CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   OpenFOAM remote cluster run error (https://www.cfd-online.com/Forums/openfoam-solving/154888-openfoam-remote-cluster-run-error.html)

krishtej23 June 21, 2015 19:29
OpenFOAM remote cluster run error
 
Hi,

I am trying to run multiphaseInterFoam in remote cluster in parallel. I getting this error which I couldn't understand:

Code:
[1] #0  Foam::error::printStack(Foam::Ostream&) in "/users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #1  Foam::sigFpe::sigHandler(int) in "/users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #2  ? in "/lib64/libc.so.6"
[1] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libmultiphaseInterFoam.so"
[1] #5  Foam::multiphaseMixture::multiphaseMixture(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libmultiphaseInterFoam.so"
[1] #6  ? in "/users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/bin/multiphaseInterFoam"
[1] #7  __libc_start_main in "/lib64/libc.so.6"
[1] #8  ? in "/users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/bin/multiphaseInterFoam"
[compute-01-29:29153] *** Process received signal ***
[compute-01-29:29153] Signal: Floating point exception (8)
[compute-01-29:29153] Signal code:  (-6)
[compute-01-29:29153] Failing at address: 0x2ef9000071e1
[compute-01-29:29153] [ 0] /lib64/libc.so.6[0x357f8326a0]
[compute-01-29:29153] [ 1] /lib64/libc.so.6(gsignal+0x35)[0x357f832625]
[compute-01-29:29153] [ 2] /lib64/libc.so.6[0x357f8326a0]
[compute-01-29:29153] [ 3] /users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKNS_5UListIdEES6_+0x125)[0x7f21eb89fec5]
[compute-01-29:29153] [ 4] /users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libmultiphaseInterFoam.so(_ZN4FoamdvINS_12fvPatchFieldENS_7volMeshEEENS_3tmpINS_14GeometricFieldIdT_T0_EEEERKS8_SA_+0x1ef)[0x7f21ef1bcadf]
[compute-01-29:29153] [ 5] /users/krmedam/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libmultiphaseInterFoam.so(_ZN4Foam17multiphaseMixtureC2ERKNS_14GeometricFieldINS_6VectorIdEENS_12fvPatchFieldENS_7volMeshEEERKNS1_IdNS_13fvsPatchFieldENS_11surfaceMeshEEE+0x5a3)[0x7f21ef198703]
[compute-01-29:29153] [ 6] multiphaseInterFoam[0x4672ba]
[compute-01-29:29153] [ 7] /lib64/libc.so.6(__libc_start_main+0xfd)[0x357f81ed5d]
[compute-01-29:29153] [ 8] multiphaseInterFoam[0x4251e9]
[compute-01-29:29153] *** End of error message ***
Please help me in this issue. Eagerly awaiting a reply.

Thanks in advance.

Regards,
Krishna.

Saideep June 22, 2015 06:19
Hi Krish;

I guess there is no problem running the case on the cluster but i guess there is some sort of problem with the code.

Maybe you edited the code and compiled it successfully however at some point while running the code you are hitting some function where you could be dividing with 0 thereby causing this error.

Maybe, the easiest way to start is just try a simple case without modification and it should work perfectly and later edit the code stepwise.

Hope this was useful;
Saideep

krishtej23 June 22, 2015 10:25
Quote:
Originally Posted by Saideep (Post 551497)
Hi Krish;

I guess there is no problem running the case on the cluster but i guess there is some sort of problem with the code.

Maybe you edited the code and compiled it successfully however at some point while running the code you are hitting some function where you could be dividing with 0 thereby causing this error.

Maybe, the easiest way to start is just try a simple case without modification and it should work perfectly and later edit the code stepwise.

Hope this was useful;
Saideep
Hi Saideep,

Thanks for the reply.

I didn't messup anything with the functions of multiphaseInterFoam.

Sure, I'l try your suggestion and get back to you.

