[shipman]

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:

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 = 9.99915e-07, Final residual = 9.99915e-07, No Iterations 0
DILUPBiCG:  Solving for k, Initial residual = 5.42143e-06, Final residual = 4.10749e-09, No Iterations 1
bounding k, min: -4.49385e-05 max: 22.1434 average: 2.3799
GAMG:  Solving for p_rgh, Initial residual = 1.51332e-05, Final residual = 5.19543e-07, No Iterations 2
GAMG:  Solving for p_rgh, Initial residual = 3.39412e-06, Final residual = 1.34432e-07, No Iterations 2
time step continuity errors : sum local = 7.89858e-14, global = 3.22401e-17, cumulative = -3.74981e-09
GAMG:  Solving for p_rgh, Initial residual = 4.0231e-06, Final residual = 2.48069e-07, No Iterations 2
GAMGPCG:  Solving for p_rgh, Initial residual = 2.29577e-06, Final residual = 5.25898e-09, No Iterations 2
time step continuity errors : sum local = 3.09576e-15, global = 4.62557e-16, cumulative = -3.74981e-09
ExecutionTime = 83056 s  ClockTime = 84614 s

Courant Number mean: 0.00166374 max: 0.124553
deltaT = 6.84932e-08
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 = 9.99938e-07, Final residual = 9.99938e-07, No Iterations 0
DILUPBiCG:  Solving for k, Initial residual = 5.42105e-06, Final residual = 4.10607e-09, No Iterations 1
bounding k, min: -0.000342354 max: 22.1435 average: 2.37999
GAMG:  Solving for p_rgh, Initial residual = 1.49518e-05, Final residual = 4.91816e-07, No Iterations 2
GAMG:  Solving for p_rgh, Initial residual = 3.29783e-06, Final residual = 1.29053e-07, No Iterations 2
time step continuity errors : sum local = 7.58245e-14, global = -2.11585e-15, cumulative = -3.74981e-09
GAMG:  Solving for p_rgh, Initial residual = 3.97379e-06, Final residual = 2.48251e-07, No Iterations 2
GAMGPCG:  Solving for p_rgh, Initial residual = 2.30443e-06, Final residual = 5.2412e-09, No Iterations 2
time step continuity errors : sum local = 3.09174e-15, global = 4.74198e-16, cumulative = -3.74981e-09
ExecutionTime = 83057.9 s  ClockTime = 84616 s

Courant Number mean: 0.00166375 max: 0.124554
deltaT = 6.84932e-08
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 = 9.9996e-07, Final residual = 9.9996e-07, No Iterations 0
DILUPBiCG:  Solving for k, Initial residual = 5.42063e-06, Final residual = 4.10458e-09, No Iterations 1
bounding k, min: -1.78709e-06 max: 22.1436 average: 2.38007
GAMG:  Solving for p_rgh, Initial residual = 1.48559e-05, Final residual = 5.20918e-07, No Iterations 2
GAMG:  Solving for p_rgh, Initial residual = 3.37095e-06, Final residual = 1.34536e-07, No Iterations 2
time step continuity errors : sum local = 7.90403e-14, global = 6.42391e-17, cumulative = -3.74981e-09
GAMG:  Solving for p_rgh, Initial residual = 4.02349e-06, Final residual = 2.48081e-07, No Iterations 2
GAMGPCG:  Solving for p_rgh, Initial residual = 2.29573e-06, Final residual = 5.27016e-09, No Iterations 2
time step continuity errors : sum local = 3.11643e-15, global = 4.43929e-16, cumulative = -3.74981e-09
ExecutionTime = 83059.8 s  ClockTime = 84618 s

