Gas Cyclone convergence problem
 

Hi everybody

This is my 1st post in this forum and hope for your co-operation.

I'm working on reverse flow gas cyclone with DPM. I'm working with RSM: Non-equilibrium wall function. I've 1,65,525 hex cells (testing phase). I'm using SIMPLEC scheme for pressure-velocity coupling, Least Square Cell Based for Gradient, PRESTO for pressure, 2nd order Upwind for Turbulent ke and for Dissipation rate, and 1st order for Transient formulation. I've inlet velocity 10 m/s and DPM too has the same inlet velocity. My inlet is velocity inlet, outlet (top) is outflow, and rest other walls. All residuals are set to 1e-05.

Now I'm facing two problems.

1. The solution in non-converging (I ran it for 3.1 sec. too!), whereas some of them claim to get convergence at 1.6 sec.
2. The time average tangential velocity (max. value around 11 m/s) is not matching with the experimental one (max. value around 18m/s). However, the time average axial-velocity is somewhat near to the experimental values.

Without DPM I'm getting nearly the same results of Tangential velocity (i.e., max. tangential velocity around 11 m/s), but with convergence. Am I doing wrong somewhere? Please suggest me to get results with convergence.

Regards

did you try to increase the number of iterations per time step? and also decrease the time step size?

Thank you sicfred for your reply. I've increased and decreased the time step, but the results are the same as before. Well, throughout I've taken max. Iterations/time step as the default value,i.e., 20. I'll check it by substituting its value to be 50. Will it have any impact on the results :confused: ??? Thanks again.

1) Do you consecutively inject particles at your inlet?
2) Do you have "Interaction with Continuous Phase" switched on?

Thanx RodriguezFatz 4 ur reply.
Yes I've checked "Interaction with Continuous Phase", and I've been injecting around 750 particles normal to the surface (from inlet) per second :( !

Ok, then try "Update DPM Sources Every Flow Iteration", thats the checkbox below. You can also set "Number of Continuous Phase Iterations per DPM Iteration" to 1. And, also in the "Discrete Phase Model Dialog box" under "Numerics" set the numeric scheme to "implicit". Particle algorithms can become ugly, when you violate CFL criterion, so with implicit you are on the safe side!

Thanx RodriguezFatz. I am already using "Update DPM Sources Every Flow Iteration" with its default value (i.e. 20). For tracking parameters I'm using 9e+05 as max. no. of steps. Under numerics, I've been using implicit for high order schemes (which is by default in fluent). Under particle treatment box, I've checked "Unsteady particle tracking" and also "Track with fluid flow time step". This means particle time step size is 0.001 (Fluent's default). Thanx.

Try "1".


Are you sure? In my case "trapezoidal" was set as default.


The rest sounds fine.
Did you calculate your particle mass flow correctly?

Hi RodriguezFatz. My mass flow rate for particles is 0.001 Kg/s. I'll try "Number of Continuous Phase Iterations per DPM Iteration" equal to 1.
Yes, for numerics, my default is : "High order scheme : trapezoidal", and "Lower order scheme : implicit". O.K.!! I'm saying this when "Automated" option is checked under "Tracking Scheme Selection"!!! Do I have to uncheck it? If so, I'm getting various options under Tracking scheme like: implicit, analytic, trapezoidal, or Runge-kutta (default is trapezoidal). So shall I proceed by unchecking "Automated" box and with implicit as tracking scheme? Is this the option (by unchecking) you were talking about? Do I need to uncheck "Accuracy Control" under "Numerics" tab too? In my case it is checked ! Thanx.

1) What's the density of your particle material? How large is the inlet area?
2) Try to uncheck "Automated". Then choose just "implicit". You have to get rid of your numerical problems first, then you can enhance accuracy. On that score, "implicit" is the best choice, since it is unconditionally stable.

Hi RodriguezFatz. Particle density is 860 Kg/m^3, and Inlet area is (0.145 x 0.058) m^2. After passing through inlet, air along with DPM experiences swirl motion to separate out the discrete phase out of the continuous phase (i.e. air) due to centrifugal action. Thanx

If my quick calculation was correctly, your input should be fine. I have a volume fraction of 1.38e-5 for your case, which is by far low enough!
Try a run with the new settings, it should work now... ;)
I will keep my fingers crossed.

Thank you RodriguezFatz, I'll try with the new settings tonight and let you know the results.

One other thing: Reduce the order of your continuous phase numerics towards more dissipative schemes ("as much 1st order upwind as possible"). That did the trick for me right now!

Hi RodriguezFatz, nice to hear you again. I think you mean that I shall reduce the spatial discretization parameters to 1st order upwind, right! As soon as I finish the previous problem (which is still in progress), I'll try that too. I hope it converges on 2nd order upwind scheme as per our discussion. Many thanx for ur support.

Hi RodriguezFatz, I couldn't achieve convergence with 2nd order upwind with DPM (image attached).
With single phase, i somehow got convergence (image attached).

To reduce simulation time, I'm working with 60,000 hex cells.

In a thesis I've read that with DPM, convergence was achieved within 1.6 to 1.7 seconds, and for me, even on single phase it took nearly 2.9 seconds to converge. Do I have to rework on single phase first to achieve convergence within 2 seconds :confused: ? I'm also not getting desired tangential velocity (1.7 to 2.5 times inlet velocity) of 18 m/s (mine is 11m/s). I still can't figure out where exactly is the problem. :( !!!!!!!!!!!!

During each timestep, do the residuals stop getting better after some iteration and remain at, let's say 1.0e-2 ?
How large is you maximum number of iterations per timestep?

Hi RodriguezFatz
After few time steps, the continuity line in the residuals is mainly fluctuating. In the beginning, all the lines slopes down in a group and after, say, nearly 2000 iterations, continuity line starts separating out and its fluctuation is more (its like, rushing up to 1e-01 residual in a very unusual manner) than any other parameter with the increasing number of time steps. Continuity line slopes up drastically at few time steps, while other parameters are comparatively fluctuating at very slow rate. At few time steps there is sudden jump in all parameters ( with sudden fall down too !), as can be seen in the figure.

Well, my Max Iterations/Time Step is 40. Since I'm working on a very coarse mesh (around 65K hex cells), I've taken time step as 0.03

That sounds exactly like my problem. Try 1st order upwind.

I'm having the same problem too.