Hello,

In fluent DPM, particle initial conditions can be read from an external file. The file has following form:

((x y z u v w diameter temperature mass-flow) name )

But what's the file's format??

Thank you for your help!!

winnie

Hi wiinie

The file has the format that you write ((x y z u v w diameter temperature mass-flow) injection0:ID ) ((# # # # # # # # # # #) injection0:0 ) ((# # # # # # # # # # #) injection0:1 ) ((# # # # # # # # # # #) injection0:2 ) ... ... ... ((# # # # # # # # # # #) injection0:n )

where # is a number under the unit that you are using.

Regards

Alex Munoz

Hi, Alex Munoz

Thank you for your answer. I would also like to know the file's type, another word, what kind of files can be accessed by fluent?

I have tried .txt, .c and so on, but they can't be input to the fluent.

Waiting for your answer!

By the way, if I have four injections, can I use four single injections? Does it have any difference with a file injection?

Regards

winnie

Hi winnie

The file is a text file, For instance I generate a file using a C code that I wrote, then I name it "bach.inj"

YOu can create four files or I guess you can write just one file containing 4 injection like this

{{ }injection0:1} ... ... {{ }injection1:1} ... ... {{ }injection2:1} ... ... {{ }injection3:1} ...

Regards

Alex Munoz

Hi, Alex

I still can't import the file to the fluent. It really confused me!

My procedure is

firstly, I create my file using C code as follows:

{{-0.0087 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.000006554} injection0:1} {{-0.0029 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.000006554} injection1:1} {{0.0029 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.000006554} injection2:1} {{0.0087 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.000006554} injection3:1}

then, I save it as 'initial.inj'

next, in fluent 'set injection properties' panel, I choose file as injection type and after put down the botton 'file...'at the bottom, I can find 'initial inj'file in dialog box, I choose it.

finally, I go back to 'injections'panel, choose the injection which is defined by the file, and put down the 'list' botton, then in fluent console window, there are following messages :

Number of injections read in=0

Particle streams from injection-0: STREAM ...........................INITIAL VALUES........................... NO TYP (X) (Y) (Z) (U) (V) (W) (T) (DIAM) (MFLOW)

It seems the injection failed. What's the matter?

Sorry to bother you so many times! But your help is really valuable for me !

Regards

winnie

Hi

You forgot to put and initial text like this

{X Y Z U V W Diameter Temperature mass-flow}injection:ID name}

In addition, you need to put a end of the line at the end of each data row

let me send you and example of my file and you see for yourself(I send the file to your e-mail adddress due to confidential issues)also you should locate your initial.inj in the directory that you launch fluent

Regards

Alex Munoz

Hi winnie

I apologize for confuse the braquet that you should use for your injection file, intead of {} use ().

the format is

(X Y Z U V W Dameter Temp Mas Flow name) (# # # # # # # # #)injection0:1)

I am so sorry for the confusion.

Regards

Alex Munoz

Hi, Alex

What I can say now is only thanks! Thank you for your kindly and valuable help!!

Regards

winnie

Hi, Alex

I am so sorry that I have to bother you once again. I followed all you have told me and after importing the initial.inj file to fluent, I list the injection and the message in the fluent console window is:

Error: FLUENT received fatal signal (ACCESS_VIOLATION) 1. Note exact events leading to error. 2. Save case/data under new name. 3. Exit program and restart to continue. 4. Report error to your distributor. Error Object: ()

when I list the injection once again, the message in the fluent console window is:

Particle streams from injection-0: STREAM ...........................INITIAL VALUES........................... NO TYP (X) (Y) (Z) (U) (V) (W) (T) (DIAM) (MFLOW)

171977144 IN -8.70e-03 0.00e+00 0.00e+00 0.00e+00 8.20e-03 0.00e+00 2.00e+01 3.00e-03 6.55e-06

0 IN -2.90e-03 0.00e+00 0.00e+00 0.00e+00 8.20e-03 0.00e+00 2.00e+01 3.00e-03 6.55e-06

It seems that fluent has catched two injections, but where are the other two?

Then I copied the case you give to me and the result is the former.

I am so tired that I neally want to give it up. Maybe I still neglect something? By the way, the .inj file should be saved in the same directory as the case file, yes?

Anyway, I really appreciate your kindly help!Thank you.

Regards

winnie

Hi Winnie

Do not quit! Do not get emotionally involve with your project!

I can guess what's going on!

The access violation means that you have not follow a logic secuences of events for your calculation.

I will tell you how I run my particle tracking with an injection file readed from my directory file

1) put the injection file "initial.inj" in the directory that you have the case and data files.

2) open fluent, set the dicrete phase parameters, then under injections read the injection file.

3) open display/particle tracking/select the injection and the particle ID that you want to plot.

4)once you clik ok, you will see that the program reads the injection file and executes the calculation!

5) then, you can list the injection files and soon!

COULD YOU PLEASE TRY A SIMPLE FILE with different name and with a fresh case and data file from your steady state calculation. I mean less than five rows of data and only one injection, instead of a long data file. This will help you to check everything faster.

I think you cannot list the injection without running first a particle tracking!

By the way, could you please tell me if you plan to run steady or unsteady particle tracking. Perhaps I will need your help later on!

Let me know what happen to your case!

Regards

Alex Munoz PS: Everyone face day of completely frustrations others like me had faced months of failure, then you learn as long as some pay my time who cares.

Thank you, Alex. I don't know how to express my gratitude!