Courant Number mean: 0.00166376 max: 0.124555
deltaT = 6.84932e-08
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_64-linux-gnu/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_64-linux-gnu/libc.so.6"
[8] #10  
[8]  in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interPhaseChangeFoam"
[efs-desktop:15779] *** Process received signal ***
[efs-desktop:15779] Signal: Floating point exception (8)
[efs-desktop:15779] Signal code:  (-6)
[efs-desktop:15779] Failing at address: 0x3e800003da3
[efs-desktop:15779] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364c0) [0x7f9f72acb4c0]
[efs-desktop:15779] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7f9f72acb445]
[efs-desktop:15779] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364c0) [0x7f9f72acb4c0]
[efs-desktop:15779] [ 3] /opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam4sqrtERNS_5FieldIdEERKNS_5UListIdEE+0x30) [0x7f9f73c02de0]
[efs-desktop:15779] [ 4] interPhaseChangeFoam(_ZN4Foam4sqrtINS_12fvPatchFieldENS_7volMeshEEENS_3tmpINS_14GeometricFieldIdT_T0_EEEERKS8_+0x138) [0x4a7ec8]
[efs-desktop:15779] [ 5] interPhaseChangeFoam() [0x4a50b6]
[efs-desktop:15779] [ 6] interPhaseChangeFoam() [0x4a5d20]
[efs-desktop:15779] [ 7] interPhaseChangeFoam() [0x494918]
[efs-desktop:15779] [ 8] interPhaseChangeFoam() [0x434399]
[efs-desktop:15779] [ 9] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f9f72ab676d]
[efs-desktop:15779] [10] interPhaseChangeFoam() [0x436271]
[efs-desktop:15779] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 8 with PID 15779 on node efs-desktop exited on signal 8 (Floating point exception).

[shipman]

My mesh internal and concave mesh pictures..

[shipman]

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

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 zip-up check OK.
    Face-face 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 (non-closed singly connected)   (-0.006 -0.008 -2.71051e-20) (0.00194 0.007 0.00194)
    outlet              100      121      ok (non-closed singly connected)   (0 -0.008 0) (0.00194 -0.008 0.00194)
    inlet               400      451      ok (non-closed singly connected)   (-0.006 0.007 0) (0.00194 0.007 0.00194)

Checking geometry...
    Overall domain bounding box (-0.006 -0.008 -2.71051e-20) (0.00194 0.007 0.00194)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (2.22526e-14 -1.42534e-17 -2.50737e-15) OK.
    Max cell openness = 2.06795e-16 OK.
    Max aspect ratio = 2.5 OK.
    Minumum face area = 3.75e-11. Maximum face area = 1.6e-07.  Face area magnitudes OK.
    Min volume = 7.03125e-16. Max volume = 6.4e-11.  Total volume = 1.37934e-07.  Cell volumes OK.
    Mesh non-orthogonality Max: 29.0546 average: 10.3431
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.6129 OK.
    Coupled point location match (average 0) OK.
    Face tets OK.
    Min/max edge length = 5e-06 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.

[Artur]

Originally Posted by shipman

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

Normally when I get my simulations blowing up on continuity with interPhaseChangeFoam it's because of the alpha field source terms. It seems that for your case there is no cavitation at all (min alpha1 = 1) though.

Can you please tell us which mass transfer model you are using? What turbulence modelling do you adopt (from your log I'm guessing k-omega model but would be nice to have this confirmed).

Peace,

A

[shipman]

Dear Arthur,

Thanks so much for your answer. I am using SchneerSauer Transport model and as you guessed i am using k-omeggaSST 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...

[Artur]

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

[wyldckat]

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:

1. The kind "oh my goodness, how did the mesh generator allow this cell to be created" - usually are cells that almost look like beans or very contorted/squished beans. To get a visual idea, have a look at the image on this wikipedia article: http://en.wikipedia.org/wiki/Concave
2. The kind "why on Earth are you complaining about this cell?" - this one is usually generated by snappyHexMesh, where one face of a cell is divided into 2 parts and one of the 2 inner vertexes is a little tiny bit into the cell... which leads to the centres of the 2 faces on that side to be able to slightly see each other on the outside of the mesh, instead of being on the inside.

The first kind is can be a bit hard to fix, but decomposing/dividing that cell usually fixes the problem. Of course the problem is how to divide/decompose that cell. According to the User Guide: http://www.openfoam.org/docs/user/st...-utilities.php - the utility splitCells should do the trick, although I've never used it.