Thank you,
Krishna.

alexeym June 22, 2015 10:39
Hi,

If we try to decipher the error message:

1. Error happened in multiphaseMixture::multiphaseMixture
2. The error was FPE, and it happened during division.

Let us check division operations in multiphaseMixture constructor:

Code:
...
nu_
( 
...
    mu()/rho()
),
...
deltaN_
(
    "deltaN",
    1e-8/pow(average(mesh_.V()), 1.0/3.0)
)
...
So you problem can be caused by

1. zero average density
2. zero mesh volume (yet in this case, I think, the error would be in pow function not in division operator)

Provide checkMesh output, check you initial conditions.

krishtej23 June 28, 2015 14:12
1 Attachment(s)
Quote:
Originally Posted by alexeym (Post 551551)
Hi,

If we try to decipher the error message:

1. Error happened in multiphaseMixture::multiphaseMixture
2. The error was FPE, and it happened during division.

Let us check division operations in multiphaseMixture constructor:

Code:
...
nu_
( 
...
    mu()/rho()
),
...
deltaN_
(
    "deltaN",
    1e-8/pow(average(mesh_.V()), 1.0/3.0)
)
...
So you problem can be caused by

1. zero average density
2. zero mesh volume (yet in this case, I think, the error would be in pow function not in division operator)

Provide checkMesh output, check you initial conditions.
Hi Alex,

Thank you for the reply and sorry for the delay in response.
I did check the output for checkMesh and everything says ok. Here is the output from checkMesh:
Code:
/*---------------------------------------------------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.4.0                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
Build  : 2.4.0-dcea1e13ff76
Exec  : checkMesh
Date  : Jun 28 2015
Time  : 14:00:25
Host  : "compute-01-30"
PID    : 17295
Case  : /auto/scratch/krmedam/drop3b_3phase_test
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:          37761
    faces:            109700
    internal faces:  106300
    cells:            36000
    faces per cell:  6
    boundary patches: 3
    point zones:      0
    face zones:      0
    cell zones:      0

Overall number of cells of each type:
    hexahedra:    36000
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:    0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch              Faces    Points  Surface topology                 
    bottom              900      921      ok (non-closed singly connected) 
    atmosphere          900      921      ok (non-closed singly connected) 
    walls              1600    1640    ok (non-closed singly connected) 

Checking geometry...
    Overall domain bounding box (-0.01542 0 -0.01542) (0.01542 0.018 0.01542)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-1.50786e-17 -9.98796e-16 1.97989e-17) OK.
    Max cell openness = 2.13078e-16 OK.
    Max aspect ratio = 27.0443 OK.
    Minimum face area = 1.22963e-08. Maximum face area = 3.37664e-06.  Face area magnitudes OK.
    Min volume = 2.16696e-12. Max volume = 2.38919e-09.  Total volume = 1.33907e-05.  Cell volumes OK.
    Mesh non-orthogonality Max: 33.0423 average: 4.55378
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.623086 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End
I also attached the case files and total output from the run in the zip file. Please have a look into it.

Thank you.

alexeym June 28, 2015 20:41
Hi,

Maybe I did not get your idea right but atmosphere patch is something special: in every alpha (air, drop, and film) it has type inletOutlet (this is OK), inletValue is 0, and initial value is 0, i.e. there is no matter at this patch and it produces nothing in case of counter-flow ;) So rho there is zero, and as a result you got division by zero FPE.

Since air is in contact with atmosphere initially, I have changed BC to:

Code:
    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 1;
        value          uniform 1;
    }
and the error disappeared.

krishtej23 June 29, 2015 02:03
Quote:
Originally Posted by alexeym (Post 552478)
Hi,

Maybe I did not get your idea right but atmosphere patch is something special: in every alpha (air, drop, and film) it has type inletOutlet (this is OK), inletValue is 0, and initial value is 0, i.e. there is no matter at this patch and it produces nothing in case of counter-flow ;) So rho there is zero, and as a result you got division by zero FPE.

Since air is in contact with atmosphere initially, I have changed BC to:

Code:
    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 1;
        value          uniform 1;
    }
and the error disappeared.
Thank you very much Alex. I corrected the mistake and it worked.


All times are GMT -4. The time now is 18:26.