Okay I'm working on a project in order to prove to a client the feasibility of us using CFD to accurately predict how our designs are going to operate. I'm running a model right now in which there is a plate with static vanes. It looks like a fan if you're looking down on it but the vanes themselves don't actually move. The air passes through them and circulates.

Working on several different equation sets I've found that the RSM unsteady model provides for the most accurate velocity and pressure drop results. 2nd order is even better but I can't get it to converge (thats another problem to deal with later).

Unfortionately I can't get the particle tracking to make any sense whatsoever. When I use the rosin-rammler distribution for the injection I get maybe 30% efficiency (70% of the particles escape the apparatus through the outlet at the top) which is completely wrong for this design. Maybe there would be some variation, but 30% efficiency is way off.

If I use a uniform particle distribution, it goes from about 0% efficiency to 100% efficiency changing the particle diameter size from 70 to 90 microns, which is also wrong because there should not be that great of a chance with such a small change in particle diameter.

I did not have the descrete phase enabled during iterations, because if I do the simulation undoubtably crashes or the results get so skewed and make no sense whatsoever.

Does anybody have any advice of what I can do? A major part of this project is being able to give accurate particle efficiencies but I've been banging my head against the walls for days trying to get this to work.

Thank you.

Just to add, why can't I run this with discrete phase enabled? Whenever I have it enabled, 75000 steps, update every 50 iterations, shared memory parallel mode, the continuity just keeps going up after every dpm iteration. I like to plot the residuals while I run simulations, and the continuity just looks like an endless staircase going up and up and up.

Are you within the DPM limits (less than 10% particle loading by volume)? Maybe your DPM URF is too high? I suppose that your particles are inert.

Regards, Remus

Yes they are inert particles. Changing the DPM URF doesn't help the continuity. Changing the momentum and pressure URfs don't really help. I mean I can certainly turn them all the way down until the residuals are within range but then the data is garbage.

I'm guessing you have already checked the usual things - mass flow of particles, particle density and other properties, etc.

On your first question of getting particle collection efficiencies, for similar projects we have taken a more manual approach. We would break the known particle size distribution down into mass fractions by diameter class. Say 5 microns reprents 30% of the mass, 10 microns is 50%, and 20 microns is 20% (of course using more diameter classes gives better resolution), we'd look at the collection efficiency of each of the diameter classes by running a DPM calculation for each diameter. Then, based on the collection efficiency for each diameter class, and the mass fraction represented by that diameter class, an overall collection efficiency can be calculated.

The R-R distribution, and the way in which Fluent handles it, is not necessarily representative.

What do you do since your fluid phase calculation is time dependant and DPM can be set for steady conditions or released at fixed intervals?

Thats a good way of doing it, but unfortionately I've tried it and still run into problems. Our normal particle size distribution is from 12 - 120 microns. On this model (using uniform distribution), anything less than 70 microns escapes the unit completely, and everything over 90 is trapped. This unit should certainly be able to trap particles smaller than 70 microns, but not a single one in fluent.

And yeah I've checked the particle density and injection properties about 100 times.

I've tried everything, from having the dpm running in steady conditions, unsteady conditions, updating dpm iteration every 10 iterations, every 50, 100 etc.,. Nothing useable

In your post you said you are using unsteady RSM. What turbulence parameters are you using for DPM? If you are using stochastic tracking then you need to change the time scale constant from 0.15 to 0.3 for RSM turbulence model. This information can be found in the help files somewhere! I would suggest reducing complexity and trying a two-equation turbulence model and calculating separation efficiency with DPM to see if you get more realistic answers.

I don't agree with the last post about the R-R not being representitive. I regularly use it to calculte cyclone efficiencies. However, you must be careful calculating efficiency as you need to associate the correct mass flow with the discrete particle size.

As for your convergence problems, I have found the same problems when the mass loading of solids to gas is high. Try setting the DPM URF to 0.01 or unsteady particle tracks.

I wrote that the way Fluent handles the R-R distribution is not necessarily representative because of a more subtle effect. If for example you choose 10 particles with a diameter range of 0 to 110 microns, Fluent will give you particle diameters of 10, 20, 30, etc. Then, based on the R-R parameters, it will assign mass fractions to each of the diameter classes. The drawback to this approach is that the first 3 diameter classes may represent only 10% of the mass fraction but 30% of the number of particles. And, the 50 micron class could represent 20% of the mass but only 10% of the particles. So, if there is a sharp breakpoint in how the particle diameter influences its ultimate fate, the results could be skewed by this way of handling it.

A better approach is to divide the particle mass into 10 equal fractions, and then based on the diameter distribution, find out what the diameter classes should be.

The R-R distribution may give a good fit for the particle size distribution data, but a lognormal or other distrution could be better depending on the process. But, this is isn't really a CFD question.

And, if the flow field can't be properly solved, then the particle distibution is irrelevant.

I think I understand what you are getting at now but I still don't agree. The number of particles tracked for each size range is irrelevant to an efficiency calculation. You only need to ensure that you track enough particles so you achieve average conditions. Also, the mass flow rate associated with a particular size is not included in the particle drag force calculation and does not influence particle trajectories. This is not true for two-way coupling as it is used for the momentum exchange force.

For example, consider a cyclone efficiency calculation. Using 0-110 microns with 10 diameters and 10 injection points, that gives a total of 100 trajectories. For each particle size, the efficency is simply number of particles lost divided by number particles injected. The total efficency can be calculated usign the mass flow rate assigned to each size range. The effect of diameter is clearly shown using this method as you track the same number of particles for each size.

For RSM, actually yes I've already changed the time scale constant to .3.

The simulation I iterated with the DPM enabled was KE-Steady state.

If I reduce the DPM URF to .01 is that going to be accurate?

I gave the URF at .01 a try, didn't really help. Not only are the residuals not converging but the results aren't even in the righ order of magnitude that they should be. Initial gas flow velocity is 1 ft/s but I'm getting velocities of 1800 ft/s so yeah thats somewhat off.....

Try reducing the mass flow rate of the particles to a small value, set URF to 1, and see if the problem persists.

Changing the DPM URF to 0.1 won't change the result it just means it takes a long time to get a converged solution.

[arjun3020]

Hi all,
thanks for this help, in this post allan walsh said that use single diameter, 5 microns reprents 30% of the mass, 10 microns is 50%, and 20 microns is 20%.
But what about mass flow rate of that particals say 5 micron size which represents 30% of mass. if total mass flow rate of particles is 0.01 kg/sec. then while running for 5 micron what mass flow rate have to be entered, (0.03 X 0.01)=0.0003 i.e. 30% of total, or 0.01 kg/sec. second question is which type of injections.? single injections or surface injections with uniform diameter distribution?
Please help.

[Amna Amanat]

hi
in DDPM tracking at fluent ,after calculating results how we'll come to know the position of certain ID particle at any time???

plz reply fast....
thank u

[Amna Amanat]

hi

During unsteady particle tracking at fluent using DDPM model.how a result file is generated? A file which shows the location of each ID particle at any time.

If someone has any idea of it plz let me know ...

[n9879005]

Hi Amna,

Now i am facing this problem.can you please help me? i think you have the solution now.

thanks in advance

[amrendra rai]

i analysed cyclone model using ansys. after analysing i proceeded to post cfd and i imported particle history trackfile. but i was unable to get full particle trajectory. it was showing like particles entering from inlet and then after travelling from inlet it got disappeared. i was not able to track any particle trajectory. please help me with some suggestions so that i can get particle trajectory. fast reply is encouraged. because i hve to go for fabrication..... please help me ?????