Learning Forum

[Shak]

Good morning, 
I am confused with the DEM option in Fluent.
Can the DEM option be simulated by selecting the DPM, transient and two-way coupling options?
Or should I do it through the DDPM option (Multiphase>Eulerian+lagrangian phases)

Thank you

[Rob]

You missed Ansys Rocky coupled with Fluent. :) 

DPM has options for DEM and DDPM. The former gets you a basic DEM framework fully under the DPM model: computationally it's OK, but it's far less refined than Rocky. DDPM adds an Eulerian phase and is set partially there and partially via the DPM injections: it's intended for systems where bulk flow is dispersed but some regions exceed the DPM recommended limits. 

[Shak]

 

Hello Rob,

The truth is that some problems are causing me to work in Rocky, so I prefer to return to Fluent and compare both results.
If we talk about pneumatic conveying with a volume fraction of 10%, I would like to obtain the concentration of the particles close to the wall (volume fraction close to the wall)
Correct me, please if I’m wrong:
If I work with the DPM option, I should only inject the particles, but since it operates under a one-way Copling, the volume fraction is not considered. The question I have is: so how is dem -option activated? If it is supposed to take into account the volume fraction of the particles
On the other hand, if I work with the DDPM option, I enter an Eulerian phase option (the air) and activate the option DEM and two-way coupling; I should be able to get the concentration of the particles, right?

 

[Shak]

Please, could you also guide me to plot the volume fraction close to the wall?

thank you

[Rob]

The DPM-DEM option also doesn't include a particle volume, it's only collisions that are worked out. It's an option in the DPM model panel, look in the Physical Models tab.

DDPM isn't DEM and uses the Eulerian model when the volume fraction gets higher. It'll also tend to be a transient calculation as the volume fraction tends to alter over the solution duration as waves/dunes of particles form and are broken up. 

With DPM there is a concentration option that may be sufficient - read the definition as it's NOT a volume fraction. 

[Shak]

Good morning,

I have two questions about my simulation; I would appreciate it if you could help me solve them.

1. Because my continuity equation does not converge, it did converge at the beginning, but after adding the particles, it stopped doing so. Should I reduce the timestep of the particles?

2. After many iterations, when my particles reached the top of the vertical pipe, some results it shows "reverse flow", why?
In my boundary conditions, I have placed that the pressure at the outlet is 0; also the velocity of the air in the inlet is 10m/s

 

 

Thank you in advance for taking the time to help me solve my doubts.

 

 

 

 

[Rob]

Have a look at why the flow is reversing before changing anything else.  Is there an explainable cause? What is the DPM condition set at the outlet? What is the outlet backflow condition, and how does that compare with the flow going out near there? 

Simulation is a tool, and you need to understand why something is happening rather than (always) worrying about the warnings. We use the warnings to focus our checks, but don't always correct them. 

[Shak]

Thanks for your answer; it made me think more deeply about the simulation while I reviewed the help manual again.
Please allow me to ask you one last additional question:
Having a simulation with a large volume fraction and I want to evaluate the collisions present, I would use the DDPM and DEM options. So my question is, under these conditions should I activate the Granular option offered by the DDPM? (I have read the manual, but I still have that doubt)

Thanks!

[Rob]

DEM is a pure collision model so volume fraction isn't checked. DDPM probably needs granular as the particles will spread out again based on the flow.