
[Sponsors] 
March 13, 2009, 16:12 
Hi..
my task is to simulate a

#1 
Member

Hi..
my task is to simulate air particle being injected (at the center) to the water as continuous medium. (Becker case) (Domain being simple 2D rectangular region sides and bottom (except at the center) being walls. Velocity inlet at the center and pressure outlet at the top) Boundary conditions 1) alpha 0 gradients at the wall 2) inlet uniform 1 3) 3/4 th water (continous phase) filled so alpha being eual to 0 and remaining 1/4 air(discrete phase) and alpha being 1 4) alpha being 1 at the "top" where pressure outlet boundary conditions are set top { type inletOutlet; inletValue uniform 1; value uniform 1; } 5) at the inlet region alpha being 1 velocityinlet { type fixedValue; value uniform 1; } am using twoPhaseEulerFoam solver also I would like to know which could be the best solver when compare with bubbleFoam (turbulence being on) Simulation errors: When I try with these boundary conditions for alpha and with 0.9 m/s velocity at the inlet (air velocity) diameter of the particle being 0.00003 m after few iterations courant number increase (around thousands!!) though the grid is not that fine also very small time step being employed. Finally simulation crashes I want to know whether boundary conditions are to be altered or there I have to modify the solver and recompile again!!?? Awaiting for replies! Regards Raghavendra 

March 14, 2009, 13:21 
Hi,
you have already asked

#2 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
Hi,
you have already asked your question here, you repeated it http://www.cfdonline.com/cgibin/Op...how.cgi?1/6412 and you wrote it personally to me, at least. I can understand you need the answer, but  You should not write multiple posts about the same problem, by simply cutting and pasting you question.  You should not hijack a thread asking something not related to the topic in the title.  You should _wait_. People is here on a volunteer basis, and these behaviours are a good way NOT to get an answer.  To obtain answers from me there is an additional condition: you need to put a working email contact in your _public_ profile, so that if someone else has a similar problem, he can contact you eventually. We should be a community of users, and help each other in the end, and not just ask and run away. About your problem, bubbleFoam and twoPhaseEulerFoam are very similar. In twoPhaseEulerFoam you can select different drag laws and other submodels, but the basic algorithm is exactly the same. For the simulation setup, you might want to take a look at H. Rusche PhD thesis, that can be downloaded from www.foamcfd.org website. Regards, A. 

March 14, 2009, 13:35 
Hello Alberto Passalacqua..and

#3 
Member

Hello Alberto Passalacqua..and others.
Yes I repeated the same question in other thread also hoping I get some replies.. yeah ..now I understand I have to wait and this kind of mistakes wont be repeated again. Also regarding the email contact you mentioned, am a student and that is the reason I have give my personal mail ID. I was very much new to the forum and OpenFOAM that made me to put my queries in other thread also. I wont hesitate to ask "sorry" regarding this and I this kind of mistakes wont be repeated again.. Regards Raghavendra 

March 14, 2009, 13:38 
and coming back to the topic.

#4 
Member

and coming back to the topic.
thanks for the H. Rusche PhD thesis I think this will be quite useful to perform my task.. thanks a lot Alberto Passalacqua Regards Raghavendra 

March 14, 2009, 15:34 
No problem, and sorry if I sou

#5 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
No problem, and sorry if I sounded too rough :)
What is the order of the time step you are using? Check if the lift force and the virtual mass coefficients are set correctly for your case too. P.S. About the email, I meant your contact is not visible in your profile here http://www.cfdonline.com/cgibin/OpenFOAM_Discus/boardprofile.cgi?action=view_profi le&profile=raagh77users ;) 

March 14, 2009, 17:35 
Hi Alberto Passalacqua,
Tim

#6 
Member

Hi Alberto Passalacqua,
Timestep I am using is 1e4 Cvm as 0.5 Cl 0 Ct 1 (which I copied from bubbleColumn tutorial) also this time I included relaxation factors but even that didn't work simulation got crashed with high timestep continuity error.. I checked the pressure values and it was in the range of 1e14 surprisingly !! these are my boundary conditions parametersinletoutletwalls alpha110gradient epsilon0.10.10gradient k1e81e80gradient p0graduniform 00gradient Theata1e081e080gradient Ua00fixed value 0 Ub0.1m/s0fixed value 0 finally in my profile settings accidentally Do not display my real email address with my profile was checked.. now my email id is visible thanks for notifying me about that Regards Raghavendra 

