Hello all.

I wonder if someone can help me? I am having problems with simulating a swirl burner that uses liquid fuel. I can simulate the flow just fine and I am able to get a recirculation zone in front of the burner as expected. The problem starts when I inject fuel droplets in the recirculation zone. My residuals go crazy, and no matter how big interval between the DPM iterations it doesn't normalize. I seem to be getting very large gas phase velocities in the same region.

I have tried smaller fuel droplets velocities, smaller under-relaxation factors for Discrete phase, but nothing works.

Has anyone had experience with that kind of problem?

Thanks in advance,

Vix

Try a small urf for density, density 0.5 and dpm 0.2 usually works fine. Do you have your own reaction kinectis?

RoM

Urf is under-relaxation factor right? OK, I'll try. I am not using reaction kinetics but equilibrium chemistry (PDF look-up tables)

Are you working on a similar problem?

ViX

If you use your own kinetics it could lead to numerical problems due to stiff chemistry but with equlibrium pdf this should not happen. I did some coal combustion recently and it worked well with underrelaxation 0.5 for density and 0.2 for dpm.

Good Luck, RoM

I seem to be getting a divergence even if I exclude reactions, just the interaction of discrete phase and continous phase is a problem.

Thanks for your advice!

Did you try a smaller particle mass flux? You may want to increase that in steps.

I am getting better results with a much lower mass flux, thanks, but still no convergence.

Could this also be a problem of the Lenght scale in the DPM panel? How does this affect residuals.

Vix

Sometimes fluent will calculate very large dpm concentrations, usually in the area of the dpm injections. You can use the adpat->iso value panel to calculate the max dpm concentration in your domain. If its close to your liquid fuel density (or even larger) you will get a problem with convergeance.

RoM

And how do I resolve this problem with a very high concentration?

There is no general solution to this problem. Your injection should enclose a large number of cells so the total mass flow is spilt. Dont use single injections or small group/cone injections for high mass flow rates. Use surface injections with fine surfaces meshes instead.

RoM

Thank you for your very helpful remarks and advice.

I' ll try to remesh my model and redistribute the DPM source and increase the number of particles in a group.

ViX

What also helped for me was to do 1 DPM iteration per continuous phase iteration (otherwise residuals oscilalte), and to create a decent initial velocity field by creating a gas velocity inlet with the spray droplet velocity at the same spot.