# 2 phase flow (3D)

 Register Blogs Members List Search Today's Posts Mark Forums Read

 December 7, 2009, 04:07 2 phase flow (3D) #1 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 i am modeling gas–liquid flow in pipes and i have a question if i want to draw the XY plot to show the velocity change across the pipeline ... how to do it ,most of the pipeline tutorials are symmetric so they take it around the centerline which is not my case. which iso-surface should i create ? so can any one help please Thank you !!!!

 December 7, 2009, 16:06 #2 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 Hi I am working on the same topic using VOF, so i hope we can have some little useful discussions About ure question, i didnt understand what do u want to plot...but anyway, no need for iso-surfaces if u can explain ure question, i can help u regards

 December 8, 2009, 02:35 #3 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 I am also using the vof to solve the problem and its my pleasure to have further discussions. there is a tutorial i have called "Simulation of Flow Development in a Pipe"... but it is a single phase flow..in the tutorial they Plot the XY profile which shows the Position(x axis) against Velocity (Y axis) ... in the tutorial only a semi circle is drawn and it is defined as symmetric and an iso-surface is defined depending on this symmetry. and then XY plot selected i want to plot the same profile but in our case the pipeline flow is not symmetric.so dont know what to do ? hope my expalnation made you understand more Anyways thanks for your help....

 December 8, 2009, 03:51 #4 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 yes i understand a bit what do u want, but i mean what is the objectif? u want to know if ure flow is fully developped?????? if yes tell me , if no correct me. Anyway friend, i hope that u are using an unsteady solver. A steady one cant do the job. In multiphase, developpement is a bit different than in monophase. U must monitor data to know if u are converged.... I think that u want to draw a isosurface of pressure to see surface drop (that is what i understood) but this is not a lot feasible in multiphase. If u are introducing surface tension, the pressure wont be the same over a section...... U must average data be4 comparing profiles..... If u want any details tell me and tell me also what is the objectif of ure isosurfaces I want to ask u a question too: do u have experimental data? or are u using a multiphase chart? if yes wich one? Regards

 December 8, 2009, 04:09 #5 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 Actually i am a new user to fluent i just learned it one month ago self learning so i i go on i learn more but i have a task to make a "2 phase flow simulation in a pipeline" and should be submitted at end of the month .... it seems you're much more ahead of me so its very nice to learn from you ... yes i am using a unsteady solver, but i think i knew one one my problems that i might be trying to use the monophase tutrials and adapt it to the multiphase which is not correct i assume ..... actually i have a paper named "CFD modeling of flow profiles and interfacial phenomena in two-phase flow in pipes" it contains expermintal data and solved using fluent i am trying to do something similar if you want me to send it send me your mail... if you can help me doing this i will be so grateful Thank you for your help

 December 8, 2009, 04:33 #6 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 i have seen the paper u are talking about....I dont remember it very much but i think that they just performed cacultion for stratified flow no??? I will give u some hints for ure work anf if u need more help, u tell me: 1-Let the 2 phases enter the domain from the same inlet. If u perform separated inlets, u will have problems with the flow developpement... 2-Make ure pipe enough long. Monitor variables to know when do u get convergence. 3-When u average ure data (to examine the pseu steady state), make sure that the flow is fully developped.(in other meaning, that ure pipe length was enough) For turbulence model, if ure pipe is straight (no dean vortices) and circular (no recirculations), i think any turbulence model can do the job....If not, theoritically, RSM must be the best....but only in theory...Somtimes isotropic models can be better... U can also use the laminar model of Fluent. Laminar model of Fluent is a DNS so it is direct solution of the NS equations and the best to use with vOF however, as ure Re is big, u will never get a real solution if u not use a very fine grid and a very small time step....but the result can be good anyway. So are u just trying to model stratified flow or other regimes? (such annular or slugs?...) If u need any help tell me and if u have other papers tell me also please Regards

