Learning Forum

[jaded_messiah]

Hello there! I am simulating flying of inert water particles in the air and have a problem. I have a pipe with massflow inlet (0.055 kg/s) and want to enter water particles flow rate 0,011 kg/s. BUT! What this velocity means? I thought this is "starting velocity" but if i enter 0 - the particles not appear at all. Please, exlain to me what this velocity doing.

[ai0013]

Hello
DPM mass flow rate and DPM initial velocity are independent inputs for your point injection. Note that this is a discrete mass flow rate and not a continuous mass flow (m_dot = rho*vel*area is not valid), instead m_dot = # particles / sec * mass_particle. If you set your DPM mass flow rate you know the mass of the particle based on density and diameter, the # particles / sec (usually referred as the "strength") is the reciprocal of your particle time step.

We have not specified any velocity here yet, so that's why you need that input too.

[jaded_messiah]

Thanks a lot, comrade! If i may ask, i want to make it clear that i understand it the right way. For example i want get 100 particles per second. Every particle mass is 5e-7 m, then mass flow must be 5e-7 * 100 = 5e-5?
Also, can i write to you via email or smth? I doing my dissertation and have a couple of questions abot DPM. I'm simulating water separator for UAV and in my university there's no people working with multiphase =(

[ai0013]

Yes, just to add a bit more on the # particles / sec:
From the injection panel I see you have a surface injection. Fluent injects 1 parcel per time-step per cell face. So from what I remember, it'd be as follows:

Let's say your surface is composed of 500 cell faces, and that you have 10 diameters in the RR distribution. Imagine your particle injection time-step is 1ms.
Then # particles / sec = 500 * 10 / 0.001 s = 5e6 [s^-1]
Particle mass = pi / 6 * rho_p *d_p^3 [kg]

So based on m_dot [kg/s] , different d_p (based on RR distribution) will be injected to satisfy the mass flow rate. You see you still need to provide particle velocity [m/s] ? That's why you need it as independent input.

You can post your doubts here (As the Forum is public, everybody can benefit )

[jaded_messiah]

So, if i simulate steady state - there's only particles that appear from cell faces only once? So, if i have 100 cells, there should be 100 particles in this simulation? Also, this is strange that ansys makes user's to count it by themselve. I mean - ansys knows density of particles and number of cells, so this strange that there's no way just to enter parameter "particles per timestep".

[ai0013]

For surface injection, Fluent injects at each face centroid, but that doesn't mean that your parcel count is limited by the number of cell faces. Please check the different parcel release method in the manual (constant mass, number, etc...) What Ive just explained is valid for the standard method.
For steady particle tracking, the particles are tracked from injection point til final state, but you can still vary the number of tries.
Bsides when using RR distribution, there's the input 'number of diameters'.
Please go through the manual for more details on particle treatment.

[jaded_messiah]

Ok, thanks! I use manual but not all tnings are clear sometimes =D The most problem - eglish language is harder there.