
[Sponsors] 
January 23, 2014, 02:52 
InterPhaseChangeFoam ERROR

#1 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Dear Foam Users;
I am trying to simulate nozzle cavitation and using interphasechangeFoam. After starting the running after 1.5 days later i received following error. I checked the velocity fields, mass flow and turbulent energy distributions. All seems ok, i couldnt find any crazy fluctuation. Just before error i could the crazy value of the time step continuity errors. Could someone give to me any idea about this ERROR please Thanks in advance. ERROR: Code:
DILUPBiCG: Solving for alpha1, Initial residual = 0.60276, Final residual = 0.000145213, No Iterations 1 Liquid phase volume fraction = 1 Min(alpha1) = 1 Max(alpha1) = 1 DILUPBiCG: Solving for omega, Initial residual = 9.99915e07, Final residual = 9.99915e07, No Iterations 0 DILUPBiCG: Solving for k, Initial residual = 5.42143e06, Final residual = 4.10749e09, No Iterations 1 bounding k, min: 4.49385e05 max: 22.1434 average: 2.3799 GAMG: Solving for p_rgh, Initial residual = 1.51332e05, Final residual = 5.19543e07, No Iterations 2 GAMG: Solving for p_rgh, Initial residual = 3.39412e06, Final residual = 1.34432e07, No Iterations 2 time step continuity errors : sum local = 7.89858e14, global = 3.22401e17, cumulative = 3.74981e09 GAMG: Solving for p_rgh, Initial residual = 4.0231e06, Final residual = 2.48069e07, No Iterations 2 GAMGPCG: Solving for p_rgh, Initial residual = 2.29577e06, Final residual = 5.25898e09, No Iterations 2 time step continuity errors : sum local = 3.09576e15, global = 4.62557e16, cumulative = 3.74981e09 ExecutionTime = 83056 s ClockTime = 84614 s Courant Number mean: 0.00166374 max: 0.124553 deltaT = 6.84932e08 Time = 0.00477801 DILUPBiCG: Solving for alpha1, Initial residual = 0.604201, Final residual = 0.000592279, No Iterations 1 Liquid phase volume fraction = 1 Min(alpha1) = 1 Max(alpha1) = 1 DILUPBiCG: Solving for omega, Initial residual = 9.99938e07, Final residual = 9.99938e07, No Iterations 0 DILUPBiCG: Solving for k, Initial residual = 5.42105e06, Final residual = 4.10607e09, No Iterations 1 bounding k, min: 0.000342354 max: 22.1435 average: 2.37999 GAMG: Solving for p_rgh, Initial residual = 1.49518e05, Final residual = 4.91816e07, No Iterations 2 GAMG: Solving for p_rgh, Initial residual = 3.29783e06, Final residual = 1.29053e07, No Iterations 2 time step continuity errors : sum local = 7.58245e14, global = 2.11585e15, cumulative = 3.74981e09 GAMG: Solving for p_rgh, Initial residual = 3.97379e06, Final residual = 2.48251e07, No Iterations 2 GAMGPCG: Solving for p_rgh, Initial residual = 2.30443e06, Final residual = 5.2412e09, No Iterations 2 time step continuity errors : sum local = 3.09174e15, global = 4.74198e16, cumulative = 3.74981e09 ExecutionTime = 83057.9 s ClockTime = 84616 s Courant Number mean: 0.00166375 max: 0.124554 deltaT = 6.84932e08 Time = 0.00477808 DILUPBiCG: Solving for alpha1, Initial residual = 0.595926, Final residual = 0.000665285, No Iterations 1 Liquid phase volume fraction = 1 Min(alpha1) = 1 Max(alpha1) = 1 DILUPBiCG: Solving for omega, Initial residual = 9.9996e07, Final residual = 9.9996e07, No Iterations 0 DILUPBiCG: Solving for k, Initial residual = 5.42063e06, Final residual = 4.10458e09, No Iterations 1 bounding k, min: 1.78709e06 max: 22.1436 average: 2.38007 GAMG: Solving for p_rgh, Initial residual = 1.48559e05, Final residual = 5.20918e07, No Iterations 2 GAMG: Solving for p_rgh, Initial residual = 3.37095e06, Final residual = 1.34536e07, No Iterations 2 time step continuity errors : sum local = 7.90403e14, global = 6.42391e17, cumulative = 3.74981e09 GAMG: Solving for p_rgh, Initial residual = 4.02349e06, Final residual = 2.48081e07, No Iterations 2 GAMGPCG: Solving for p_rgh, Initial residual = 2.29573e06, Final residual = 5.27016e09, No Iterations 2 time step continuity errors : sum local = 3.11643e15, global = 4.43929e16, cumulative = 3.74981e09 ExecutionTime = 83059.8 s ClockTime = 84618 s Courant Number mean: 0.00166376 max: 0.124555 deltaT = 6.84932e08 Time = 0.00477815 [8] #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [8] #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [8] #2 in "/lib/x86_64linuxgnu/libc.so.6" [8] #3 Foam::sqrt(Foam::Field<double>&, Foam::UList<double> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [8] #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::sqrt<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interPhaseChangeFoam" [8] #5 [8] in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interPhaseChangeFoam" [8] #6 [8] in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interPhaseChangeFoam" [8] #7 [8] in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interPhaseChangeFoam" [8] #8 [8] in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interPhaseChangeFoam" [8] #9 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" [8] #10 [8] in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interPhaseChangeFoam" [efsdesktop:15779] *** Process received signal *** [efsdesktop:15779] Signal: Floating point exception (8) [efsdesktop:15779] Signal code: (6) [efsdesktop:15779] Failing at address: 0x3e800003da3 [efsdesktop:15779] [ 0] /lib/x86_64linuxgnu/libc.so.6(+0x364c0) [0x7f9f72acb4c0] [efsdesktop:15779] [ 1] /lib/x86_64linuxgnu/libc.so.6(gsignal+0x35) [0x7f9f72acb445] [efsdesktop:15779] [ 2] /lib/x86_64linuxgnu/libc.so.6(+0x364c0) [0x7f9f72acb4c0] [efsdesktop:15779] [ 3] /opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam4sqrtERNS_5FieldIdEERKNS_5UListIdEE+0x30) [0x7f9f73c02de0] [efsdesktop:15779] [ 4] interPhaseChangeFoam(_ZN4Foam4sqrtINS_12fvPatchFieldENS_7volMeshEEENS_3tmpINS_14GeometricFieldIdT_T0_EEEERKS8_+0x138) [0x4a7ec8] [efsdesktop:15779] [ 5] interPhaseChangeFoam() [0x4a50b6] [efsdesktop:15779] [ 6] interPhaseChangeFoam() [0x4a5d20] [efsdesktop:15779] [ 7] interPhaseChangeFoam() [0x494918] [efsdesktop:15779] [ 8] interPhaseChangeFoam() [0x434399] [efsdesktop:15779] [ 9] /lib/x86_64linuxgnu/libc.so.6(__libc_start_main+0xed) [0x7f9f72ab676d] [efsdesktop:15779] [10] interPhaseChangeFoam() [0x436271] [efsdesktop:15779] *** End of error message ***  mpirun noticed that process rank 8 with PID 15779 on node efsdesktop exited on signal 8 (Floating point exception). 

