June 21, 2022 at 1:58 amreza121Subscriber
In the following problem, I have a geometry consisting of multiple layers of screens that are supposed to filter out the particles from the incoming contaminated flow.
A steady K-Omega SST turbulent model is used to solve the flow. The duct dimensions are 0.4*0.4*15 mm. There is a one-way interaction between the particles and the flow. Therefore, the flow is solved first. After convergence (errors down to 1e-10 or lower), the particles are injected at the inlet using the group feature (3 groups of 20 parcels) with the same velocity as the flow at the inlet. the particle size is 1 micron and their mass flow rate is 1e-20 (infinitesimal).
In the following, you can see a screenshot of the CFD mesh. 7 layers of inflation are added. The cell size close to the walls zone is 4e-6m and away from that (I call it downstream and upstream of the domain) is 8e-6 in one case and 16e-6m in the other. The problem is that the number of trapped particles on the walls is dramatically different in these two cases while the CFD mesh is different only away from the walls. I have checked the Z-velocity (the velocity along the duct) as a grid study parameter and the graphs align very well. So, the grid resolution seems to be sufficient. However, DPM results are different and we know that for Lagrangian solutions, as long as the flow is converged and consistent (for the drag forces), DPM results should not vary with the grid size since it just calculates the particles' trajectories by solving F=ma for each particle along its path.
additional information: BCs: velocity inlet (1.7 - 3 m/s) pressure outlet (0 gauge) Symmetry walls on 4 side walls of the duct, no-slip walls for the screen walls.
Please help me with what I should do.
Thanks in advance
June 21, 2022 at 9:05 amRobAnsys Employee
The images aren't showing, but I suspect that's the new software having some glitches removed: IT are playing whack-a-mole with the forum gremlins. Normal service will be resumed once we've caught them all....
For a 1micron particle you'll have virtually no inertia, so they'll closely follow the flow. As you resolve the flow boundary layer, what flow feature will help the particles penetrate to the wall? Inertial separators at that scale are difficult to model so check the overall mesh resolution and flow field. The near wall cell is deeper than the particle which is good, so at least you should predict hitting a wall.
June 21, 2022 at 9:52 pmreza121Subscriber
Thank you so much for your reply, Robert.
I have been reading Dr. Amine's and your comments on different topics in the forum in the past few years. I am so excited that you are helping with my problem now!
Unfortunately, I couldn't upload the photos with the description. I even tried uploading them on google drive and sharing the link (even though I know you prefer not to click on the links) but that didn't work either. Do you have any idea on how I can share the photos? It'll help a lot with the illustration of the problem.
I have cylindrical walls (representing screen wires) that are subtracted from the bulk air duct. The wire diameter is 100 microns and the screen opening is 200 microns. My domain is purely made of air with the walls subtracted. The walls are solid and not porous and a "trap" DPM boundary condition is applied to them. Therefore, neither the flow nor the particles pass through them. Yes, I am trying to count the number of the particles that will hit the walls and then will be eliminated from the domain and will be counted as captured in the report.
June 21, 2022 at 9:18 amDrAmineAnsys Employee
I like the tracer idea: it wil just trace: do you see Flow penetrating the wall? If not then what will the tracer do?
June 27, 2022 at 8:30 pmreza121Subscriber
Dear Dr. Amine,
Will you please reconsider this problem now that the photos are uploaded and hopefully the problem is clearer?
All the walls (screen wires) are set to "trap" the particles in their DPM setting tab. They are solid walls and neither the flow nor particles penetrate them.
The issue is that even though the flow parameters show an identical trend with all the different mesh resolutions (scatter plot of flow z-velocity on a line according to one of the uploaded photos or skin friction factor on the walls), I am getting different numbers of trapped particles at the walls with different mesh resolutions in either vicinity of the walls or away from the walls. As I explained earlier in the previous posts, using the "body of influence" meshing feature, I give fluent meshing two mesh element sizes: one in the vicinity of the walls (called vicinity region) and one away from that (which I call up/downstream)
Here are some of the particle trap results for different mesh resolutions:
1- up/downstream 16e-6 , vicinity 4e-6. # trapped= 50/60
2- up/downstream 8e-6 , vicinity 4e-6. # trapped= 35/60
3- up/downstream 4e-6 , vicinity 4e-6. # trapped= 26/60
In the studies above, I kept a constant mesh size for the vicinity region and changed the mesh size in the up/downstream region only. Also, in another study that I carried out earlier, I kept the up/downstream mesh size constant and changed the vicinity mesh size and the DPM results still change drastically. In the photo below, you can see better what I mean by vicinity and up/downstream regions.
