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 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 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 your 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.but 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 then 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 particles 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 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 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 change 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! 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 on 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 particle 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 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 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 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, if 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 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 written 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 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 problem 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 much 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 often 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. 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 is 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. 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 term 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 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 because 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 temperature 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 ) (# # # # # # # # # # #) 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 files type, another word, what kind of files can be accessed by fluent? I have tried .txt, .c and so 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 injection like this injection0:1 . . injection1:1 . . injection2:1 . . injection3:1 . Regards Alex Munoz Hi, Alex I still cant 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 injfile in dialog box, I choose it. finally, I go back to injectionspanel, 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. Whats 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-flowinjection: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 address 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 whats 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 dont 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 vertical 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 in continuous, 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 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 whats the matter? Regards winnie 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 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 dont 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