How can i get my particles to stick?
 

I have a pipe with a spiral in it, and i am simulating how different particles will move toward the wall of the pipe with respect to their size. This has been successful, but if i want to keep the particles stuck to the walls of the pipe once the hit it, how can i do this? I would like to look at a pipe with different sizes of particles stuck in different places.

Any help on this would be great!

It's funny I'm facing the same issue.

In order for the particles to "stick" I though it would be sufficient to change the wall boundary conditions --> DPM --> play around with the values for the normal and tangential momentum conservation. As I barely saw anything, then I switched the walls to "trap", but even though many particles are reported to be trapped, I don't see any particle track coming to an end in a wall...

Let me know if you make any progress

Hey,

Just wondering if you are using a transient simulation, as a build up of particles wouldn't be steady state? I haven't done this myself to be honest but will be trying something similar soon so I'd be interested to know how you get on.

Cheers,

Neil

Hi,
you have to use the wall-film model (in the boundary conditions) but you have to know that it is ONLY VALID for LIQUID materials. So you have to define the material type of your particles as e.g water-liquid, and then change the name or property of it.
Hope this helps.

regards,
spring

Hi spring!

So it is possible to use the wall film method, and "trick" the program into thinking that the particles are water? I tried changing the restitution constant to 0 and its.....not as successful as id like.

Hi zmaxcomputer,

I didn't exactley understnand what you mean, but I can tell you what I did to make my particles stick on the walls.

1. when I injected the particles, I chaneged their material to water-liquid:
define/models/dpm/injections/create-injection
injection_1_01
yes
inert
yes
file
yes
water-liquid
"1mu.inj"
no
no
no
no
;

2. after I injected all my particles I changed the name and density of the material to the values I needed:
;
define/materials/change-create
water-liquid
aerosol
; change density
yes
;1005.25
1025
no
no
yes
;

3. then I changed the boundary conditions for the walls to make the particles be trapped on them:
;
; make all particles be trapped when touching walls
;
define/boundary-conditions/wall/wall_pb_main
no
no
yes
trap
define/boundary-conditions/wall/wall_cz_main
no
no
yes
trap
;........ and so on ......... do this for all your walls

And that's waht I did. I got the notice to use water-liquid as the material for the particles if I want them to stick on the walls from fluent user's guide. It's written there explicitely, that if you want the particles to be trapped on the walls they have to be liquid.

I hope my TUI commands can help you.

regards,
spring

Hi Sarah,

Did you manage to find out what number of your particles stuck and where? It'd be interesting to be able to plot a contour plot of the number of trapped particles on different surfaces. Have you done that by any chance?
Best regards,

Hi kingjewel1,

yes it is possible to find out where the particles stuck and how many --->> SUMMARY REPORT. Therefore you have to tell fluent to make a summary report before starting to simulate the discrete phase model. This report type contains the zones with the ID number (=for every wall a number) and the amount of particles stuck on this zone. In Fluent's user's guide chapter 23.7.2 (fluent version 12.0) it is explained how you can request this report type.

To SEE where my particles stuck I did the following:

1. Before I started the discrete phase model simulation I requested another type of report: REPORT->SAMPLE (of trajectories). This type of report gives you the particle states like position, velocity, diameter, mass flow .... when the particles cross or touch a boundary. It can be used as an injection file, too. AND THAT'S THE CLUE.

2. Request a report sample for ALL your walls and after the dpm simulation is finished use this sample files (with the ending ".dpm") as your new injection files in a new dpm simulation, with the purpose to visaulize the particles in your geometry.

3. Choose only one integration step to prevent the particles from beeing tracked again across the hole geometry.

4. After you've done this settings (.dpm injection, integration step, ...) go to: graphic and animations -> partickle tracks -> and choose particle density as the parameter you want to see, and choose "point" not the default shape "line" to see your particles as points.

5. In the mesh option, choose to see just the features of your walls.

6. Finally mark all your walls (which are in the injections window in the particle tracks window) and click display.

With this way I got really very good pictures of my stuck particles in my geometry. Maybe there is another (less complicated) way, but I don't know it.

I wrote much, hehe. But I hope I could explain everything clearly to you. If not just ask!

regards,
spring

Hi Spring,

That is a great detailed explanation... one which FLUENT should publish!:)


After going through carefully I found that FLUENT produced an error while reading the injection files: ERROR unable to open injection file. During iteration stage. However the .dpm files are in the correct format. Any ideas why?

(zone-25 12)
( X Y Z U V W diameter T parcel-mass mass n-in-parcel time name)

It seems that I can manually open the .dpm files and count the particles deposited per zone.... but I have 25 (!)

A method I found useful for visualising contour plots of particle deposition was to use the Erosion/Accretion method, though I'm not sure how apt this is here. My particles are fine water droplets in reality from a person's sneeze.:p What do you do?