January 23, 2014, 04:20 
hi

#2 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
My mesh internal and concave mesh pictures..


January 23, 2014, 05:22 
Hi

#3 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
When i check the quality of my mesh gives following error about concave mesh...Is there anyone who can advice to me how can i correct this error? And is this error really important or ignorable?
Thanks... mesh check: checkMesh allTopology allGeometry Code:
Mesh stats points: 654382 faces: 1596014 internal faces: 1412748 cells: 471322 boundary patches: 3 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 410213 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 61109 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Topological cell zipup check OK. Faceface connectivity OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology Bounding box wall 182766 183793 ok (nonclosed singly connected) (0.006 0.008 2.71051e20) (0.00194 0.007 0.00194) outlet 100 121 ok (nonclosed singly connected) (0 0.008 0) (0.00194 0.008 0.00194) inlet 400 451 ok (nonclosed singly connected) (0.006 0.007 0) (0.00194 0.007 0.00194) Checking geometry... Overall domain bounding box (0.006 0.008 2.71051e20) (0.00194 0.007 0.00194) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (2.22526e14 1.42534e17 2.50737e15) OK. Max cell openness = 2.06795e16 OK. Max aspect ratio = 2.5 OK. Minumum face area = 3.75e11. Maximum face area = 1.6e07. Face area magnitudes OK. Min volume = 7.03125e16. Max volume = 6.4e11. Total volume = 1.37934e07. Cell volumes OK. Mesh nonorthogonality Max: 29.0546 average: 10.3431 Nonorthogonality check OK. Face pyramids OK. Max skewness = 1.6129 OK. Coupled point location match (average 0) OK. Face tets OK. Min/max edge length = 5e06 0.0004 OK. All angles in faces OK. Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 1 All face flatness OK. Cell determinant (wellposedness) : minimum: 0.821136 average: 13.565 Cell determinant check OK. ***Concave cells (using face planes) found, number of cells: 58628 <<Writing 58628 concave cells to set concaveCells Failed 1 mesh checks. 