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:

    Overall domain bounding box (-0.006 -0.008 -2.71051e-20) (0.00194 0.007 0.00194)
[...]
    Min volume = 7.03125e-16. Max volume = 6.4e-11.  Total volume = 1.37934e-07.  Cell volumes OK.

• The smallest cell has got a volume of 7.0e-16 m³.
• The biggest one has got 6.4e-11 m³.
• The bounding box equates to approximately a box shaped as 0.008 x 0.011 x 0.0019 m³.

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 1e-4 to 1e-5 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.

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:

[8] #1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[8] #2   in "/lib/x86_64-linux-gnu/libc.so.6"
[8] #3  Foam::sqrt(Foam::Field<double>&, Foam::UList<double> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

A SIGFPE is explained at wikipedia: http://en.wikipedia.org/wiki/SIGFPE#SIGFPE - and the line below indicates which operation lead to a floating point error. For a square root to give such an error, it's very likely trying to find the square root of a negative number. For better or for worse, OpenFOAM doesn't handle flows in the imaginary/complex realm of mathematics, hence the crash.

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:

1. In one case the rho1 field might have a negative value;
2. On the other it might have an imbalance on this expression:
   

   mag(p - pSat()) + 0.01*pSat()

   In other words, if pSat is negative and the following occurs:
   

   mag(p - pSat()) < mag(0.01*pSat())

   then sqrt can crash, due to a negative value.

Without a more deeper inspection - possible by following the information provided here: http://openfoamwiki.net/index.php/HowTo_debugging - I'd say that this solver is not prepared to handle simulation domains so small as this one. Something similar was spotted sometime ago, as mentioned on this thread: http://www.cfd-online.com/Forums/ope...tml#post453034 post #16
Nonetheless, has a look into this post as well: http://www.cfd-online.com/Forums/ope...tml#post454869


Best regards,
Bruno

[shipman]

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 :

The bounding box equates to approximately a box shaped as 0.008 x 0.011 x 0.0019 m³.

Could you tell me what does it mean exactly??

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=18.7e-6, deltaT is set to =1e-7 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)

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 1e-4 to 1e-5 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.

4. Based on your following comment:

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.

what kind of special settings need to make for multiphase simulations??

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.

[wyldckat]

Hi shipman,

Originally Posted by shipman

1. you mentioned about the bounding box dimensions :

The bounding box equates to approximately a box shaped as 0.008 x 0.011 x 0.0019 m³.

Could you tell me what does it mean exactly??

This output from checkMesh:

Overall domain bounding box (-0.006 -0.008 -2.71051e-20) (0.00194 0.007 0.00194)

is telling you the left-bottommost points and the right-topmost points of the box inside which your mesh fits inside. If you subtract one position from the other, you get the length, width and height of the box. And the dimensions are in metre.

Originally Posted by shipman

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=18.7e-6, deltaT is set to =1e-7 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?

The problem is that it really depends on the the size of the cell where the flow is the quickest. You could have a very large cell with 1 m/s, but the Courant number be 0.1, while a very small cell with 0.0001 m/s could have a Courant number of 1.5.
There is an utility in OpenFOAM named Co which will calculate the field for the Courant number on all cells.

Originally Posted by shipman

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)

Essentially answered in #2.

Originally Posted by shipman

4. Based on your following comment:

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.

what kind of special settings need to make for multiphase simulations??

So many that I don't know all of them and it depends on a case-to-case basis. Which is why one should first test in serial/sequential mode (not parallel), to isolate the source of the problem... which implies that one should first test with a less complex case first, so that it runs faster in serial/sequential mode.

Originally Posted by shipman

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...

bubbleFoam? Mmm... seems like this solver no longer exists as of OpenFOAM 2.2, but it's still present in 2.1. You can find 3-4 tutorials on this topic, by running:

find $FOAM_TUTORIALS -name bubbleColumn

Because "bubbleColumn" was a tutorial for the bubbleFoam on OpenFOAM 2.1.

Originally Posted by shipman

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).

You can find a list on these wiki pages:

• Pre-processing section only: http://openfoamwiki.net/index.php/Ma...Pre-Processors
• GUI's in general, should already include mesh generators: http://openfoamwiki.net/index.php/GUI

Best regards,
Bruno

[shipman]

Thanks so much for your kind answers Bruno...

