CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   DPM Iteration, incomplete (http://www.cfd-online.com/Forums/fluent/31617-dpm-iteration-incomplete.html)

 rookie June 9, 2003 14:08

DPM Iteration, incomplete

Hello Folks,

Do you know what "incomplete" means in the following message? Thanks a lot.

DPM Iteration .... number tracked = 2100, escaped = 0, aborted = 0, trapped = 32, evaporated = 0, incomplete = 2068

Rookie

 xiangrb June 9, 2003 20:36

Re: DPM Iteration, incomplete

Incomplete means that your trajectory caculations are not completed. In this case, you should increase the max.number of steps in the Discrete Phase Model Panel if you are sure that the particle is not recirculating somewhere in your domain. Good Luck!

 Alex Munoz June 10, 2003 12:49

Re: DPM Iteration, incomplete

Hi

Xian gave you in my opinion unacurate answers.

Imcoplete trajectory means that a particle or particles were traped by the flow. Therefore the number of time steps that you specify were not enough to allow the particle(s) to reach the outlet.

As a result, you can increase the number of time step to allow Fluent follow those particle in a longer path that the actual one. However, This approach is not going to solve the problem because always some particles will remain trapped.

Therefore, You have to determine a statistical criteria such as 95 or 98% of the particles should leave the domain to consider a satisfactory simmulation of the discrete phase.

Best regards

Alex Munoz

 xiang June 10, 2003 20:35

Re: DPM Iteration, incomplete

Hello, I think "trapped" and "incomplete" are different. If you set particle boudary type for the walls as "trapped", the particle will be trapped whenever this particle collide with the wall and the trajectory calculation for this particle will be terminated. Therefore, those particles which touch the wall will not reach the outlet. However, the trajectory calculation for these particles are completed.

"incomplete" means the particle doesn't collide with any boundary, the trajectory calculation terminates somewhere inside the domain upon reaching the max. number of time steps. If you increase the number of steps, the particle will move further.

In my opion,if no particle touches the other boundary type and no particle is recirculating in the domain, all particles should reach the outlet and leave the domain with sufficient number of time steps.

Thanks.

 Alex Munoz June 10, 2003 23:53

Re: DPM Iteration, incomplete

Hi rockie

Perhaps I wasn't clear enough. When I wrote particles trapped by the flow means particles that get inside a vortex or eddy for a time period longer that you allow to the particles to exit the domain. In any instance I wrote particles traped by the boundaries of the domain, However, it seems that some people understand the word "trap" in the terms that fluent use it.

BTW, Some people like me expect that you reply a thank you note as a simbol of message read, and also as form of curtesy. I am aware of that some culture are not use to reply a thank you note, but keep in mind that I and other CFD user take a few minute of their time to read your question. Therefore, they deserve a note of acknolegde

Best regards

Alex Munoz

 rookie June 12, 2003 20:31

Re: DPM Iteration, incomplete

Hello Alex, Xiang and All,

Thank you very much for your kindness replies. If the particle can not reach the outlet (incomplete), does the particle keep moving in the next trajectory periods?

Thanks again, Alex and Xiang.

Rookie.

 winnie June 12, 2003 21:44

Re: DPM Iteration, incomplete

Hi, rookie

During each dpm iteration, the particles' trajectories are calculated based on the current continuous field from their injections to either trapped by the boundary or complete at the outlet or incomplete in the field, so whether they complete or incomplete during the last iteration, they will be calculated from injection to get their another path again.

But why don't you give a larger Max. Number of Steps to complete the trajectory. In my opinion, if the particles don't reach the outlet, the exchange(mass, momentum...) between discrete phase and continuous phase are not completely calculated which effect the correctness of the ultimate result.

Regards

winnie

 iman_be April 18, 2016 00:24

Hello all,
I have the same problem. I try to model the microfluid in turbulent forced convection. when I increase the maximum time steps my simulation faces the divergence problem. but at the low time step, my simulation is converged without reaching the particles to the pipe outlet.

Quote:
 Originally Posted by winnie ;106494 Hi, rookie During each dpm iteration, the particles' trajectories are calculated based on the current continuous field from their injections to either trapped by the boundary or complete at the outlet or incomplete in the field, so whether they complete or incomplete during the last iteration, they will be calculated from injection to get their another path again. But why don't you give a larger Max. Number of Steps to complete the trajectory. In my opinion, if the particles don't reach the outlet, the exchange(mass, momentum...) between discrete phase and continuous phase are not completely calculated which effect the correctness of the ultimate result. Regards winnie

 Nuha April 18, 2016 17:25

fluidization proper pattern issues

Hi

i m simulating a 3 phase fluidized bed using DDPM with DEM collisions.
particles of 38 mm are introduced through surface injection on a mesh of 40mm . As a simulation result i want a fluidized bed but i got totally dispersed bed in which particles moves too far from each other and ultimately reached to outlet which is highly undesirable .

what is its reason?? if anyone knows it then please let me know .

 kantay May 18, 2016 12:08

fluidized bed

Hi everybody,
if you don't mind i will ask you ,
in my final projecti should I have to determine the point of optimal fluidization operation (the necessary air speed and particles), I work on a biomass boiler, I draw the geometry and I did the mesh (there is not chemical reactions or combustion in the beginning, there is just fluidization), but regarding the models I found difficulties ,there are several choices and more bars, I am dispersed ,if you can help me I will be appreciated souria, guide me please.
thanks for any help :)

 All times are GMT -4. The time now is 04:32.