January 23, 2014, 05:30 

#4  
Senior Member
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 268
Rep Power: 7 
Quote:
Can you please tell us which mass transfer model you are using? What turbulence modelling do you adopt (from your log I'm guessing komega model but would be nice to have this confirmed). Peace, A 

January 23, 2014, 05:36 
hi

#5 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Dear Arthur,
Thanks so much for your answer. I am using SchneerSauer Transport model and as you guessed i am using komeggaSST turbulence model. Actually, when i checked and compared final my mass flow rate with experimental data still it shows no cavitation formation. In addition, what you think about the my checkmesh error for the concaveCells. Do you think that is it important error? Thanks... 

January 23, 2014, 05:47 

#6 
Senior Member
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 268
Rep Power: 7 
Well, mesh check errors are generally detrimental when it comes to the solution quality, especially when problems occur early on in the continuity equation (which is what I think is going on in this case from looking at your log). Your geometry looks simple enough to be meshed with blockMesh without too much trouble I think so perhaps that's one way to factor one thing out.
A 

January 24, 2014, 19:58 

#7 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,531
Blog Entries: 36
Rep Power: 97 
Greetings to all!
I'll start by commenting on the concave cells topic. From my experience, there are 2 kinds of concave cells that checkMesh will complain about, then doing a full diagnostic:
As for the second kind... er... ignore and carry on Side note: when visualizing the concave cells, make sure to use the polyhedron option (aka to not decompose polyhedral cells). Onward to the next topic: the crash by interPhaseChangeFoam. I've never used this solver in any practical sense, so I have no idea of how to diagnose it's operation. Nonetheless, I do have some experience with Courant Number based solvers. The key detail usually is: if you have very smalls cells, then you're asking for a veeery slow simulation. In this case, checkMesh is reporting these critical details: Code:
Overall domain bounding box (0.006 0.008 2.71051e20) (0.00194 0.007 0.00194) [...] Min volume = 7.03125e16. Max volume = 6.4e11. Total volume = 1.37934e07. Cell volumes OK.
Therefore, the first step would be to ascertain if the meshed domain has got the correct size. The error output seems to imply that the simulation is running in parallel. This is a very important detail, since multiphase simulations in parallel tend to need special settings. In addition, the stack trace is indicating a very important detail: Code:
[8] #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [8] #2 in "/lib/x86_64linuxgnu/libc.so.6" [8] #3 Foam::sqrt(Foam::Field<double>&, Foam::UList<double> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" Taking a look into the source code for this solver, namely at "applications/solvers/multiphase/interPhaseChangeFoam"  the problem might be in this method: https://github.com/OpenFOAM/OpenFOAM...errSauer.C#L94 There are 2 sqrt calls in this method:
Nonetheless, has a look into this post as well: interFoam  validation for bubble/droplet flows in microfluidics Best regards, Bruno
__________________
I'll be at OFW11 in Portugal 

