Learning Forum

[Lorenzo_P]

Hi, I'm trying to replicate a particle (allumina) - gas (air) flow in a converging-diverging nozzle found in an academic paper. I'm following an eulerian-lagrangian approach for a steady state problem. Here some data:

1. particle mass fraction = 30%
2. Injection type: surface, position: inlet.
3. Axisymmetric problem (2D geometry, surface body)
4. MESH: 60 cells in radial direction, 150 cells in axial direction.
5. Particle diameters: 100 micrometer, 50 micrometer, 30 micrometer, 10 micrometer, 2 micrometer
6. B.C. INLET: pressure inlet; WALL: specified shear = 0 (in order to avoid the boundary layer generation) OUTLET: pressure outlet.

The results are good only for 100 micron particles (they match with the ones of the paper), while for smaller particles the solution is completely wrong. I get a huge DPM concentration next to the axis (order of magnitude bigger than in the rest of the domain), which leads to an enormous momentum/temperature lag and therefore to a wrong gas mach number and temperature distribution near the axis.

I have also tried to implement the full 3D case, but I get a similar error this time near the walls. Basically, when I am injecting particles with a diameter smaller than 100 micron, the DPM concentration results wrong and therefore all other gas variables. Have you got any hint about what happens ? I thought that it could be related to the big number of particles injected: maybe Fluent cannot track so many particles and as a consequence it introduces a numerical error which leads to the wrong DPM concentration. Thanks for your help.

[Rob]

Given you're injecting parcels and not particles (I know the TUI reports aren't clear on this) the size shouldn't effect anything other than drag. For 30% mass fraction I'm assuming volume fraction is under 10% and you're using the "interacts with continuous phase" option. Please can you post some images? Velocity field and particle tracks would be useful.

[Lorenzo_P]

Thank you for your answer. Yes, I'm using "interacts with continuous phase". I'm going to post the results for the 1 micrometer particles case.

[Lorenzo_P]

I also want to underline that for what concern DPM concentration, the values far from axis (between 20 and 45 kg/m^3) are correct and similar to the ones of the paper. Only the axis region is completely wrong. Thank again for your help.
Lorenzo P

[Rob]

Is this CFX or Fluent? Can you replot the concentration with a different range? I think the concentration is skewed by the cell volume: at the centre it's low as you're next to the axis.

[Lorenzo_P]

This is fluent. Yes, sure, this is the concentration with the range set as global, now I can diminish the maximum value.

[Lorenzo_P]

As you can see, near the axis of the nozzle (the line on the bottom of the geometry) the DPM concentration is greater than above. Maybe here the volume mass fraction exceeds the maximum of 10%?

[Rob]

Possibly, replot with the maximum level reduced to around 3. If you look at the results in Fluent it may make more sense.

[Lorenzo_P]

here I have plotted both in Fluent and in post.

[Lorenzo_P]

Also I have used the only gas solution, which is correct, to initialize the particle-gas one.

[Rob]

Initialise from the inlet and let the solver sort itself out.
Those plots look about right. Basically the axi-symmetric approach means the cell sizes are messing with the DPM concentration plots as the cell "volume" near the axis is small compared to nearer the outer radius. Try scaling the injection by surface area. But then note the parcels won't all have the same mass.

[Lorenzo_P]

Thank you, I'll try it. To scale the injection by surface area do you mean to activate the option "Scale flow rate by face area"? And if so, how do I need to modify the value of total flow rate of particle? Can I leave the same value?
Again, thank you for your support.

[Rob]

Scale flow by area and see what happens. You'll still get a parcel released from each inlet facet but the parcel mass should vary. I can't remember how intelligent the function is with axi-symmetric meshes.
Leave the mass as is: it's your setting for the injection so the solver will add that amount of mass (per PI or 2PI radians - can't remember but it's in the manual).

[Lorenzo_P]

Hi, now the simulation seems working well. I'm going to post some images of the charts I have obtained for the 10 micrometer particles, related to the DPM concentration and mach/velocity contours. Maybe, as a further improvement, should I set two types of injectors, one without the "scale flow" option and the other one with the "scale flow" option ? For example, since I need to inject 0.6 Kg/s of particles, I could set a surface injector which releases 0.3 Kg/s of mass flow without the surface scaling and another surface injector with the surface scaling which injects the remaining particle mass flow. I don't know if this makes any sense, but it would help to keep the parcels mass more uniform.
You have really saved my thesis, again thank you!

[Rob]

You're welcome. Now it's established what the problem is, you need to decide what to do about it. Setting the scale by area means you're now tracking variable mass parcels so there's more DPM mass in the "outer" parcels than those on the centre line. This may or may not be something to think about.
As an aside, staff are not permitted to open attachments so please repost the images.

[Lorenzo_P]

This is the DPM concentration in the global range.
this is the dpm concentration with the maximum fixed at 3 Kg/m^3.
This is the Mach number.
So, in the end, if I have understood well, the problem is related to the different volume of the cells: it is smaller for the cells near the axis with respect to the cells in the outer region. This is beacuse in axisymmetric problem the geometry is represented as a "clove" of some degrees of the whole 3D body. As a consequence, it fails to manage the DPM concentration near the axis, causing the errors we saw. Is this a good explanation?