 December 8, 2009, 04:59 #7 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 yes my i just modeling stratified flow at the moment ... Thank you for your hints 1- for the inlet ..the two phase enter from the same inlet but its separated .To imagine it consider a circle cut into two halves the upper is gas inlet the lower is liquid inlet and once they enter the start mixing ..am i doing it correct 2-my pipeline is 50 m long dont know whether this is enough or not 3- thanks for u tips about turbulence and laminar models 4- yes i have other paper concerning 2 and 3 phase flow i hope they are related to what you are doing so shall i write their names or directly mail them i have no problem

 December 8, 2009, 15:23 #8 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 Hi again for the papers mail it for me please (cfduser@live.fr) and thanks in advance 1-I would prefer that u dont divide the inlet in 2 parts...In fact, imagine that the real water height in the channel is 2cm, and that in ure simulation, ure water inlet (or the lower part of ure inlet) is 3 cm. So, to get ure real solution, Fluent must lower ure water height from 3 cm to 2 cm right??? The water will loose height due to friction with the air phase, or the air phase is 1000 times lighter than the water, so lowering water height to 2 cm will recomend an enormous amount of momentum transfer.....That is my opinion. I think that u will need a lot more of pipe length to get a fully developped flow. SO the best solution in my opinion is to have a single inlet, with water and air coming from it. This is the best choice, unless u are searching to calculate the length needed by the flow to fully developp.... 2- 50 m is enormous....u will need a lot of time to converge(if u want to do a DNS with grid independance solution, u will need more than a year of calculation..)...the length needed by the flow to be fully developped depends on the volume fraction, on the fluid proprieties, the flow configuration and the pipe diameter.... Some flows as slug flows sometimes need 100 m to get a fully developped state...so the length needed depnds on every simulation... Anyway, i think 50 m is too much. If ure pipe diameter is d, i think a length of 100 d is really sufficiant. If ure simulation shows that 100 d was not enough, than u can try a longer pipe.... If u give me more details about ure pipe diameter and the flowrates that u want to simulate, i can maybe advice u more . Hope that i could be clear If u need anything more, tell me please and tell me about ure results whenever u get it. Regards and good luck

 December 9, 2009, 02:59 #9 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 hi i sent you the papers hope they can help you 1-if i made the a single inlet how would i control the velocity of the mixture entering mixture ? in other words how do i set my boundary conditions ? all i know is setting the velocity ( say x m/s) and the Liquid volume fraction . 2-my pipeline diameter is 1 inch so should my pipeline length be 100 d which is about 2.54m long is it enough !!! your tips are very helpful i dont know what to say thank you!!!!!

 December 10, 2009, 14:31 #10 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 Hi thanks very much for the articles 1-For a single inlet: u know ure gas and liquid flow rate. In fluent, u must give it those same flow rates but in specifying one velcity and a volume fraction so: Ql=alpha*V*S Qg=(1-alpha)*V*S Alpha=liquid retention V: velocity at inlet (in simulation) S: surafce of inlet Ql: liquid flow rate 2 eq, 2 unknowns 2- 2.54 m is theoritically sufficient in experiences....In simulation u will MAYBE need some more length. We cant know the solution a priori. U must try to see if it sufficient or no.... Take care and hope to talk again

 December 14, 2009, 02:52 #11 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 Thank you for your tips and hope that the papers are helpful !!!! Can you explain more please 1- while setting the Boundary conditions for the inlet i have only two Data spaces to fill a)the Velocity magnitude so how should specify both the velocity of both gas and liquid b) volume fraction it depends on the air to liquid ratio . i am ok with it 2- how to know whether the pipeline is sufficient or not what should i expect ? thank you for you help Regards

 December 14, 2009, 17:00 #12 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 Hi my friend 1- as i explained before, u choose the flowrates of each phase: Qg and Ql. Qg=alpha*V*S Ql=(1-alha)*V*S So u have 2 eqs. and 2 unkowns that are V and alpha, that u must give to Fluent. 2-U must monitor data. When ure data monitors become to show steady (oscillatory around a certain mean) behavior, u must average ure variables in time (in the iterate pannel). After a certain time, u look to ure unsteady statistics: if ure mean velocity profile does not change with x (the pipe axis) that means that ure solution is fully developped and that ure pipe lenth was sufficient... I hope that i coule be clear with my bad english ...(if u understand french, it will be very easier to me to explain...)If i was not clear, write to me again Regards