After check the your advices i will write you again.

[shipman]

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:

Max Ur Courant Number = 0.178827
DILUPBiCG:  Solving for alpha, Initial residual = 0.0146972, Final residual = 1.72969e-13, No Iterations 3
DILUPBiCG:  Solving for alpha, Initial residual = 4.24562e-05, Final residual = 2.94794e-12, 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 = 2.11395e-05, global = -5.68872e-07, cumulative = -4.94907e-05
DICPCG:  Solving for p, Initial residual = 0.195699, Final residual = 9.28547e-11, No Iterations 207
time step continuity errors : sum local = 8.24032e-10, global = 8.23939e-10, cumulative = -4.94899e-05
ExecutionTime = 127.44 s  ClockTime = 128 s

Courant Number mean: 0.0164668 max: 2.20072
Time = 3.6e-05

Max Ur Courant Number = 1.63354
DILUPBiCG:  Solving for alpha, Initial residual = 0.0407433, Final residual = 3.10458e-12, No Iterations 5
DILUPBiCG:  Solving for alpha, Initial residual = 0.00045346, Final residual = 9.07722e-13, 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 = -4.1366e-06, cumulative = -5.36264e-05
DICPCG:  Solving for p, Initial residual = 0.954797, Final residual = 8.72267e-11, No Iterations 462
time step continuity errors : sum local = 8.31059e-10, global = 8.23925e-10, cumulative = -5.36256e-05
ExecutionTime = 133.36 s  ClockTime = 134 s

Courant Number mean: 30.4657 max: 16654.1
Time = 3.7e-05

Max Ur Courant Number = 7309.4
DILUPBiCG:  Solving for alpha, Initial residual = 0.992949, Final residual = 9.77191e-11, No Iterations 25
DILUPBiCG:  Solving for alpha, Initial residual = 0.481133, Final residual = 2.49122e-12, 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 = 4.98582e-05, No Iterations 1001
time step continuity errors : sum local = 5.67408, global = 8.51898e-05, cumulative = 0.000198407
ExecutionTime = 144.96 s  ClockTime = 145 s

Courant Number mean: 720893 max: 1.88011e+08
Time = 3.8e-05

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 = 3.9e-05

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_64-linux-gnu/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_64-linux-gnu/libc.so.6"
#12  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/bubbleFoam"
Floating point exception (core dumped)

It says something floating points error about DILUP preconditioner but, i couldnt understand it well. also i set Fvsolver as follow; Could you help me how can i solve this problem.

solvers
{
    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-10;
        relTol          0.1;
    }

    pFinal
    {
        $p;
        tolerance       1e-10;
        relTol          0;
    }

    alpha
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-10;
        relTol          0.1;
    }

    alphaFinal
    {
        $alpha;
        tolerance       1e-10;
        relTol          0;
    }
   Ua
   {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }
   Ub
   {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }
   "(k|epsilon)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }

    "(k|epsilon)Final"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }
}

PIMPLE
{
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    nAlphaCorr      2;
    correctAlpha    no;
    pRefCell        0;
    pRefValue       0;
}

Thanks in advance

[shipman]

Also, I tried my case as laminar, but it gives same error as follow;

Max Ur Courant Number = 7309.4
DILUPBiCG:  Solving for alpha, Initial residual = 0.992949, Final residual = 9.77191e-11, No Iterations 25
DILUPBiCG:  Solving for alpha, Initial residual = 0.481133, Final residual = 2.49122e-12, 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 = 4.98582e-05, No Iterations 1001
time step continuity errors : sum local = 5.67408, global = 8.51898e-05, cumulative = 0.000198407
ExecutionTime = 141.22 s  ClockTime = 142 s

Courant Number mean: 720893 max: 1.88011e+08
Time = 3.8e-05

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 = 3.9e-05

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_64-linux-gnu/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_64-linux-gnu/libc.so.6"
#12  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/bubbleFoam"
Floating point exception (core dumped)

[shipman]

Dear Bruno,

I moved my question to this post. If you can answer i will be appreciated.

thanks in advance.

http://www.cfd-online.com/Forums/ope...imulation.html

and one additional question about the difference of HEM and VOF models...

http://www.cfd-online.com/Forums/ope...of-models.html

Thanks in advance.

