Injection of fine dust using the AEROSOL parameter

[Aliaksei Patsekha]

Dear all,

I would like to ask for a piece of advice on the following matter. I am trying to simulate the injection of fine dust (diameter of 1 micron) inside a square space using the AEROSOL function.

The dust properties are as follows:

&SPEC ID='Dust', MW=60.08, AEROSOL=.TRUE., DENSITY_SOLID=2270.0, CONDUCTIVITY_SOLID=1.1, MEAN_DIAMETER=1.E-6/

The dust mass flow rate is 0.012 kg/s.

I am trying to implement two ways of adding these dust "particles" into my space.

 

1. By initiating a dust cloud:

&INIT ID='Dust Cloud', SPEC_ID='Dust', MASS_FRACTION=0.009942, XB=0.0,1.0,-0.5,0.5,0.0,1.0/

The dust mass fraction is equal to Mass_Dust/(Mass_Air+Mass_Dust).

If consider a 1 s injection (it gives 0.012 kg of dust), then MASS_FRACTION=0.012/(1.195+0.012)=0.009942 kg/kg.

This approach works fine until the mass of the added dust increases. For example, for theoretically obtained 0.012 kg (for 1 s) the simulated mass is 0.0119 kg (that is pretty good), but when comparing the dust mass within 50 s, then it is 0.6 kg (in theory, with the MASS_FRACTION=0.33426) against 0.484 kg (simulated). And this difference in masses gets bigger with the increasing time (added dust amount):

I would appreciate any suggestions on how to fix this situation.

And for this method, I'd like to ask how accurate would it be to introduce a cloud of tracers to follow the dust "particle" movements. Or are there any better options for this?

 

2. But the described method (1) is good to introduce a one-time portion of dust. When a continuous dust injection is needed (e.g., during X seconds), I think it's possible to use the MASS_FLUX parameter.

The dust injection through a circular hole (0.1 m in diameter, A = 7.9E-3 m2) in the wall is described as:

&SURF ID='Dust Hole', MASS_FLUX=1.5279, SPEC_ID='Dust'/

&VENT ID='Dust Vent', SURF_ID='Dust Hole', XB=1.0,1.0,-0.1,0.1,0.4,0.6, RADIUS=0.1, XYZ=1.0,0.0,0.5/

where MASS_FLUX=Mass_Flow/Hole_Area=0.012/0.0079=1.5279 kg/(m2*s).

According to simulation results, this approach works well in terms of the added amount of dust, but the only concern is that dust (from the hole on a wall) just "falls" down on the floor and, as a result, only a low (experiments showed a higher level above the floor) dust cloud is formed.

I tried to add a velocity to these dust particles to imitate a stream of air with dust:

&SURF ID='Dust Hole', MASS_FLUX=0.6,1.5279, SPEC_ID='AIR','Dust'/

The behaviour of the resulted ("accelerated") flow is more like a water jet, and again, the dust is not dispersed within the volume and quickly drops down to form a low dust cloud just above the floor. Maybe it should be like this because of the “hole” area and high dust density emitting from the surface?

I'd appreciate all the comments.

BR
Aleks

[dr_jfloyd]

The AEROSOL routine in FDS does not turn the dust into true particles. The species is still tracked as if it were a gas just that the species transport equation has a drift flux term applied to it for gravitational settling and thermophoresis. By setting MW=60 your aerosol species has twice the density as the ambient air whose MW is ~29. This is probably the primary reason your dust is dropping quickly to the floor and once the species hits the floor it gets removed from the gas which is probably why you are seeing the divergence. Setting the gas MW to that of air would avoid this issue. 

Using AEROSOL on SPEC works best when the aerosol mass fraction is not that large and the particle sizes are small. For typical FDS fire applications soot mass fractions are fairly low. With your VENT you are injecting almost pure aerosol, and the AEROSOL feature was not intended for this kind of application.

You may want to try using PART, MATL, and SURF to define the particle size and mass. 

[Aliaksei Patsekha]

Dear Dr. Floyd, thank you for your reply.

As expected, the change of the gas MW to 28.8 resulted in a gas stream normally directed from the VENT surface with the U-velocity ≈1 m/s. This velocity depends on the MW and I wonder are there any ways to set up or control it in a simulation. 

And a few questions, related to gravitational settling.
How accurate the gravitational deposition would work in this case (change of the MW from 60 to 28.8)? Would this change somehow cause a need for correction in the required MASS_FLUX of “dust”?

Why does the settling of aerosol species look as expected (slow fall) even with MW=60 when the aerosol is injected inside a volume through the INIT line?

Thank you and  BR

Aleks

пятница, 27 мая 2022 г. в 15:08:54 UTC+2, dr_jfloyd:

[dr_jfloyd]

With AEROSOL, the species uses the exact same transport equations as a gas species without AEROSOL.  The only change is there is an additional forcing term added for thermophoresis and gravity. This term is dependent on the solid particle properties as discussed in the Technical Reference Guide. The MW does not play a role in this additional term.

With INIT you are placing a small mass fraction into a volume. The average molecular weight of the gas in that volume is going to be very close to the average molecular weight of the gas outside that volume. This means no density difference for the gas transport. With your VENT, the aerosol species was a significant portion of the mass. So the average molecular weight of the gas near the vent was much higher than the rest of the domain making it much more dense, so you get a negative buoyancy for the gas plus the additional settling for the aerosol.