Learning Forum

[Zwernjayden]

Despite 3000k temps, my DPM particles are colliding, but barely evaporating causing a huge build up and causing the iterations to stall. Can they not evaporate after breakup? I also have an issue with the minimum temp being lower than the injected temp which in this case is obviously not possible. I have attached my full setup, and screenshots.

General

• Pressure based, steady state, 3d

Models

• Energy equation on
• k-e realizable turbulence model
• Species transport, 66 step, 31 species chemkin file for ethanol reaction and thermo properties (it is using units CAL/MOL. Do I need manual unit conversion?) 
  • eddy dissipation, relax to chemical equilibrium
• DPM settings
  • Interact with continous phase on
  • unsteady particle tracking on
  • update dpm sources every flow iteration on, iterations set to 1
  • Max number of tracking steps set to 50,000
  • particle time step set to 1e-6
  • stochastic collision, breakup, volume displacement, two-way turbulence coupling on
• DPM injections, some of which are angled to impinge (start time 0, stop time 999999999). All positioned -.0001 below surface in order to make sure all particles end up in domain 
  • 25 multicomponent plain oriface atomizers with 10 steams 
    • 75% c2h5oh
    • 25% h2o
    • Temp=400k
    • location, diameter, length, mass flow rate taken from real injector
    • vapor pressure 50 psi
    • A=4.9, radius of curvature=1e-5, 0-360 angle (all left unchanged)
  • 16 droplet plain oriface atomizer with 10 streams
    • 100% Lox
    • Temp=90k
    • location, diameter, length, mass flow rate taken from real injector
    • vapor pressure is 14psi
    • A=4.9, radius of curvature=1e-5, 0-360 angle (all left unchanged)
• Chemkin mechanism mixture set to ideal gas in order to model compressible flow
• Boundary conditions
  • No inlets (all material injected using DPM)
  • Pressure outlet set to no backflow, DPM escape
  • Wall set to trap to help particles evaporate
• Initialized at 300 psi expected operating pressure
• Patched chamber to 2500k for ignition

 

As I mentioned, the particles seem to build instead of evaporating. In this photo you can see there is 74 million particles, despite having a simple geometry with only 570 total streams

 

 

[Rob]

With a very small particle time step you're adding droplets at a very high frequency, which may explain the high count. Depending on the injection angle you're also potentially adding them into the flow boundary layer - do they have sufficient momentum to penetrate the flow domain? Why 50,000 integration steps? Shed implies you're also running a wall film model? 

[Zwernjayden]

I used a high frequency because at a lower time step it said that many of them were lost outside the domain. I am using a high tracking step number because I was under the impressure that it just meant fluent would track the particles for longer. The injections near the edge are straight down to simulate the effects of film cooling. Shed is due to having the breakup model on. There is no wall film model. None of this really explains why the particles wouldn't be evaporating though...

[Rob]

If you have or want film cooling model that, LWF should be sufficient. With that many steps it'll take ages to do an update, and you risk solver issues with anything that gets stuck. 

Thinking about the physics. With that many collisions the volume fraction must be fairly high near the injections. What does that do to the local flowfield? Have the particles actually moved far enough (and for long enough) to actually evaporate? Ie how old are the particles in your domain? 

No idea about the units. Fluent uses SI in the solver numerics so it'll depend on what you set the Units as for any imports: I'd generally recommend SI for everything to avoid confusion later on. 

[Zwernjayden]

 

 

 

 

I’m unsure what you mean by volume fraction. Do you mean how much of the cell is DPM? I think my case is a bit weird because my continuous phase is just made up of 100% evaporated particles.

I was able to lower the tracking from 50,000 to 1,500 and decrease the time step size to 3e-4, which seems to stop particles from building up, but now k and epsilon residuals keep spiking and falling back down again after all other residuals have leveled off. Should I try a different turbulence model?

In terms of LWF, should I turn that on in addition to the rest of my model? It’s unclear what you mean by LWF should be sufficient, as the placement of the injectors matches up with a physical machined injector, and it seems adding LWF will just complicate the model further. Also I’m not sure if LWF makes sense because at those temps won’t the injected fuel vaporize into a gas?

 

 

 

 

[Rob]

Initially you have a high volume fraction of droplets near the injectors. These will hopefully evaporate very quickly. But, if you add droplets in at very close proximity that are travelling in about the same direction & speed with collision on they're going to agglomerate. Then the next droplet hits etc. Very quickly the region around the injector is droplet and you may or may not evaporate faster than liquid is added. 

Hence increasing the injection interval. 

Normal droplets on a wall will become trapped by the viscous sublayer. Wall films are designed to work with the wall shear and move. 

 

Most multiphase models are fairly easy to set up. The really hard part is understanding the likely flow field and physics to decide what to set up. 

[Zwernjayden]

Ok thank you Rob. Should I just be changing the particle time step size then, or turning off "update dpm sources every flow iteration" and increasing "dpm iteration interval"

[Rob]

Particle time step is likely the best option. Updating the sources that frequently tends to assist solver stability, and the integration interval shouldn't make too much difference in a transient model. 

[Zwernjayden]

It isn't a transient analysis right now, it's steady state. Should it be transient instead?

[Rob]

Possibly, or do you need to initialise a sensible gas mixture to get it lit? 

[Zwernjayden]

Since I am using the eddy dissipation model it initializes with some species present without me having to do it manually