[wyldckat]

Hi shipman,

Regarding the previous two posts, the issues seem to be:

• Using a fixed deltaT can lead to problems, if you don't know how to do the math. It's best to leave it to automatically calculate the necessary deltaT.
• The mesh cells seem very small. 1e-16 m3 is the smallest indicated by checkMesh, which implies that the deltaT is going to also have to be very small as well.

I'll have a look into the other two threads you've created.


Best regards,
Bruno

[shipman]

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(p-pSat())???

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.

[wyldckat]

Hi shipman,

Quoting from the header: https://github.com/OpenFOAM/OpenFOAM...SchnerrSauer.H

 SchnerrSauer cavitation model.

Reference:
\verbatim
Schnerr, G. H., And Sauer, J.,
"Physical and Numerical Modeling of Unsteady Cavitation Dynamics",
Proc. 4th International Conference on Multiphase Flow,
New Orleans, U.S.A., 2001.
\endverbatim

Therefore, part of the answer comes from there, namely as to why the magnitude function "mag" is used. This function basically calculates the absolute value. Probably it's because the pressure difference is what matters for the model.

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 equation-solving (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 equation-solving is how simpleFoam usually works.

Best regards,
Bruno

[shipman]

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.

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 equation-solving (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.

In interphasechangeFoam, I saw inside 0 file the p.rgh and When i checked the p.Eqn file, this pressure is calculated ==> p_rgh == p- rho*gh. So u mean that p_rgh is relative pressure in the InterPhaseChangeFoam??

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.cfd-online.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

[wyldckat]

Hi Baris,

Originally Posted by shipman

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...

Sometimes when there is a division by a value that could be zero, it's computationally cheaper to divide by a very small value, instead of using one or several "if" expression(s) to check the validity of the value.
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.

Originally Posted by shipman

On the other hand, based on the your following comment i couldnt understand what you mean exactly by saying relative pressure.

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 equation-solving (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.

[...]
Could you tell me reason why all pressures should be always (+) if absolute pressure is used?

Mmm... I see that you haven't studied enough about pressure and OpenFOAM's approach on how to handle it. The simple explanation is this:

• Relative pressure is when (for example) you subtract the atmospheric pressure to all pressure values in your domain, so that your relative pressure reference is "0" instead of "1 atm". This is used by many solvers in OpenFOAM, mostly incompressible ones. For example, have a look into the tutorials for simpleFoam and icoFoam.
  Note: in this example, the absolute reference pressure is "1 atm", but it could be anything else, depending on the environment being simulated.
• Absolute pressure is when all pressure values already include "1 atm". For example, if you wanted to simulate something at sea level, while also including 1km above and below, you use the absolute pressure, so that the pressure values range from something like 0.8 to 1.5 atm.

The really short version of this explanation:

• Relative pressure is when we use the initial value of 0 Pa and the pressure values can be negative.
• Absolute pressure is when all values must be positive. 0 Pa would mean that it was in perfect vacuum.

As I've mentioned before, it all depends on the solver you're using. The usual trick in OpenFOAM is to check what units the pressure fields are in:

• If the dimensions for the pressure field are defined as:
  

  dimensions      [0 2 -2 0 0 0 0];

  Then it's the relative pressure. More specifically, it's the "relative kinematic pressure", in the sense that this pressure only becomes the absolute pressure if you calculate:
  

  p*rho + p_atm

  Namely the current "relative kinematic pressure" times density plus "1 atm".
• If the dimensions for the pressure field are defined as:
  

  dimensions      [1 -1 -2 0 0 0 0];

  Then it's very likely to be absolute pressure.

Best regards,
Bruno

[shipman]

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.

[snak]

Hi, shipman,

Originally Posted by shipman

Dear Bruno,
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???

Absolute pressure is used only if the absolute pressure value is needed.
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.