June 22, 2022 at 3:59 pmRobAnsys Employee
The not clicking on links or downloading attachments is one of the rules we have to follow - otherwise we're not permitted to answer anything due to Export Law.
If you abuse the cell zone reference frame to set the reference axis along one of the wire cylinders what is the fluid approach velocity towards the surface? If you plot the particle track how does it alter towards the mesh surface?
June 25, 2022 at 7:01 amreza121Subscriber
I am not sure if I understood your point here, Robert.
As you can see in the photos, the wires are not straight cylinders and are curved. This is what the particle track looks like for a group injection of 5 parcels for 2 different cases. The body of influence feature has been used for mesh generation and CFD mesh size close to the walls is 4e-6m for both cases and the mesh size up/downstream of the walls is 8e-6m in one case and 16e-6m in the other. All the other settings are the same for both cases and only mesh size has changed)
in the images below, you can see that a specific particle injected at the same location and velocity and ... in both cases ends up getting trapped in one of the cases and in the other one it maneuvers and passes the wall and ends up escaping the domain at the outlet.
Please note that what you see in the photo is the 4th screen layer and the particle track is coloured by its distance from the wall in the range of [1e-8 to 1e-6m].
June 25, 2022 at 7:02 am
June 25, 2022 at 6:21 am
June 25, 2022 at 6:22 am
June 25, 2022 at 6:22 am
June 25, 2022 at 6:22 am
June 25, 2022 at 6:23 am
June 25, 2022 at 6:29 amreza121Subscriber
Dear Dr. Amine and Robert,
After sending an email to Ansys Community Help, I am able to upload the photos now. I apologize for the inconvenience. Please read the problem description again, considering the screenshots this time.
Using the "Body of influence" feature in meshing, I have created a denser mesh in the vicinity of the walls (screens) but by changing the mesh resolution either in that area close to the walls or far away from them, I get different numbers of trapped particles after particle tracking.
June 27, 2022 at 1:19 pmRobAnsys Employee
No worries, we're still wrapping up the migration, so expect a few of the glitches to disappear in the next few weeks.
OK, with 90 particles you're also subject to statistical issues. Assuming it's turbulent switch on turbulent dispersion and number of tries to 10-100. You need alot more particles.
The difference may be mesh/flow related, but could just be injection position and luck, hence putting in many more parcels.
June 27, 2022 at 7:42 pmreza121Subscriber
I kept all the turbulence dispersion features off in the DPM settings. I will use them in my final study.
I know that based on the Random walk theory, a u'=\zeta * sqrt (average (u'^2)) term will be added to the flow in which zeta is a normally distributed random number meaning that I will get different DPM results even with the same mesh and settings if I track the particles twice in a row. to avoid that, I kept it off and am still getting different DPM results for different meshes.
June 28, 2022 at 6:33 pmreza121Subscriber
Please let me know if additional information is required. Thanks.
June 30, 2022 at 11:19 pmreza121Subscriber
How does this forum work? You and Dr. Amine asked one or two questions at first and I answered them. but it's been a couple of days that I haven't heard back from you guys. Should I wait for you to come back for my problem? I'm afraid that you forget to do that considering the large number of new questions that you receive daily.
June 27, 2022 at 9:35 pmreza121Subscriber
Dear Robert and Dr. Amine,
There are two theories that I have about this problem that I'd like to share with you and ask your opinion about:
1- I know that DPM tracks the particle trajectories point-wise and doesn't consider the diameter of the particle and updates the particle path by integrating F=ma for each particle in each time step. According to the model, if the center of a particle comes in contact with a wall cell, that particle will be considered trapped and will be eliminated from the domain (please correct me if I'm wrong).
Having said that, I may need a higher mesh resolution (larger number of cells) on my walls and close to the walls to better capture the wall geometry curvatures and therefore particle paths close to the walls. As a reminder, my wires are 0.05 mm in diameter and my finest mesh size around the walls was 4e-6 m. According to the two photos that I sent as a reply to Robert on June 25, 2022, at 7:01 am, you can see that particles may follow different paths in case of different mesh resolutions close to the walls. It is noteworthy that I already have 7 inflation layers and based on velocity vectors close to the walls, I already have more than 10 nodes in my boundary layer and also my y+ value is about 0.015.