January 26, 2014, 04:28 
hi

#8 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Dear Bruno,
Firstly, Thanks so much for your detailed information. I am really appreciated Since i am the new OF user, I read all of the threads and your comments. these information are very useful even some of them are very difficult for me to understand at this stage. Therefore, I have some questions; 1. you mentioned about the bounding box dimensions : HTML Code:
The bounding box equates to approximately a box shaped as 0.008 x 0.011 x 0.0019 m³. 2. Actually i didnt do any example about Courant number based solvers. Just i calculate the it based on this equation: Co= deltaT*U/min.Cell.Dimension ==> my min cell is=18.7e6, deltaT is set to =1e7 and U is = 3.1 m/s ==> Therefore Co uquals very small value as 0.0017. Could you give me some advice to set the Co number? 3. On the other hand could you give a bit more details about your following explanations; how did you estimate the flow speeds should not be faster than 1e4... (I want to know how can i ascertain the correct size of the mesh) HTML Code:
I'm not in the mood to do any Courant Number related math right now, but I'm estimating that the flow speeds should not be faster than 1e4 to 1e5 m/s, otherwise the simulation is going to be slooooow... Therefore, the first step would be to ascertain if the meshed domain has got the correct size. HTML Code:
The error output seems to imply that the simulation is running in parallel. This is a very important detail, since multiphase simulations in parallel tend to need special settings. 5. After your explanations, i agree with you that this solver is not fit to make cavitation simulation inside of nozzle. Truely speaking, i am studying bubble dynamics which are very important to determine the bubble growth and collapse during cavitation phenomena. I choosed Schneer model bcs it includes bubble dynamics model (Rayleigh method was used) and i thought that i can insert my extended bubble dynamics model instead of this. Now, I am a bit confused that which solver is more convenient for me to make nozzle cavitation simulation based on bubble dynamics??If you can give me some advice will be very happy... 6. Final question is about the mesh creator programs. I talked with my prof. and he said that he could supply for me a mesh creator program which can work compatible with OPENFOAM. Therefore, could you give advice about some commercial or free mesh creator programs (which are not very difficult to create mesh). If you can have time to reply me, i will be so appreciated. Thanks so much Bruno. (Indeed, at the beginning, i was so pessimistic about using of OF, but after started to learn step by step feel better..) Thanks in advance. 

January 26, 2014, 08:09 

#9  
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,531
Blog Entries: 36
Rep Power: 97 
Hi shipman,
Quote:
Code:
Overall domain bounding box (0.006 0.008 2.71051e20) (0.00194 0.007 0.00194) Quote:
There is an utility in OpenFOAM named Co which will calculate the field for the Courant number on all cells. Quote:
Quote:
Quote:
Code:
find $FOAM_TUTORIALS name bubbleColumn Quote:
Bruno
__________________
I'll be at OFW11 in Portugal Last edited by wyldckat; February 16, 2014 at 14:21. Reason: changed name "George" to "shipman"... I must have confused the names... 

January 26, 2014, 22:02 
Hi

#10 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Thanks so much for your kind answers Bruno...
After check the your advices i will write you again. 

