March 12, 2021 at 2:33 pmTE_HafSubscriberHi,nI am simulating a particle-air jet and I am interested in the particle-particle collisions. Therefore I am using the DEM collision model available in Fluent. This forces me to work with instationary particles (although I am looking for a steady solution, where the particle collisions dictate the spread). nMy idea is to inject particles, until the fluid and the particles have achieved a steady state. Due to the use of the DEM model, and the collisions between different sized particles, I am using a very small time step (10^-6) while calculating 100 particle iterations during each fluid iteration. Since I am continuously injecting particles, I thought the simulation would be too slow if I had 1 particle time step for each fluid time step, so I increased the number of particle iterations per time step to speed the process up. nThe problem is, even with the stagger Positions option active (I am using the Group injection), particles are injected too frequently, so that overlap and collisions already occur at the injection stage. nIf I change the number of particle iterations to 1 (1:1 particle:fluid iterations) the staggering of particles work. On the other hand, it gets 100 times slower. nMy question is, is there a way to control the particle injection frequency within one fluid time step? Let's say, I want to inject every 10 of the 100 particle iterations. Is something like that possible? nOr, would it be possible to make the staggering option work between particle time steps within one fluid time step? (Since I am injecting 100 times per time step only every 100 particle the injection staggering is working).nUsing an UDF I managed to switch injections on and off by changing the injection time (start/stop) each fluid time step. But then I only inject every 1 of 100 particle iterations (it only lasts one particle iteration each new time step). In this case I would have to change the number of particle iterations to 10 to obtain what I was looking for. But I think, this is just a matter of injecting every nth Particle iteration, there must be an easier way to acess the variable that controls the injections. nThat leads me to the last question. UDF are called at the beginning or end of the fluid iteration. Is there something similar, where I can make changes every particle iteration, without having to set the number of particle iterations to 1? If not, how could I skip the fluid calculation in one fluid time step? Let's say I am only interested in dry collisions (DEM Model) in sandblasting. Is that possible in Fluent?.
March 12, 2021 at 3:11 pmRobAnsys EmployeeYou can turn off the flow equations to just model the DPM/DEM particle motion. You may need to drop the carrier viscosity to avoid getting too much drag though. nYou can increase the particle time step relative to the flow step. This should reduce the frequency of the injections. n
March 15, 2021 at 8:07 amTE_HafSubscriber
You can turn off the flow equations to just model the DPM/DEM particle motion. You may need to drop the carrier viscosity to avoid getting too much drag though. You can increase the particle time step relative to the flow step. This should reduce the frequency of the injections.https://forum.ansys.com/discussion/comment/110576#Comment_110576Thanks, I will give it a try.nAbout the flow time steps, If I increase it, I end up with collisions where the velocity after collision is larger than the maximum velocity previous to the collision. My guess was, that the overlapped region of the particles is larger than it should be, resulting in a too high acceleration.nRegarding the other questions, there is no way of controlling the injection frequency, without changing the time step and the number of iterations per fluid time step, right? n
March 15, 2021 at 11:01 amRobAnsys EmployeeDEM collisions require a very small particle time step to avoid the overlap: much as you suspect. Unfortunately that also means you inject at the same particle time step. I'll stick an enhancement in you've reminded me in a way I can more easily explain. n
March 19, 2021 at 9:28 amTE_HafSubscriber
DEM collisions require a very small particle time step to avoid the overlap: much as you suspect. Unfortunately that also means you inject at the same particle time step. I'll stick an enhancement in you've reminded me in a way I can more easily explain.https://forum.ansys.com/discussion/comment/110816#Comment_110816So, is there a way to avoid injections every time step, or to control when the injections should occur? nSomething else I've observed is, that when using the Rosin-Rammler size distribution some particles are injected more often than others, and tend to overlap. nMy previous solution was setting the injection initial and final times every time step with the UDF (Group injection). It looked like: t_final= t_step+dt, where dt is the particle time step. This, however, does not work with the size distribution, since dt is not enough for the larger particles to be injected. If I use 2*dt or 5*dt to also inject larger particles, the smaller particles overlap and are accelerated several times their own velocity, which sounds unphysical. In summary, I can only have one particle size for this approach to work.nDo you have a better suggestion?
March 19, 2021 at 2:55 pmRobAnsys EmployeeYou can use the start & stop times to set up a sequence of injections, that's more time consuming to set up, hence me logging the enhancement suggestion. nRR looks at the size distribution and injected mass, and this can cause larger particles to be injected less often (as it should) but it doesn't control where they're injected. If two parcels are too close together then the resulting high velocity can become a problem. n
- 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.