On the other side, as you can see in the post on June 27, 2022 at 8:30 pm as a reply to Dr. Amine, DPM results change even when I keep the mesh size around the walls constant and change the mesh size up/downstream only. It leads me to my second theory that:
2- the flow (velocity and pressure field) may actually not be fully resolved. As described earlier, I see an identical trend of the Z-velocity plot on a line drawn parallel to the flow direction (please refer to the following images). However, when I report Z-velocity on a specific point in the domain, I see up to a 10% difference in z-velocity for different mesh resolutions. These local differences may change the particle path since it will appear in the drag force on the particle in F=ma.
If this is the reason for my issue and I still need to decrease my mesh element size, what is a better criterion to check whether the flow parameters are fully resolved?
June 27, 2022 at 9:35 pm
July 11, 2022 at 3:21 pmRobAnsys Employee
Simply, we answer questions as we see them and we're on here: the "day job" for Amine and I is European support, which includes pretty much anything involving Fluent and our customers. So, we've not forgotten but with the recent forum downtime we might miss questions by not being on for a few days. In theory the new system is going to catch unanswered questions, but it's still being deployed.
The particle count will be low without the stochastic tracking, and you need more particles to ensure you get a statistically meaningful result. Yes, it may differ slightly, so you may want to do the tracks a few times and take an average. If the solution is changing with different mesh size/count it could be you've not got a mesh independent result. However, given the size of the particles a small deviation in flow could have a significant effect on the capture rate.
The particles will contact the wall if they're in the near wall cell, and then I think the diameter is checked against the position, can't find the DOC reference though. If the particle is bigger than the cell and isn't in the near wall cell it won't hit it.
July 14, 2022 at 1:06 amreza121Subscriber
Thanks for your reply Robert,
I am injecting 716 particles using the surface injection. To test whether it is enough or not based on what you suggested, using the group injection feature, I once injected 1900 particles and then injected half of that number, 950 particles. The percentage of trapped particles was exactly the same for both of the injections. Please refer to the screenshot. therefore, I believe the number of injected particles is sufficient.
With the Random walk model activated, I used to get different results each time I tracked particles, but I get the same number of trapped particles. The good news is that this number is not changing for the different mesh sizes. So, I'll keep the model activated for my future studies. however, I would still like to know why my results are changing with mesh when this model is not active since one part of my research is studying the impact of the random walk model on the particle capture results.
For the mesh independence, as you can see in the previous posts, for different mesh size cases, I plotted flow Z-velocity on a line that is parallel to the flow and I can see that the results are matching very well. Moreover, in order to study the velocity close to the wire walls, I created rings around a wire and plotted the velocity magnitude on this ring for different mesh size cases. Again, the velocities are perfectly matching for the 2 mesh sizes (8e-6 and 16e-6m) You can find the relevant photos in the following. Consequently, I believe my flow is mesh-independent and the problem must be coming from the DPM settings. I would be glad to further analyze it if you have any suggestions to investigate the mesh independency in a better way. By the way, the skin friction factor is also identical for the two mesh cases (up to the third decimal digit).
I think DPM is considering the particles point-wise and doesn't consider their radius in the capture criterion. The reason I say so is that I can see that some of my particles get closer than a radius distance to a wall but won't be considered captured and escape away eventually. please let me know if you found any documents on how "trap" on walls works and whether I'm wrong. Although my particles are small and this won't be a big deal for my case, it's good to know how the model works.
Thanks for your time
July 14, 2022 at 1:07 am
July 14, 2022 at 1:09 am
July 14, 2022 at 1:10 am
July 14, 2022 at 1:23 amreza121Subscriber
By the way, I also tried the Random walk model whit number of tries = 1, 10, 20, and 50 and I get similar results for all of these cases for different mesh sizes- ~33% for all of them (As I said, with the Random walk model activated, there seems to be no problem with the mesh sizes). So, again, I think that I am injecting a sufficient number of particles, and whatever the problem is for the random walk-off case, it must be with my DPM settings. Do you have any thoughts on that?
July 22, 2022 at 10:48 amRobAnsys Employee
How large are the cells (wall normal distance) relative to the particle size? We only check for wall proximity in the near wall cell.