 December 15, 2009, 02:59 #13 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 heeey unfortunately i i cant speak french but i understand you English its very well written but if you prefer to write in french you can and there is a friend of mine who can translate or just use the google translator if this is easier "if ure mean velocity profile does not change with x (the pipe axis)" this is what i am trying to plot but i fail each time so how can i plot it your tips and hints are very useful thank you

 December 15, 2009, 07:58 #14 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 hello again i will speak in english if u say that u understand me u must do some segments (surface-->line) that are orthogonal to the x axis in different locations, then plot the mean xvelocity PROFILE (mean=average in time) on those segments, and see if it the same. If u want, any mean profile on these segments must be the same if ure flow is fully developped.(or from the location where ure flow become fully developped) Of course, the instantaneous profiles are not the same since u can have waves on the interface. (u can also have eddies that appears and disappears....) So the mean profiles can tell u if ure flow is fully developped and steady, and ure instanatnesous profiles will tel u about ure flow regime (stratified, stratified wavy, slugs..) N.B: u must be sure also that u reached the steady state, i mean that at the same location, the mean profile % time does no more change too.

 December 16, 2009, 03:12 #15 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 heeeey i am very grateful for your tips 1-instantaneous profiles how can i do it 2- the mean velocity profile can we do this using surface----->iso-surface or not? 3-what do you mean by S: surface inlet area (formula area of circle) thank you

 December 16, 2009, 03:59 #16 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 hi 1-plot--->xyplot--->velocity 2-plot--->xyplot--->unsteady statistics (it will appear after that u do ure time average) 3-yes did u finish ure first simulation???

 December 16, 2009, 07:51 #17 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 heeeeey again , i am very sorry if i am disturbing you actully i am still entering random data ....to try to draw the xy profile velocity and i am still failing dont know how to choose the points depending on what my current pipeline is horizontal on the Positive Z axis with a diameter of 1 inch and length of 5 m . i will keep trying

 December 16, 2009, 17:05 #18 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 hi no problem comrade u can ask me and i will answer when i am here (if u have a lot of questions, try to ask it soon because when i go to holidays, i will not have internet) For the xy plot: u are trying to plot a profile on a segment that is parallel to the y axis? if yes, so in the plot xy plot pannel, there is a place where it is written x 1 y 0 z 0 so put x 0 and y 1 and then try to draw the plot If u still face problems (or didnt understood what i have written), tell me

 December 17, 2009, 03:44 #19 Member   Sherif Join Date: Mar 2009 Posts: 33 Rep Power: 10 heey, thank you actually my problem is is creating the Line/rake it self or should i create a plane or an Iso-surface? i am making plot a profile on a segment that is parallel to the z axis? so x 0 y 0 z 1 and i have another question can we do the same procedure if i am modeling gas condensate in pipes hope you will enjoy your holiday ; )

 December 17, 2009, 09:17 #20 Senior Member   karine Join Date: Nov 2009 Posts: 158 Rep Power: 9 hi if u draw a line rake, u can PLOT a profile on it and u can compare results on excel.(or in Fluent also if u want) so u can know if u reached steady and fully developped state For the questin 2, i didnt understand it. U want to model gas condensation? u mean that u have phase change? If that is the case, i dont know if Fluent VOF can handdle it. I never tried this be4 but of course there will be a problem: Vof give the same velocity for air, liquid, and the interface at the interface. If u have phase change, all this will not be true so i dont know if there is options in Fluents that allow to do thus simulations in VOF.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Sandeep Rane Main CFD Forum 9 February 17, 2010 07:23 shashwat Main CFD Forum 0 April 4, 2008 02:20 KK CFX 5 February 14, 2008 17:48 Madhavi Krishnan FLUENT 3 June 6, 2005 05:52 Nicolas Main CFD Forum 0 December 13, 2003 15:19

All times are GMT -4. The time now is 21:08.