February 3, 2022 at 11:04 amLorenzo_PSubscriber
Hi, I'm trying to replicate a particle (allumina) - gas (air) flow in a converging-diverging nozzle found in an academic paper. I'm following an eulerian-lagrangian approach for a steady state problem. Here some data:
- particle mass fraction = 30%
- Injection type: surface, position: inlet.
- Axisymmetric problem (2D geometry, surface body)
- MESH: 60 cells in radial direction, 150 cells in axial direction.
- Particle diameters: 100 micrometer, 50 micrometer, 30 micrometer, 10 micrometer, 2 micrometer
- B.C. INLET: pressure inlet; WALL: specified shear = 0 (in order to avoid the boundary layer generation) OUTLET: pressure outlet.
The results are good only for 100 micron particles (they match with the ones of the paper), while for smaller particles the solution is completely wrong. I get a huge DPM concentration next to the axis (order of magnitude bigger than in the rest of the domain), which leads to an enormous momentum/temperature lag and therefore to a wrong gas mach number and temperature distribution near the axis.
I have also tried to implement the full 3D case, but I get a similar error this time near the walls. Basically, when I am injecting particles with a diameter smaller than 100 micron, the DPM concentration results wrong and therefore all other gas variables. Have you got any hint about what happens ? I thought that it could be related to the big number of particles injected: maybe Fluent cannot track so many particles and as a consequence it introduces a numerical error which leads to the wrong DPM concentration. Thanks for your help.February 3, 2022 at 11:38 amRobAnsys EmployeeGiven you're injecting parcels and not particles (I know the TUI reports aren't clear on this) the size shouldn't effect anything other than drag. For 30% mass fraction I'm assuming volume fraction is under 10% and you're using the "interacts with continuous phase" option. Please can you post some images? Velocity field and particle tracks would be useful.
February 3, 2022 at 12:02 pmFebruary 3, 2022 at 12:06 pmLorenzo_PSubscriberI also want to underline that for what concern DPM concentration, the values far from axis (between 20 and 45 kg/m^3) are correct and similar to the ones of the paper. Only the axis region is completely wrong. Thank again for your help.
February 3, 2022 at 2:33 pmRobAnsys EmployeeIs this CFX or Fluent? Can you replot the concentration with a different range? I think the concentration is skewed by the cell volume: at the centre it's low as you're next to the axis.
February 3, 2022 at 3:01 pmFebruary 3, 2022 at 3:04 pmLorenzo_PSubscriberAs you can see, near the axis of the nozzle (the line on the bottom of the geometry) the DPM concentration is greater than above. Maybe here the volume mass fraction exceeds the maximum of 10%?
February 3, 2022 at 4:41 pmRobAnsys EmployeePossibly, replot with the maximum level reduced to around 3. If you look at the results in Fluent it may make more sense.
February 3, 2022 at 4:54 pmFebruary 3, 2022 at 4:58 pmLorenzo_PSubscriberAlso I have used the only gas solution, which is correct, to initialize the particle-gas one.
February 3, 2022 at 5:13 pmRobAnsys EmployeeInitialise from the inlet and let the solver sort itself out.
Those plots look about right. Basically the axi-symmetric approach means the cell sizes are messing with the DPM concentration plots as the cell "volume" near the axis is small compared to nearer the outer radius. Try scaling the injection by surface area. But then note the parcels won't all have the same mass.
February 3, 2022 at 5:23 pmLorenzo_PSubscriberThank you, I'll try it. To scale the injection by surface area do you mean to activate the option "Scale flow rate by face area"? And if so, how do I need to modify the value of total flow rate of particle? Can I leave the same value?
Again, thank you for your support.
February 4, 2022 at 12:13 pmRobAnsys EmployeeScale flow by area and see what happens. You'll still get a parcel released from each inlet facet but the parcel mass should vary. I can't remember how intelligent the function is with axi-symmetric meshes.
Leave the mass as is: it's your setting for the injection so the solver will add that amount of mass (per PI or 2PI radians - can't remember but it's in the manual).
February 4, 2022 at 2:27 pmLorenzo_PSubscriberHi, now the simulation seems working well. I'm going to post some images of the charts I have obtained for the 10 micrometer particles, related to the DPM concentration and mach/velocity contours. Maybe, as a further improvement, should I set two types of injectors, one without the "scale flow" option and the other one with the "scale flow" option ? For example, since I need to inject 0.6 Kg/s of particles, I could set a surface injector which releases 0.3 Kg/s of mass flow without the surface scaling and another surface injector with the surface scaling which injects the remaining particle mass flow. I don't know if this makes any sense, but it would help to keep the parcels mass more uniform.
You have really saved my thesis, again thank you!
February 4, 2022 at 3:41 pmRobAnsys EmployeeYou're welcome. Now it's established what the problem is, you need to decide what to do about it. Setting the scale by area means you're now tracking variable mass parcels so there's more DPM mass in the "outer" parcels than those on the centre line. This may or may not be something to think about.
As an aside, staff are not permitted to open attachments so please repost the images.
February 4, 2022 at 4:29 pmLorenzo_PSubscriberThis is the DPM concentration in the global range.
this is the dpm concentration with the maximum fixed at 3 Kg/m^3.
This is the Mach number.
So, in the end, if I have understood well, the problem is related to the different volume of the cells: it is smaller for the cells near the axis with respect to the cells in the outer region. This is beacuse in axisymmetric problem the geometry is represented as a "clove" of some degrees of the whole 3D body. As a consequence, it fails to manage the DPM concentration near the axis, causing the errors we saw. Is this a good explanation?
Viewing 15 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
Top Rated Tags
© 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.