February 9, 2014, 23:35 

#11 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Dear Bruno,
After your suggestion, I started to try the bubblefoam for my nozzle cavitation simulation. However, i couldnt succeed yet. Always, Co number reaches a crazy value after some iteration later and gives following error: Code:
Max Ur Courant Number = 0.178827 DILUPBiCG: Solving for alpha, Initial residual = 0.0146972, Final residual = 1.72969e13, No Iterations 3 DILUPBiCG: Solving for alpha, Initial residual = 4.24562e05, Final residual = 2.94794e12, No Iterations 2 Dispersed phase volume fraction = 0.000173122 Min(alpha) = 0.208749 Max(alpha) = 1 DICPCG: Solving for p, Initial residual = 0.430025, Final residual = 0.0327875, No Iterations 3 time step continuity errors : sum local = 2.11395e05, global = 5.68872e07, cumulative = 4.94907e05 DICPCG: Solving for p, Initial residual = 0.195699, Final residual = 9.28547e11, No Iterations 207 time step continuity errors : sum local = 8.24032e10, global = 8.23939e10, cumulative = 4.94899e05 ExecutionTime = 127.44 s ClockTime = 128 s Courant Number mean: 0.0164668 max: 2.20072 Time = 3.6e05 Max Ur Courant Number = 1.63354 DILUPBiCG: Solving for alpha, Initial residual = 0.0407433, Final residual = 3.10458e12, No Iterations 5 DILUPBiCG: Solving for alpha, Initial residual = 0.00045346, Final residual = 9.07722e13, No Iterations 4 Dispersed phase volume fraction = 0.000173123 Min(alpha) = 0.228074 Max(alpha) = 1 DICPCG: Solving for p, Initial residual = 0.896893, Final residual = 0.0850594, No Iterations 99 time step continuity errors : sum local = 0.00040694, global = 4.1366e06, cumulative = 5.36264e05 DICPCG: Solving for p, Initial residual = 0.954797, Final residual = 8.72267e11, No Iterations 462 time step continuity errors : sum local = 8.31059e10, global = 8.23925e10, cumulative = 5.36256e05 ExecutionTime = 133.36 s ClockTime = 134 s Courant Number mean: 30.4657 max: 16654.1 Time = 3.7e05 Max Ur Courant Number = 7309.4 DILUPBiCG: Solving for alpha, Initial residual = 0.992949, Final residual = 9.77191e11, No Iterations 25 DILUPBiCG: Solving for alpha, Initial residual = 0.481133, Final residual = 2.49122e12, No Iterations 26 Dispersed phase volume fraction = 0.000173124 Min(alpha) = 0.244426 Max(alpha) = 1 DICPCG: Solving for p, Initial residual = 0.964588, Final residual = 0.0810355, No Iterations 377 time step continuity errors : sum local = 4.64573, global = 0.000166842, cumulative = 0.000113217 DICPCG: Solving for p, Initial residual = 0.999336, Final residual = 4.98582e05, No Iterations 1001 time step continuity errors : sum local = 5.67408, global = 8.51898e05, cumulative = 0.000198407 ExecutionTime = 144.96 s ClockTime = 145 s Courant Number mean: 720893 max: 1.88011e+08 Time = 3.8e05 Max Ur Courant Number = 1.40578e+08 DILUPBiCG: Solving for alpha, Initial residual = 0.999967, Final residual = 0.134631, No Iterations 1001 DILUPBiCG: Solving for alpha, Initial residual = 0.98207, Final residual = 0.0979581, No Iterations 1001 Dispersed phase volume fraction = 326297 Min(alpha) = 2.51536e+13 Max(alpha) = 1.66226e+13 DICPCG: Solving for p, Initial residual = 0.999969, Final residual = 526.487, No Iterations 1001 time step continuity errors : sum local = 2.2233e+11, global = 7058.54, cumulative = 7058.54 DICPCG: Solving for p, Initial residual = 0.958766, Final residual = 4.5949, No Iterations 1001 time step continuity errors : sum local = 6.79927e+13, global = 5.53265e+07, cumulative = 5.53194e+07 ExecutionTime = 190.36 s ClockTime = 191 s Courant Number mean: 9.57491e+13 max: 5.34135e+19 Time = 3.9e05 Max Ur Courant Number = 4.99329e+19 #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::DILUPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam::DILUPreconditioner::DILUPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 Foam::lduMatrix::preconditioner::addasymMatrixConstructorToTable<Foam::DILUPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #6 Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #7 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #8 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #9 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/bubbleFoam" #10 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/bubbleFoam" #11 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #12 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/bubbleFoam" Floating point exception (core dumped) Code:
solvers { p { solver PCG; preconditioner DIC; tolerance 1e10; relTol 0.1; } pFinal { $p; tolerance 1e10; relTol 0; } alpha { solver PBiCG; preconditioner DILU; tolerance 1e10; relTol 0.1; } alphaFinal { $alpha; tolerance 1e10; relTol 0; } Ua { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } Ub { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } "(kepsilon)" { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } "(kepsilon)Final" { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } } PIMPLE { nCorrectors 2; nNonOrthogonalCorrectors 0; nAlphaCorr 2; correctAlpha no; pRefCell 0; pRefValue 0; } Last edited by wyldckat; February 16, 2014 at 14:17. Reason: [QUOTE] > [CODE] 

