Learning Forum

[venkat2810]

Greetings,

I am a PhD student in the US and am currently working on a project which inolves CFD-DPM in Ansys Fluent. I have a simple rectangular 2D domain in Ansys Fluent and I want one corner of this domain to be initialized with particles(say 10,000 particles) at t=0s in a transient simulation. Could you please let me know if there is a way to do this? Thanks in advance

[Rob]

What sort of volume fraction will that give? You could use a transient injection so it's only going to trigger once, you may need to use the volume release depending on what you're actually modelling.

[venkat2810]

Hello . Thank you for responding. I am not entire sure what he volume fraction here would be because I don't intend to do a multi-phase simulation. The idea is to have the particles inside a simple 2D rectangular domain (filled with water) when the simulation starts at t=0. From then on, I want these particles to start 'diffusing' within the 2D domain and distribute themselves inside the domain. For the diffusion part, I am hoping to just use 'multi-component diffusion' under 'species transport'.

[Rob]

DPM particles don't diffuse as such, they're discrete "lumps" of material. So they'll go with the flow, float or sink depending on size and properties.

[venkat2810]

I see. But is there a way to start a simulation with particles present in the domain already at t=0s? Ideally in a transient cfd dpm injection, the injection starts at t=0s and continues until the specified time limit. Alternatively, I am looking to cut down on the injection time and just start my simulation with particles already inside the domain. To summarize, my 2D rectangular domain should have 10,000 particles in it after initializing the setup. This is my 2D domain.

[Rob]

You'll need a transient injection, and then either use a volume release or injection file. If you set the time so that the injection only happens once, ie injection start & stop times are close enough to only trigger once you'll get a number of parcels added to the domain. Read up on parcel theory in the DPM bit of the theory guide: you may not see 10k particles, and almost certainly don't need that precise a number in the system.

[venkat2810]

. Thank you for the input!

[ai0013]

 

As suggested above, you can try:

(1) The injection file. For that you’ll need to specify parameters such as

(( x  y  z  u  v  w  diameter  temperature  parcel-mass  mass  n-in-parcel  time  flow-time)  name)

in a raw ascii file. You can control the injection by start-time and stop-time.

 

(2) Alternatively, if during the pre-processing you prepare a mesh that distinguishes a fluid region where the parcels are to be injected. You can later use an “artificial” surface injection selecting the proper int_fluid region. Then, the parcels will “sprout” from the face centres of such region.