有关DPM的问题.docx

1、有关DPM的问题1. DPMI d like to set 3 particle injections (e.g, 30particles for each injections) for different diameter of 20um,1um, 0.01um and compare the deposition velocity. i am using the unsteady tracking, the problem is when i starting the iteration, Fluent mix the 3 injections together, that is ,it

2、 will show on the console windows: number tracked=90,trapped=15,escaped 75,sth like this, so i cant get the trapped number of particles for each diameter. Can you help me? thanksHi I was thinking in your case! Why do you want to run the three diameters in only one iteration? I think you can run each

3、 diameter separately in order to measure the variable that you request, after all the particle tracking is individual for each particle and it is not affected by other particles! In addition I think that 3 point of injection are to low! Perhaps more point per area could be more representative for yo

4、ur case than 30 particles launched from one point! Give your comment back I am interested in your case! Alex thanks for your responding! I mean if I can submit 3 injections (just the particle diameter is different, the other parameters are the same) in one time steps and get the results seperately.b

5、ut now i can only put one injection at one time. for example, i need the results during 20 time steps, one time step costs 1 hour, then for one injection i need 20 hours, if i put the injection one by one, then i have to spend n*20 hours! so i wonder if i can put all the injections together, and the

6、n the time need is only 20 hours. hope i explain it clealy,thanks! HI Candy Yes I can help you! Solution Made Three files with the following format and information data (x,y,z,v,v,w,d,T,mass-flow)injectionID:particle ID) where x,y,z are the cordinates u,v,w, are the absolute velocity of the particle

7、s d diameter m T temperature Kelvin Mass-flow Kg/s Injection ID: particle ID=Injectioni:j where i the number of point for injection (in your case 0 to 2)and j the number of particle per injection point (in your case 0 to 29) Then read that files in your injection window (below single, group, surface

8、 you will see file) Then at the bottom of the injection window you will se a box with the name file. Click on the file. box and select the file (name the file candy0.inj, candy1.inj and candy2.inj) Then, run the particle tracking for you steady case Make sure that you are getting reasonable results

9、Then, write a UDF dpm Outlet to write a file with the variable that you wish Then, open reportdiscrete phasesample select you surface, injection and output file compute, plot the histogram reportdiscrete phasehistogram make sure that your statistical moments for the variables of concern does not cha

10、nge after incresing the number of particles Then, run the unsteady case with all you injections Import the output.dpm file to Excel Then, you can see the variable of concern for each injection ID:particleID Finally you can play with your results as you want! Have fun! If i miss something think smart

11、! Regards Alex Hi candy Now, I need you help I have not run unsteady particle tracking! could you please explain me how you do it Thank you Alex 1.Open DISCRETE PAHSE MODEL panel, select Unsteady tracking. 2. Go to Injections-set injection property-creat, if you select a surface as injection, then o

12、n the below of the panel, there will exist point properties for unsteady tracking, it will appear the item “start time and stop time, particle will be released at every time step during the period of time you defined. After the period of time you set, particle will still be tracked until all the par

13、ticle are trapped or escaped or. 3.note that unsteady tracking is calculated together with the fluid iteration,that is,open iteratepanel, and iterating, after each time step iteration, the particle will be released and caculated. hope the above is useful, good luck!unsteady particle tracking is only

14、 active when you select the unsteady option in the solver.hello Candy and Hedonist Thank you for your information! Regards Alex MUnoz Hi candy I forget to ask you one detail. is your DPM couple with the continuous fluid? becuase my case is not couple with the continuous flow, and I wonder if I need

15、to iteterate the flow. Thank you for answer me these questions! Best regards Alex Munoz My case is also not couple too, but it is also needed to iterate the flow, otherwise how can you do the unsteady tracking since the case and data file only record the flow in a definite time?Hi Candy Thanks a lot

16、 for your reply, I thought about it! Just I want to be sure Thank you Alex Munoz Hi candy I want to ask you another question! Perhaps, you wonder Why I dont run Fluent and I check for myself, Currently, we are making modification and I cannot run an iteration for more than 5 minutes using the GUI, i

17、f I run iteration for more than 5 minutes I have to do it under batch mode. I dont know if you have working under this mode but I have to be 100% sure what I am doing. The question is the following I have to report particle tracking under ReportDPMSample and I have to speficy the Start time and Stop

18、 time. Fluent documentation says the For unsteady particle tracking, clicking on the Start button will open the files and write the file header sections. If the solution is advanced in time by computing some time steps, the particle trajectories will be updated and the particle states will be writte

19、n to the files as they cross the selected planes or boundaries. Clicking on the Stop button will close the files and end the sampling I am very confuse with this information perhaps you can help to understand this issue. Thank you in advance! Alex Munoz 2. Problem of DPMDear everyone: I am using DPM

20、 method to simulate drops distribution in a compartment. The residuals are always oscillatory and dont converge. Could you please tell me how to make my solution convergence ? Thank you very much for your help. I am looking forward to your reply. With best regards, You I have exactly the same proble

21、m if it is any consolation!Hi you, can you give more detail on your case : coupled or segregated solver ? two way coupled dpm calculation or not ? with stochastic particle track ? does the calculation for the continuous phase converge without particle, . best regards Alain Hi Alain, Thank you very m

22、uch for your reply. I am using segregated solver and coupled dpm calculation with stochastic particle track. The calculation for the continuous phase converges without particle. The drop diameter is 1.2 mm. Do you provide enough information? Best regards, You Can it have something to do with how oft

23、en you inject particles ? ChristianDear you 1) Drop diameter is fairly big compared to the general DPM application. So, I think, its momentum source is fairly large. Because you use stochastic particle tracking, small change in momentum source in local area (local cell) can cause fairly big effect.

24、So, how about to try mean particle tracking (without stochastic option) ? 2) When I try DPM and convergence is difficult, I increase gas phase iteration, that is, 50100 iteration per each DPM iteration. At that time, I set residual convergence criteria very low value, e.g., 1.e-05. Then, iteration i

25、s continued. After many iterations (at least 50100 DPM injection iteration), I check every residual whether they are enough low or not. With this approach, in general (not every case), I was successful. Hi, Thank you very much for your reply. I have tried injecting particles every 5 to 20 iterations

26、. With best regards, You I hope that it might be helpful to you. Sincerely, Jinwook Dear you I agree with jimwook. Your lack of convergence is certainly do to stochastic tracking. Note that this can also be the result of a physical phenomenon ! Stochastic tracking introduce implicitly a temporal ter

27、m in the momentum equation due to fluctuation of the term of exchange. This can be observed experimentaly in dense two phase flow such as pneumatic transport or fluidized bed. Take a look at your momemtum source term and your flow pressure and velocity field. Your source term can fluctuate but your

28、field can be steady. In this peculiar case your flow is converged even if your residuals remains high. At last, if your flow diverge, you can also underrelax the source term coming from DPM. Best regards Alain Add to previous comment : Increasing injection number might be helpful for convergence bec

29、ause momentum source of each injection is relatively small with many injection number. Sincerely, Jinwook3.Using file to define injection distribution!(DPM)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 temperat

30、ure mass-flow) name ) But whats the files 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 ) (# # # # # # # # # # #) inject

31、ion0:2 ) . . . (# # # # # # # # # # #) 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 files type, another word, what kind of files can be accessed by fluent? I have tried .txt, .c and so

32、 on, but they cant 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 injecti