@ kingjewel1,


hmmmm...I only had this problem (UNABLE TO OPEN FILE) when I forgot to place the injection files in my working folder (whose path has to be set when starting fluent) because fluent automatically searches for all files in the working folder. If you've already done this, another thing that sometimes has to be done, when I want to inject the ".dpm" files, is that I have to make a test-injection first. That means that I make any injection (file, or surface) and let it run. After that I inject my "walls.dpm" files.

Yes you can open this sample files. They are similar to text files. To be honest, I always trusted the information in the summary report and never tried to count the particles from the sample (.dpm) files. But the number "12" isn't the number of the particles, it's a default number in the .dpm file. Look in the summary file (ending .PART also can be opend with txt editor). It should look like this for example:

Fate Number Elapsed Time (s) ....
Incomplete 2 5.739e-01
Trapped - Zone 26 630 ..........
Trapped - Zone 30 49 .......
.
.
.
Escaped - Zone 52 2620 ...............

I simulate a inspiration/expiration of particles in a lung and want to know where they deposit. I can't tell you anything about the Erosion/Accretion method, because I don't know it, hehe.

regards,
spring

Grüss dich!

As in simulating chamical deposition in lungs? Interesting work!

The zones don't correspond to anything I recognise however. Yours had specifically Zone 26 or so. I only have 25zones.. In any case it looks like this:
__________________________________________________ ______
Fate Mass (kg)
Initial Final Change
---- ---------- ---------- ----------
Trapped - Zone 10048 1.600e-01 1.600e-01 0.000e+00
__________________________________________________ ______

What do you think?:cool:

Guten Tag, haha!


My zones have numbers which correspond to walls, because they've been defined when the geometry was made. I think it's the same procedure like defining inlet and outlet boundaries, they are also zones with numbers.

My file from the summary report looks like the example from Fluent's user's guide page 1290 (chapter 23.7.2). That's all I can tell you.

Do you have any expirience with transient simulation? I think I have some questions.

Viele Grüße,
spring

Super! Dann kann wir ein bisschen deutsch reden, aber um das andere Leute uns auch verstehen sollten wir wahrscheinlich auf englisch schreiben.

Yes I defined all zones previously and otherwise the .dpm files look good. I.e. they show the particles which become trapped, but the summary file shows 'quatsch'. I will ask FLUENT customer help directly why this is.:cool:

Fire away your questions about transient simulations... I have some experience, let's see if I can help :).

Nicht schlecht deine Deutschkenntnisse!

First, that's waht I do:
My model is a part of a lung, with an inlet and five outlets. In this lung is a tube (for tracheal respiration). What I want to observe, is the influence of a tube while breathing air with particles (micro meter) with and without a magnetic field to trace the particles (for example to a tumor in the right lung). I've made steady simulations without a tube and it went very well. But the tube is causing problems (swirls, although it's a laminar flow -> Re<2300) (see attachment), so that it doesn't converge in a steady simulation. That's why I have to make a transient simulation. By the way my flow is incomprssible.

Now to my problem(s):
I have problems to let my simulation (just the flow) converge. As a convergence criteria (residuals) I chose a dorp of three orders ( but I chose REALTIV as the convergence criteria). My question is: is it too strict to choose only "relative" as a conv. creteria or should I choose "absolute and relative" ? I ask because when I chose "absolute & relativ" my solution converges at every time step, but doesn't when I choose just "relativ".

What I did, additionally is to lower the urf (under-relaxtion-factors) and then the solution was better. And I've chosen SIMPLEC as my solver because of my very small time step size.

I am also monitoring other values (max velocity in the outlets), but they don't make any sense when in one time step my solutin converges but in the next step it doesn't, then in the next 10 time steps it converges, then it doesn't ......and so on.

I've been playing arbitrarily for weeks with all paramters to let my solution converge, but I don't know if I can justify this parameters anymore.

I am so desprate. http://www.cfd-online.com/Forums/images/icons/icon9.gif

Interesting problem. It shouldn't surprise you greatly that the solution has a hard time converging given the geometry specification. Ie T junctions and the like. I have 2 questions:

1)How many iterations do you allow per time-step?
2)When you say your outlet velocities don't make sense, what do you mean?

When judging convergence via residuals it's always very hard given that your initial guess might be extremely close anyway. I usually use some sort of surface monitor... for example the concentration of some scalar at a certain point eg the outlets. Let's see if we can sort this one out.:)

Hi kingjewel1,

1, I allow 20 timesteps per iteration (my solution converges between 10 and 15 iteratiosns)

2, My outlet velocities don't make sense because they are very flat, and I don't thik I can't trust them if the residuals are not always reaching the convergence criteria.

By the way: my new time step is 1e-05s and I want to simulate 0.1s realtime, that means 10 000 time steps. That's toooooo much (I need at least 10 days to finish this simulation) but the flow needs 0.1s realtime to leave my geometry. Is there another way to say, that my simulatuion is converged without having to simulate all time steps?

Thank's for your help. :o
I really appreciate this, though I think there is no help for me anymore, :D.

Regards,
spring