March 14, 2009, 23:22 
Hi,
I'm running a simple t

#7 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
Hi,
I'm running a simple test case like this base = 0.2m height = 1m initial liquid height = 0.45 I'm using your data and an inlet 4cm wide just to try to see what happens, and the solution is very stable with dt = 0.001s also on a poor quality grid. What is you geometric setup? About relaxation factors, you should not use them in bubbleFoam/twoPhaseEulerFoam or you will delay your solution in time. Regards, A. 

March 15, 2009, 08:50 
Hello Alberto Passalacqua,

#8 
Member

Hello Alberto Passalacqua,
Thanks for your concern my simulation domain details are .> base 0.5m .> height 2.5m .> initial liquid height 2m .> inlet 4mm (probably this could be the problem!!?) .> velocity inlet 0.9m/s. Is it possible to share the test case files with me? so that I can compare with mine.. Awaiting for your reply.. Regards Raghavendra 

March 15, 2009, 08:53 
Hello Alberto Passalacqua,

#9 
Member

Hello Alberto Passalacqua,
Thanks for your concern :) my simulation domain details are base 0.5m height 2.5m initial liquid height 2m inlet 4mm (probably this could be the problem!!?) velocity inlet 0.9m/s. Is it possible to share the test case files with me? so that I can compare with mine.. Awaiting for your reply.. Regards Raghavendra 

March 15, 2009, 22:17 

#10 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
Hi,
no, the problem is not the small inlet. It is the turbulence model. If you switch it off, the simulation proceeds without problems. I didn't play with its parameters, but the problem is there. You might want to consider other approaches instead than a mixture turbulence model based on transport equations. For example:
Do you take the gas velocity at the injection from the experiments? I didn't check Becker's work, but it seems high, considering you have 0.45 cm of water. 

March 16, 2009, 07:22 

#11 
Member

Hi Alberto Passalacqua,
Yes as you said the gas velocity at the inlet was not same as in Becker case. I made the following changes (corrected mistakes) . increased inlet width (4cm) . reduced velocity at the inlet (0.1 m/s) . and the direction of gravity force was wrong, it was in zdirection and the simulation is stable now (with turbulence being on) Now I will try to simulate with the exact dimensions as in the Becker case (my test case was not with the same dimensions as of Beckers' case) I think it shouldn't create problems Finally the references you quoted is quite useful, I will go through it before simulating with the exact dimensions as in Becker case.. I am really thankful for your support Regards Raghavendra 

March 16, 2009, 11:13 

#12 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
Hi,
happy to here it's working! Are you going to do a validation against experiments of the code? It would be interesting to see the results if/when possible! Regards, A. 

March 16, 2009, 16:06 

#13 
Member

Yes, am trying to simulate Becker case and compare the results experimentally done by D. Pfleger and S. Becker .
Moreover am very much new to the OpenFOAM and what I do could be very much simple to others I will definitely share the results with the community if something interesting yeah my test case was quite successful but now am trying to simulate with the exact dimensions as mentioned in the "Becker case". 0.2 m width 0.6m width (0.45 m hegith of the liquid column) 1mm inlet air velocity 0.17cm/s other parameters being absolutely same. but after 2 or 3 iterations i ll get some error msg (this time even cournat number is well with in the limit and even timestep continuity error is with in the limit) I will copy paste the error message what I get.. Courant Number mean: 2.32789e05 max: 0.0723331 Max Ur Courant Number = 0.222155 Calculating averages Time = 0.016 DILUPBiCG: Solving for alpha, Initial residual = 3.06836e07, Final residual = 2.36065e11, No Iterations 1 Dispersed phase volume fraction = 0.257994 Min(alpha) = 1.0429e20 Max(alpha) = 1.0026 DILUPBiCG: Solving for alpha, Initial residual = 3.05854e09, Final residual = 1.83218e13, No Iterations 1 Dispersed phase volume fraction = 0.257994 Min(alpha) = 9.43671e20 Max(alpha) = 1.0026 #0 Foam::error:rintStack(Foam::Ostream&) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0xb80e3400] #3 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #4 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #7 Foam::fvMatrix<double>::solve(Foam::Istream&) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libfiniteVolume.so" #8 main in "/home/ragh/OpenFOAM/OpenFOAM1.5/applications/bin/linuxGccDPOpt/twoPhaseEulerFoam" #9 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #10 Foam::regIOobject::readIfModified() in "/home/ragh/OpenFOAM/OpenFOAM1.5/applications/bin/linuxGccDPOpt/twoPhaseEulerFoam" [1]+ Done paraFoam Floating point exception Is the real problem is with the small inlet (sorry I am repeating) and small grid size at the inlet ?? as all parameters except small inlet are same Regards Raghavendra 