Yes, I have tried following your procedure and found that when I write only one or two injections in my data file, fluent can catch the injection but there are messages as follows:

ERROR reading injection 0 for injection: injection-0.

Number of injections read in=2

number tracked = 2, escaped = 2, aborted = 0, trapped = 0, evaporated = 0, incomplete = 0

But when I add my injection number more than two, there are access-violation messages.

I am simulating bubbly flow in virtical pipe. Since I hope to get the new continuous phase velocity field after the bubbles are injected, coupled is necessary and as for steady or unsteady, I am still hesitating. Because I want to get the local void fraction of bubbles,and steady simulation will make the local void fraction incontinuous, and in the real bubbly flow,the bubbles' trajectories are some stochastic, an unsteady calculation may be closer to the real case and can give me more information.

Regards

winnie

Hi winnie

I was wondering was going on... FLuent should be able to read your file

It seems to me that one of the x ,y, z coordinates is out the domain. Ohh yes that is the problem. Could you please locate your injection points a few milimiters far from the inlet and walls.

Also check that your C-code is generating x-y-z values inside the domain.

Regards

Alex Munoz

Hi, Alex

I checked the location and they are surelly in the domain. Then I have another try. I locate all the injections nearlly at the center of the pipe, the fluent catch these injections. But there still the messages:"ERROR reading injection 0 for injection: injection-0."

Thank you! Alex. anyway, this has made me take a deep breath.

But what should my locations do now?? ^_^

Regards

winnie

Hi,Alex

I have tried many injection locations and find that whether fluent can catch the injections depends on the location coordinates.

but it is really strange. Here is my domain extents:

x-coordinate: min (m) = -1.449986e-02, max (m) = 1.449986e-02

y-coordinate: min (m) = -8.829759e-18, max (m) = 3.700000e+00

z-coordinate: min (m) = -1.450000e-02, max (m) = 1.450000e-02

and the injections:

((x y z u v w diameter temperature mass-flow) name)

((0.001 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.0000016385)0)

((-0.001 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.0000016385)1)

((0.0001 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.0000016385)2)

((-0.0001 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.0000016385)3)

((-0.002 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.0000016385)4)

((0.002 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.0000016385)5)

((0.0015 0.0 0.0 0.0 0.0082 0.0 0.003 20.0 0.0000016385)6)

can all be catched by the fluent.

when x-coordinate exceeds 0.002, there will be "access violation" message.

So strange!!!

Do you know what's the matter?

Regards

winnie

Hi winnie

Your domain is a pipe with diameter 2.88cm therefore, you cannot locate particle at the edge, talking in radial coordinates at R=1.44cm. You must locate the injection point one milimeter from the wall(R=1.34). In addition, put the particles at less one milimeter inside the domain in the y direction if you put them at 0.0 the code cannot asign this position. Keep in my that your domain in the y-direction is 3.7 m one milimeter difference isnot going to affect your calculation!!

Now, I do not know your problem. However, you have to distribute your particles in a rand manner. The distribution should be equal number of bubbles per flow rate of continuous flow. If your injection point is not a jet!!

The bubble velocity should be absolute not relative as a results the bubbles near to the wall must have 0.0 m/s y-velocity and at the center the maximum velocity of your velocity profile

Again, I do not your problems but your bubbles seem to me too big to apply the DRWM, the biggest diameter that I have seen is 1.0mm

Please, temperature in Kelvin. K=C+273.15. therefore 293.15K not 20

And finally, injection name. You better use injection-0:1..... injection0-N.

Regards

Alex Munoz

Hi, Alex

Many, many thanks to your kindly help!!

I am simulating the laminar bubbly flow in vertical pipe. The geometric and boundary conditions are from the data I have got. What I hope to calculate from the DPM simulation is the local void fraction and if possible, the liquid velocity field. I know that fluent neglect the volume effect of the bubble to the continuous phase, but I don't know how this negligence will effect the result of the simulation calculation. Do you think it is suitable to use DPM for bubbly flow simulation with bubble diameters around 3mm?

Waiting for your suggestions!

It seems that I have too many questions. ^_^ Hope you have a chearful mood!

Regards

winnie

HI

Because I never answer a question if I am not 100% sure, I could not give any coment about the bubble size. However, I suggest that you read this paper.

Coupling of a Langrangian model with a CFD code: Application to the numerical modeling of the turbulent dispersion of droplets in a turbulent pipe flow. DOMGIN JF, HUILIER D, BURNAGE H. GARDIN P. Journal of Hydraulic research vol 35, 1997, no4

I need to ask you that help another user that is having problem with DPM, his name Gael Corre.

Thank you in advance

Alex Munoz

Hi, Alex

Don't say 'thank you' to me and it is me that should thank you.

I will try my best to help anyone I can because during my studying I have got so many helps from others, especially you.

But in fact, I am still a fluent beginner, what I have done is only 'eat' the fluent document. By now, I haven't calculate a result successfully. I am working hard!

Regards

winnie

[CaryKenny]

hi all

regarding the injection file, to recall, the file is to be written like the following, e.g.:
(( x y z U V W particleDia particleTemperature massFlow) injection:0)


Assume I have 2E-6 kg of mass.
Density of the solid is 1500 kg/m3.
Assume I have particle dia of 50E-6 m (50micron).

How do we calculate the massFlow?
Hope anybody can help

many thanks
cary

[Zabulor]

Hello CaryKenny

You can't calculate it with the data available. You have to know the time during which your m =2E-6 kg of particle are injected. Then your massFlow is = m/t.
Do you have this information ?