[yaldizli]

Hi All,

This is the first time that I am using DPM model and my problem is this:
I am simulating a steady state air flow problem where inert coal particles are injected at the inlet. When I use realizable k-epsilon model with turbulent intensity and viscosity ratio b.cs, the particles except the ones next to the pipe wall stay within the first cell. The fist thing that I came up with was to increase the number of time steps that I am using. I was using 20000 steps and increased it but it did not help. Has anybody seen this kind of problem with using realizable k-epsilon and any suggestions?

Thanks,

Myaldizli

[Ilu]

Have you checked that you have some reasonable velocity in the inlet? I once had that problem cause I loaded a wrong data file and there was no velocity in the flow field and of course the particles didn´t move at all Soryy I can´t come up with any other solution. good luck!

[yaldizli]

Hi,

Thanks for your reply. Actually I started to inject the particles after solving the clean air flow first. The results for the clear simulations is just fine. When I turn on the DPM, i got this problem. Interestingly, if I use RNG instead of rke
the particles travel. However, in this case my results are not that much accurate. So I want to stick to rke.

Any other suggestions ?


Thanks,

Myaldizli

[xrs333]

Have you got massage which reads 'DPM iteration, ...incomplete=###.....' in the console?

[yaldizli]

Thanks,

Yes I have. Actually, most of the particles are incomplete. The ones either escape or trapped are those next to the pipe walls. The only explanation that I got is the the time scale for the one at the center are too small compared to the ones next to the pipe wall which is basically calculated from the wall function not from the ratio of k and e.

Thanks,

[xrs333]

Particle trajectory calculation is not related directly with turbulent model.
try to increase Max. Number of Steps under tracking parameters in Discrete Phase panel, this number should be increased to ensure most partiles complete their travel in the domain.
i hope this can be effectual.

[yaldizli]

Hi xrs333,

Thank you for your response, But I have already tried to increase the Max. Num. Steps. The weird thing is the particles in the cells adjacent to the wall are traveling all the way from inlet to outlet. If the issue was Max. Num. Steps they would stay within the first cell either but they do not. The time step that the particle trajectories are calculated is computed from 0.15*k/e for k-epsilon models, which I refer to in my previous post. In the cells adjacent to the wall however it is calculated from the wall functions.

myaldizli

[Mohsin]

Hi yaldizli

Dont increase number of steps too much. solve with 2nd order discretization scheme you wont get incomplete particles.

Also check your injection types. Generally "Group injection" creates problems like this.

Good luck

[xrs333]

I cannot think up an idea right now. But if you give out more info about the model, for example, is moving reference frame used, what type injection is used, etc., I may have new idea.
further, is the factor 0.15 in the formulation 0.15*k/e the Time Scale Constant under Stochastic Tracking in the Set Injetion Properties panel? But this option is for turbulent dispersion, not for average trojectory of the particle.

[yaldizli]

Hi All,

Thanks for your responses again. I have tried to apply DPM in a different problem set up using rke and again I am getting the same kind of particles staying within the first cell at the interior zone of my inlet. I think on my machine either this way is not working or i am really missing a keystone somewhere using this DPM.

Let me more informative. I am running a coal classifier problem. My flow is turbulent and steady state. After running clean air case for 18k iteration i start to inject coal particles at my inlet using surface injection. My particles are injected uniformly and they are inert. No Energy equation. I am using 10% Intensity and 5 for the turbulent viscosity ratio. The Max. Num of Steps is 20000 and the length scale is turned on with a value of 0.5 inches. Number of continuous phase per particle calculation is 10. Also, the discrete random walk model is on with 1 tries and 0.15 time scale constant.

Thanks,

myaldizli

[xrs333]

I reproduced your trouble. I think it's because of the turbulent dispersion model used, the discrete random walk model.
And I think the turbulent intensity of 10% too high for usual instance.

[yaldizli]

Hi All,

Thanks again for your time. I figured out recently that it is 100% bcs issue. The intensity seems to be ok but the dissipation is calculated too high which gives very small time step for particle calculations according to the 0.15*k/e formula. When I just set the viscosity ratio to an enormous value of 1000. The particle in the center moves up. So, this explains why hydraulic diameter bc is also working. The dissipation rate is calculated smaller with when hydraulic diameter is used along with intensity.