March 16, 2009, 16:39 

#14 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
Does it run switching the turbulence model off? Could you post the case or email it to me so I can check it?
Thanks, Alberto 

March 16, 2009, 16:58 

#15 
Member

Hi..
Yes I switched off turbulence and gave a run but again I am getting the same error. I will send you the case file to your mail Regards Raghavendra 

March 16, 2009, 17:38 

#16 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
Hi,
I remeshed the domain because you splitted the inlet face in three, but you did not project it on the outlet face, so the mesh is not perfectly orthogonal. In GAMBIT simply build two rectangles: one big as the bubble column (0.2 x 0.6m) and the other (0.001 x 0.6m). Move the second along x of 0.0995 so to have it in the centre, and then use the split function. Your bubble column is now divided in three. At this point create a nonuniform mesh on the base, but not along the height. In my example I put six cells inside the inlet and used the bellshaped distribution on the inlet sides, with a base step of 0.002m. Pay attention to specify the nodes also on the outlet at the same time, or the mesh generation will not give rise to a perfectly orthogonal mesh! With this mesh, I can run the laminar case without any problem, but the turbulent one doesn't work. You might want to check the parameters. Btw, I changed also the outlet boundary conditions to have a "cleaner" solution, especially for the velocity fields. There is no backflow at the outlet (and if there is you can avoid it by increasing the height a bit), so you do not need the InletOutlet. Simply use a fixedValue for pressure, and a zeroGradient for the other quantities. Check your email for the updated case. I hope this helps. 

March 17, 2009, 06:02 

#17 
Member

Hi Alberto Passalacqua,
Yes, as you said the simulation is quite stable with turbulence being off (even I tried with my earlier mesh in both bubbleFoam solver and twoPhaseEulerFoam solver). Now, in order to include turbulence I thought to map the results from laminar case and start that as my initial conditions. (According to the tutorial cavityFine in userguide). Hope it will work Regards Raghavendra 