February 9, 2014, 23:44 

#12 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Also, I tried my case as laminar, but it gives same error as follow;
Code:
Max Ur Courant Number = 7309.4 DILUPBiCG: Solving for alpha, Initial residual = 0.992949, Final residual = 9.77191e11, No Iterations 25 DILUPBiCG: Solving for alpha, Initial residual = 0.481133, Final residual = 2.49122e12, No Iterations 26 Dispersed phase volume fraction = 0.000173124 Min(alpha) = 0.244426 Max(alpha) = 1 DICPCG: Solving for p, Initial residual = 0.964588, Final residual = 0.0810355, No Iterations 377 time step continuity errors : sum local = 4.64573, global = 0.000166842, cumulative = 0.000113217 DICPCG: Solving for p, Initial residual = 0.999336, Final residual = 4.98582e05, No Iterations 1001 time step continuity errors : sum local = 5.67408, global = 8.51898e05, cumulative = 0.000198407 ExecutionTime = 141.22 s ClockTime = 142 s Courant Number mean: 720893 max: 1.88011e+08 Time = 3.8e05 Max Ur Courant Number = 1.40578e+08 DILUPBiCG: Solving for alpha, Initial residual = 0.999967, Final residual = 0.134631, No Iterations 1001 DILUPBiCG: Solving for alpha, Initial residual = 0.98207, Final residual = 0.0979581, No Iterations 1001 Dispersed phase volume fraction = 326297 Min(alpha) = 2.51536e+13 Max(alpha) = 1.66226e+13 DICPCG: Solving for p, Initial residual = 0.999969, Final residual = 526.487, No Iterations 1001 time step continuity errors : sum local = 2.2233e+11, global = 7058.54, cumulative = 7058.54 DICPCG: Solving for p, Initial residual = 0.958766, Final residual = 4.5949, No Iterations 1001 time step continuity errors : sum local = 6.79927e+13, global = 5.53265e+07, cumulative = 5.53194e+07 ExecutionTime = 186.03 s ClockTime = 186 s Courant Number mean: 9.57491e+13 max: 5.34135e+19 Time = 3.9e05 Max Ur Courant Number = 4.99329e+19 #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::DILUPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam::DILUPreconditioner::DILUPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 Foam::lduMatrix::preconditioner::addasymMatrixConstructorToTable<Foam::DILUPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #6 Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #7 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #8 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #9 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/bubbleFoam" #10 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/bubbleFoam" #11 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #12 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/bubbleFoam" Floating point exception (core dumped) Last edited by wyldckat; February 16, 2014 at 14:19. Reason: [QUOTE] > [CODE] 

February 12, 2014, 19:30 

#13 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Dear Bruno,
I moved my question to this post. If you can answer i will be appreciated. thanks in advance. http://www.cfdonline.com/Forums/ope...imulation.html and one additional question about the difference of HEM and VOF models... Difference of definition between HEM and VOF models Thanks in advance. 

February 16, 2014, 14:25 

#14 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,531
Blog Entries: 36
Rep Power: 97 
Hi shipman,
Regarding the previous two posts, the issues seem to be:
Best regards, Bruno
__________________
I'll be at OFW11 in Portugal 

February 22, 2014, 01:57 

#15 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Dear Bruno,
Thanks for your kind answer. I read my this post again with your comments i have one question which made me confused: above at #7 comment of you: On the other it might have an imbalance on this expression: Code: mag(p  pSat()) + 0.01*pSat() 1. what is the meaning of mag exactly? what kind of mathematical function it makes for this: mag(ppSat())??? 2. even if Psat < 0 how can this can occur acc. to your comment? In other words, if pSat is negative and the following occurs: Code: mag(p  pSat()) < mag(0.01*pSat()) then sqrt can crash, due to a negative value. if the psat becomes negatif how this form mag(p  pSat()) < mag(0.01*pSat()) can be neg? i really dint understand? Could you let me know please? one more thing: why did programmer not use absolute command inside of the sqrt to avoid the floating point error? do u have any idea? thanks in advaance. 

