi Dr Amine Thank you for your reply!
To avoid particles bigger than mesh cells, I just initially used very coarse mesh. Therefore, the velocity and solid volume distribution were not perfectly matching with experimental results but still catching up with most of the solid-liquid flow behaviours. I want to improve it for further investigations. Thus, I add very fine inflation layers at the wall but these layers trapped particles and affected my results. Thus, I tried to use UDF (the DPM_SCALAR_UPDATE macro I mentioned earlier) to keep particles away from the inflation layers. Although most of the particles were away from the wall, some of them still trapped. Do you have any suggestions on this issue?
Secondly, as you mentioned adding an interior DPM wall to the system, I am very interested in this idea! Could you please explain it a little bit more? I am wondering if it means creating two domains in the meshing procedure (I am using ICEM) and importing them into Fluent?
March 30, 2022 at 11:43 amudni12SubscriberHello Currently I am working for spray drying process for different salts like Nacl, Mgcl2 and wanted to simulate atomizer and drying process in Ansys fluent suggest me appropriate boundary conditions and methodology. I have used DPM for that and injection boundary condition but results are not up to the marks.
March 30, 2022 at 12:34 pmDrAmineAnsys EmployeeYes two cell zones separated by an internal boundary. Mesh is conformal. The interior boundary you use it as porous jump BC where you tell Fluent to reflect particles.
March 30, 2022 at 12:34 pmDrAmineAnsys EmployeeI still however think to rather avoid using DPM if the mesh is in the same size as the particles.
March 30, 2022 at 12:39 pmDrAmineAnsys Employeejust think about particle radius and particle to wall distance and that in DPM there is no volume displacement and the particle will first need to touch the wall (it's center) before feeling its presence. Generally large particles will have enough momentum to just penetrate thru the laminar BL so that it should not get stuck there. If this is not the case then additional considerations are required.
Do you require the gas phase to be accounted for?
March 30, 2022 at 3:35 pmyyds4092SubscriberDear Dr Amine
Thank you so much for your suggestions!
I tried the porous jump boundary. However, when I defined the porous jump boundary and turned on the DDPM model, it got the warning: "Warning: The porous-jump zone type is not valid with currently enabled models. Change zone type or enable appropriate models before proceeding". I am wondering if it is not fit with the DDPM model or if I did something wrong.
As for your 2nd comment, I'd like to avoid the DPM model as well since its initial assumption is massless dilute particles. However, I already tried the E-E DDPM model and the results were validated by the experiment data. I need to get lagrangian data to push my study further. Initially, I thought the DDPM model, which was proven by the E-E results, could help the DPM to perform better and it did work for most of the pipe regions except for the boundary wall.
For your third comment, I think it might be because of the turbulence random walk model. Moreover, I found the velocities of these trapped particles are zero or negative to the flow direction, which probably means the drag force calculated in that boundary cell is in the opposite direction. I changed all the drag force models but not worked. Anyway, I still doubt that the DPM calculation for such big particles at the fine wall layers was wrong and the best choice is to keep particles away from the boundary. And I need to consider the fluid phase velocity since I got experimental results for validation.
April 25, 2022 at 3:23 amMahdiSubscriberCould you get any solution for your problem? I have some similar issues.
May 6, 2022 at 9:37 amyyds4092SubscriberHi Mahdi I did not manage to solve the problem. I am still trying to work it out and I am doing smaller particles.
Viewing 23 reply threads
December 20, 2022 at 11:30 amPedro AlvesSubscriber
I have the same problem that you described regarding reflecting the particles one radius away from the wall. Have you managed to find a solution?
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?
- Heat transfer coefficient
- 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
© 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.