CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   questions with Discrete Phase (http://www.cfd-online.com/Forums/fluent/29973-questions-discrete-phase.html)

 cwflying July 3, 2002 02:26

questions with Discrete Phase

During my calculation with discrete phase modeling, I have met some problems:

The default max number of steps is 500,according to fluent's help documents,"default value of 500 time steps is insufficient for completion of the trajectory calculation" and then fluent gives a simple way to decide the max number of steps and length scale(supposed you choose "specify length scale"), that is: "if you want the particles to advance through a domain of length D, the Length Scale times the Max. Number Of Steps should be approximately equal to D." Even though I think Fluent does not give it a clear explanation of how to decide the max number of steps,500 is to small comparing with (10,9)!

If I use "group" injection and when I enter the required parameters such as the positions of first and last point(which are inside the domain of my model). But if you choose to list the injiction it says "unable to locate injection-0" and the number tracked is 0". There is no problem when I used surface injection. But I have found the distance but I find the distance betweent the starting point and the wall is smaller than I have set before( which I adopt'group'). I'd like to know: How does FLUENT decide the number of stream lines and how to decide the distance between each particle.

 Lanre July 4, 2002 00:18

Re: questions with Discrete Phase

Q1. If you specify N steps and following you trajectory calculation you have, in the report, a message saying "# incomplete" where, # > 0. Then you likely have not specified enough steps.

Q2. Part 1. When you set a group injection, make sure that the start and end of the line exist entirely within your computational domain. Watch out for round-off, i.e., your model zero may actually be 1e-12, so starting your group line at 0 will put the first injection outside the domain.

Q2. Part 2. If you specify the number of particles in the group to be 10, and the distance between the start and end points of your group line is 1 m. Then 10 equidistant injections are made, i.e., distance/(N-1).

 cwflying July 4, 2002 02:19

Re: questions with Discrete Phase

(1)but I have not put the starting point at 0 position,it still reports error!

(2)if I choose surface, how does FLUENT itself calculate the number of particles? In my question, I got 14 (N0.0 through No.13, where does 14 come?

Thanks a lot!

 Lanre July 4, 2002 11:31

Re: questions with Discrete Phase

Q2. A DPM particle is released from every facet on the surface.

To determine the number of facets on a surface, and thus the number of injections, go to Surface-->Manage...

Counting from 0 to 13 gives you 14.

 david July 17, 2002 20:42

Re: questions with Discrete Phase

Lanre >>Q1. If you specify N steps and following you trajectory calculation you have, in the report, a message saying "# incomplete" where, # > 0. Then you likely have not specified enough steps.

DC >> Don't you think its other way around ??

 Lanre July 18, 2002 07:07

Re: questions with Discrete Phase

The DPM model solves a force balance on the particle, i.e., mass*acceleration = drag + etc. Acceleration is essentially du/dt. You don't explicitly specify the time in the integration of the force balance but rather you set the distance (recall from physics that distance = velocity x time). Loosely, you use the step length to set the distance for integration of the particle trajectory. This leaves another parameter that needs to be set...the number of discrete distance steps for integration. This is where you specify the number of steps. The number of steps just has to be large enough for the slowest moving particle to exit the domain. It does not mean that every particle will explicitly use the number of steps you specify since, in most applications, some will leave earlier and others will leave later.

 All times are GMT -4. The time now is 11:24.