February 22, 2014, 06:43 

#16  
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,531
Blog Entries: 36
Rep Power: 97 
Hi shipman,
Quoting from the header: https://github.com/OpenFOAM/OpenFOAM...SchnerrSauer.H Quote:
As for "pSat" being negative: I forgot that both "p" and "pSat" might be both zero, hence the division by zero is what might be causing the crash. As for the possibility of "pSat" being negative: I'm not familiar with this model nor solver, but I suspect that both should not be used with incompressible equationsolving (I can't remember the accurate name for this), which sometimes uses relative pressure instead of absolute pressure (i.e. relative to a reference; and absolute as it already includes the reference pressure). In other words, if absolute pressure is used, then all pressures should always be positive. Note: What I meant by incompressible equationsolving is how simpleFoam usually works. Best regards, Bruno
__________________
I'll be at OFW11 in Portugal 

February 23, 2014, 13:00 
hi

#17 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Hi Bruno,
Firstly, Thanks so much for your reply. As far as i understood from your answer that if mag function calculates the absolute value which means that this term mag(p  pSat()) is always positive than i found that the reason of floating point error (shown above at #1) is term 0.01*pSat. Because, I checked setting again and saw that i set pSat as 23000Pa for this calculation and it gives floatin error. And, also I checked the forum and original paper of model again but i couldnt find any reason why this term 0.01*pSat is used in the equation... On the other hand, based on the your following comment i couldnt understand what you mean exactly by saying relative pressure. HTML Code:
As for the possibility of "pSat" being negative: I'm not familiar with this model nor solver, but I suspect that both should not be used with incompressible equationsolving (I can't remember the accurate name for this), which sometimes uses relative pressure instead of absolute pressure (i.e. relative to a reference; and absolute as it already includes the reference pressure). In other words, if absolute pressure is used, then all pressures should always be positive. And also When i checked the my result in interphasechangefoam, I found out that pressure never become negatif if i set the pSat as pozitif. So, I think that you are right about this comment: In other words, if absolute pressure is used, then all pressures should always be positive. Could you tell me reason why all pressures should be always (+) if absolute pressure is used? Because, I also checked the result of pressure by using interFoam (instead of interphasechageFoam) I saw that pressure drops below zero and become negatif. But in interphasechangefoam (if the pSat >0 ) never drops below zero.(or if pSat<0, as you know it gives floating point error) And also, in my previous post http://www.cfdonline.com/Forums/ope...foam_help.html about the disaappearing of the cavitation region i found out that although mass flow is increasing, cavitation region disappears due to pressure increases. Do you think that this problem is related with your explanation??? Thanks in advance for your kind support Bruno. If you let me know the reason, I think that i will be able to understand my general problem in interphasechangefoam. Best regards. Baris 

February 23, 2014, 15:18 

#18  
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,531
Blog Entries: 36
Rep Power: 97 
Hi Baris,
Quote:
In this case, instead of using a "VERY_SMALL" value, they might have chosen to use "0.01*pSat", since it keeps values within an acceptable operating region. Quote:
Bruno
__________________
I'll be at OFW11 in Portugal 

February 24, 2014, 02:10 

#19 
Senior Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 129
Rep Power: 5 
Dear Bruno,
Thanks so much for very valuable information for me. After your reply, also read many posts about the reference and absolute pressures. could you tell me i am right or not: 1. My conclusion is that in incompressible solvers (like simple, ico ,pisofoams..) reference pressure is used because only the pressure gradient is relevant for such flows. Hence the absolute value of pressure is absolutely unimportant. 2.However, i am a bit confused now about the interphasechageFoam which is also incompressible solver but it uses absolute pressure instead of reference value ....could you give me some insight about it? The reason is its multiphase flow??? Thanks in advance. 

February 24, 2014, 04:48 

#20  
Member
shinji nakagawa
Join Date: Mar 2009
Location: Japan
Posts: 31
Rep Power: 9 
Hi, shipman,
Quote:
In interPhaseChangeFoam, you need the saturation vapour pressure pSat. pSat is expressed in the absolute pressure. This is the reason why interPhaseChangeFoam use the absolute pressure. In interFoam, nothing depends on the absolute pressure because the physical properties in the solver is constant. There is no need to use the absolute pressure. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh  gschaider  OpenFOAM  300  October 29, 2014 19:00 
c++ libraries and solver compiling  vaina74  OpenFOAM Installation  13  February 3, 2012 18:43 
Saving ParaFoam views and case  sail  OpenFOAM Paraview & paraFoam  9  November 25, 2011 16:46 
DecomposePar links against liblamso0 with OpenMPI  jens_klostermann  OpenFOAM Bugs  11  June 28, 2007 17:51 
user defined function  cfduser  CFX  0  April 29, 2006 10:58 