July 22, 2022 at 10:49 am
July 22, 2022 at 6:52 pmreza121Subscriber
The particle size has always been 1 micron for all the cases I have studied so far. The smallest I will ever track later will be 0.1 microns.
here's a screenshot of the Cell Wall Distance reported in fluent on my walls. I got it using the following path:
reports>Area-weighted average>mesh>cell wall distance> All my walls
Also, Using Fluent meshing, I selected one random near-wall element on one of the walls and measured its height. it was: Distance = 2.016724e-07 as you can see in the following photo.
I couldn't find any better way to report near-wall cell height in fluent meshing. If you know any, please let me know.
And if you are interested, here is my Y+ reported as Area-weighted average on my walls again. Based on these values, I guess my near-wall cells are too thin. I purposefully created a fine mesh to make sure that I am in a safe zone on the Eulerian side of the solution.
July 22, 2022 at 6:57 pmreza121Subscriber
Can you elaborate a little more on what you mean by "Fluent only checks for wall proximity in the near wall cell"?
What is the particle trap criterion? Is a particle considered traped as soon as its center enters the first mesh layer around a wall?
Or the particle center has to hit the wall and the distance between the on-wall mesh element and particle center has to become zero (or smaller than a certain value?) for it to be considered traped?
Thanks again for your time
July 25, 2022 at 6:33 amDrAmineAnsys Employee
Particle are mass points: so they do not displace volume. So any fate is calulcated based on the particle mass centroid and cell/boundary intersection. Check the customization manual where it lists an example how Fate Reflection is done: you can understand more how LPTM is done.
July 25, 2022 at 6:47 amreza121Subscriber
Thanks for your reply Dr. Amine.
I will check it for sure. So, what do you think? is my first layer thickness large in comparison to my particle diameter size? Is that the reason I am getting different DPM results with different mesh sizes?
July 25, 2022 at 6:57 amDrAmineAnsys Employee
I only refer here that to have consistent results with particle tracking when doing mesh sensitivity analysis then the number of streams should be increased. If you cannot afford that then stick to the "recommended" (not obligation) to have the particles smaller than the cell sizes. Your results wiuth DRW are fine so why not going the next step and be satifisfied with what you obtained?
July 26, 2022 at 1:13 amreza121Subscriber
Dear Dr. Amine,
You probably overlooked previous posts. The number of trapped particles is changing a LOT for different mesh sizes I have run so far. As you can see in the photo below, I get 77% for one mesh size and 65% for another. The purpose of this study is to investigate the impact of some parameters like wire diameter in my screens, screen layer distances, velocity and … on the particle capture rate. If I can’t get consistent results for one particular case, I won’t be able to compare my results for different cases when I am studying these parameters. Please double-check the previous posts and let me know what you think and where the problem could be.
Thanks in advance
July 26, 2022 at 5:52 amDrAmineAnsys Employee
But you are getting proper results when random walk is on and that what one is aming for.
Do you know the goal of random walk? Do you know why increasing the number of trajectories is important whenver one wants to make a mesh sensitvitiy analysis?
July 26, 2022 at 10:15 amreza121Subscriber
Dear Dr Amine,
I explained above that because I want to compare the results of random walk on/off cases and study the impact of this model, I still need to get random walk off work properly too. Besides, I'm still worried that something might be wrong with my DPM settings because when RWM is on, for different inlet turbulence cases, my DPM results do not change while based on the guide, u'=zetha*sqrt(2k/3). What do you say? Am I righ? Should it change?
I know that the required high number of parcels is related to probability and statistical issues. However, I explained earlier that the problem when random walk is off, is not coming from insufficient number of parcels. Because, using group injection, I created twice that number of parcels and the results were still the same (same percentage of trapped particles.)
Please correct me if I'm wrong in any part of the above discussion.
July 26, 2022 at 10:17 am
July 26, 2022 at 11:14 amDrAmineAnsys Employee
The one part will be the number of streams and the other part will be how to make trajectories more realistic: that is where the DRW and number of tries are trying to achieve.
July 26, 2022 at 3:20 pmreza121Subscriber
I see. Thanks for your reply. So what do you think about the number of trapped particles not changing with the incoming turbulence? It is not what we expect, right?
I was thinking that this is because of high number of tries that many parcels fill the whole domain no matter what intensity and consequently, U' is.
Is that right?
- 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.