March 17, 2009, 10:43 

#18 
Member

Hi ..
am back unfortunately with probelms again.. I tried to simulate the case with turbulence being "on" so that it can be compared with experimental results.. As I said in the previous post I started with mapFields (mapping results from laminar case to the turbulent case and using this as my initial solution). When I switch on turbulence after few iterations its the same old problem..simulation crashes with the following error Time = 0.005 DILUPBiCG: Solving for alpha, Initial residual = 1.45502e06, Final residual = 1.68436e12, No Iterations 1 Dispersed phase volume fraction = 0.25 Min(alpha) = 5.92206e08 Max(alpha) = 1.00039 DILUPBiCG: Solving for alpha, Initial residual = 1.21911e09, Final residual = 2.57683e16, No Iterations 1 Dispersed phase volume fraction = 0.25 Min(alpha) = 4.0857e15 Max(alpha) = 1.00039 GAMG: Solving for p, Initial residual = 0.000977288, Final residual = 8.85769e09, No Iterations 14 time step continuity errors : sum local = 1.81087e08, global = 2.49117e10, cumulative = 1.17943e09 GAMG: Solving for p, Initial residual = 7.59477e05, Final residual = 6.43625e09, No Iterations 12 time step continuity errors : sum local = 6.608e08, global = 1.14294e08, cumulative = 1.26088e08 DILUPBiCG: Solving for epsilon, Initial residual = 0.873223, Final residual = 7.10405e06, No Iterations 56 DILUPBiCG: Solving for k, Initial residual = 0.999832, Final residual = 0.00272598, No Iterations 1001 ExecutionTime = 7.93 s ClockTime = 8 s Courant Number mean: 0.0664316 max: 61.9321 Max Ur Courant Number = 63.6085 Calculating averages Time = 0.006 DILUPBiCG: Solving for alpha, Initial residual = 0.00329163, Final residual = 1.74616e11, No Iterations 10 Dispersed phase volume fraction = 0.25 Min(alpha) = 0.230798 Max(alpha) = 3.05932 DILUPBiCG: Solving for alpha, Initial residual = 0.017891, Final residual = 8.03225e12, No Iterations 17 Dispersed phase volume fraction = 0.25 Min(alpha) = 0.0448055 Max(alpha) = 1.54693 GAMG: Solving for p, Initial residual = 0.879569, Final residual = 2.32629e+47, No Iterations 1000 time step continuity errors : sum local = 1.87375e+48, global = 1.79721e+45, cumulative = 1.79721e+45 GAMG: Solving for p, Initial residual = 0.826277, Final residual = 2.57506e+46, No Iterations 1000 time step continuity errors : sum local = 1.35281e+95, global = 1.29755e+92, cumulative = 1.29755e+92 #0 Foam::error:rintStack(Foam::Ostream&) in "/apps/OpenFOAM/OpenFOAM1.5/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/apps/OpenFOAM/OpenFOAM1.5/lib/linux64GccDPOpt/libOpenFOAM.so" #2 __restore_rt at sigaction.c:0 #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/apps/OpenFOAM/OpenFOAM1.5/lib/linux64GccDPOpt/libOpenFOAM.so" #4 Foam::fvMatrix<double>::solve(Foam::Istream&) in "/apps/OpenFOAM/OpenFOAM1.5/lib/linux64GccDPOpt/libfiniteVolume.so" #5 main in "/apps/OpenFOAM/OpenFOAM1.5/applications/bin/linux64GccDPOpt/twoPhaseEulerFoam" #6 __libc_start_main in "/lib64/libc.so.6" #7 Foam::regIOobject::readIfModified() in "/apps/OpenFOAM/OpenFOAM1.5/applications/bin/linux64GccDPOpt/twoPhaseEulerFoam" Floating exception $ As it can be seen the the error could be because of maximum courant number (also with timestep continuity error..) I made the following changes as compared to my laminar case . decreased velocity 100 times! (from 0.17cm/s to 0.17e2 cm/s) . also decreased timestep considerably . changed the default ddT schemes but none of these changes doesn't contribute for the stable simulation Am really wondering what could be the error that has occured by just switching on the turbulence...!! Regards Raghavendra 

March 17, 2009, 12:04 

#19 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
Hi,
this line should show you what you need to check:


March 17, 2009, 17:16 

#20 
Member

Hello Alberto,
There was some problem with nutb because of its very high value (1e+10) the simulation used to crash. To correct this I initialized very low value of epsilon (1e08..previous value was 0.1) and the simulation was quite stable for around 3 seconds and now the same problem .. Courant number suddenly increases from a value 0.0342002 at Time T=3.441seconds part of the log file is pasted below Courant Number mean: 0.00419636 max: 0.964209 Max Ur Courant Number = 1.17271 Calculating averages Time = 3.443 DILUPBiCG: Solving for alpha, Initial residual = 1.24005e05, Final residual = 1.12019e12, No Iterations 3 Dispersed phase volume fraction = 0.249998 Min(alpha) = 1.09456e25 Max(alpha) = 1.00728 DILUPBiCG: Solving for alpha, Initial residual = 1.45091e06, Final residual = 6.05932e11, No Iterations 2 Dispersed phase volume fraction = 0.249998 Min(alpha) = 1.09456e25 Max(alpha) = 1.00163 GAMG: Solving for p, Initial residual = 0.000133255, Final residual = 8.68084e09, No Iterations 47 time step continuity errors : sum local = 6.08486e06, global = 2.17887e06, cumulative = 7.01493e06 GAMG: Solving for p, Initial residual = 2.98824e12, Final residual = 2.98824e12, No Iterations 0 time step continuity errors : sum local = 0.000581419, global = 2.30176e06, cumulative = 9.31669e06 DILUPBiCG: Solving for epsilon, Initial residual = 1, Final residual = 7.62948e06, No Iterations 4 DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 7.48601e06, No Iterations 6 ExecutionTime = 1167.96 s ClockTime = 1172 s Courant Number mean: 0.0110784 max: 5.80792 Max Ur Courant Number = 16.9409 Calculating averages Time = 3.444 DILUPBiCG: Solving for alpha, Initial residual = 0.000897952, Final residual = 1.44798e11, No Iterations 7 Dispersed phase volume fraction = 0.250028 Min(alpha) = 1.4176e06 Max(alpha) = 1.52832 DILUPBiCG: Solving for alpha, Initial residual = 0.00051464, Final residual = 3.42879e12, No Iterations 6 Dispersed phase volume fraction = 0.249998 Min(alpha) = 1.08619e25 Max(alpha) = 1.18786 GAMG: Solving for p, Initial residual = 0.000202578, Final residual = 8.51716e09, No Iterations 7 time step continuity errors : sum local = 1.62171, global = 0.25112, cumulative = 0.251111 GAMG: Solving for p, Initial residual = 2.76714e08, Final residual = 8.22339e09, No Iterations 1 time step continuity errors : sum local = 0.540509, global = 0.169541, cumulative = 0.420652 #0 Foam::error:rintStack(Foam::Ostream&) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0xb7ff7400] #3 Foam:ILUPreconditioner::calcReciprocalD(Foam::Fi eld<double>&, Foam::lduMatrix const&) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #4 Foam:ILUPreconditioner:ILUPreconditioner(Foam: :lduMatrix::solver const&, Foam::Istream&) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #5 Foam::lduMatrix:reconditioner::addasymMatrixCons tructorToTable<Foam:ILUPreconditioner>::New(Foam ::lduMatrix::solver const&, Foam::Istream&) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #6 Foam::lduMatrix:reconditioner::New(Foam::lduMatr ix::solver const&, Foam::Istream&) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #7 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #8 Foam::fvMatrix<double>::solve(Foam::Istream&) in "/home/ragh/OpenFOAM/OpenFOAM1.5/lib/linuxGccDPOpt/libfiniteVolume.so" #9 Foam::fvMatrix<double>::solve() in "/home/ragh/OpenFOAM/OpenFOAM1.5/applications/bin/linuxGccDPOpt/twoPhaseEulerFoam" #10 main in "/home/ragh/OpenFOAM/OpenFOAM1.5/applications/bin/linuxGccDPOpt/twoPhaseEulerFoam" #11 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #12 Foam::regIOobject::readIfModified() in "/home/ragh/OpenFOAM/OpenFOAM1.5/applications/bin/linuxGccDPOpt/twoPhaseEulerFoam" Probably at this time the plume may just touche the interface at the top I started the simulation again from this time t = 3.44seconds by initializing k and epsilon again (don't know how far it will affect the accuracy of the result) but after few seconds again it crashes. When I checked the nutb variations in ParaFoam at the interface it creates problem with very high value (around 1e+9)... 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Burgerbs equation non constant Boundary Conditions Initial Conditions  arkangel  OpenFOAM Running, Solving & CFD  1  October 2, 2008 14:48 
Boundary conditions for turbulent boundary layer  Thomas  FLUENT  1  June 17, 2008 05:14 
boundary conditions for boundary layer flow  A. Alzoubi  CFX  0  November 3, 2007 08:11 
TwoPhaseEulerFoam and InletOutlet boundary condition  hemph  OpenFOAM Running, Solving & CFD  10  January 29, 2007 10:47 
Integral boundary conditions turbulent intensitylength boundary conditions  olesen  OpenFOAM Running, Solving & CFD  0  July 27, 2006 07:18 