CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

OpenFOAM remote cluster run error

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

Like Tree1Likes
  • 1 Post By alexeym

Reply
 
LinkBack Thread Tools Display Modes
Old   June 21, 2015, 19:29
Default OpenFOAM remote cluster run error
  #1
New Member
 
krishh
Join Date: Apr 2012
Posts: 16
Rep Power: 5
krishtej23 is on a distinguished road
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.
krishtej23 is offline   Reply With Quote

Old   June 22, 2015, 06:19
Default
  #2
Member
 
Saideep
Join Date: Apr 2015
Location: INDIA
Posts: 96
Rep Power: 2
Saideep is on a distinguished road
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
Saideep is offline   Reply With Quote

Old   June 22, 2015, 10:25
Default
  #3
New Member
 
krishh
Join Date: Apr 2012
Posts: 16
Rep Power: 5
krishtej23 is on a distinguished road
Quote:
Originally Posted by Saideep View Post
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.
krishtej23 is offline   Reply With Quote

Old   June 22, 2015, 10:39
Default
  #4
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,303
Rep Power: 23
alexeym will become famous soon enoughalexeym will become famous soon enough
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.
alexeym is offline   Reply With Quote

Old   June 28, 2015, 14:12
Default
  #5
New Member
 
krishh
Join Date: Apr 2012
Posts: 16
Rep Power: 5
krishtej23 is on a distinguished road
Quote:
Originally Posted by alexeym View Post
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.
Attached Files
File Type: zip droptest.zip (13.5 KB, 1 views)
krishtej23 is offline   Reply With Quote

Old   June 28, 2015, 20:41
Default
  #6
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,303
Rep Power: 23
alexeym will become famous soon enoughalexeym will become famous soon enough
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 likes this.
alexeym is offline   Reply With Quote

Old   June 29, 2015, 02:03
Default
  #7
New Member
 
krishh
Join Date: Apr 2012
Posts: 16
Rep Power: 5
krishtej23 is on a distinguished road
Quote:
Originally Posted by alexeym View Post
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.
krishtej23 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mesquite - Adaptive mesh refinement / coarsening? philippose OpenFOAM Running, Solving & CFD 94 January 27, 2016 10:40
GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM 300 October 29, 2014 19:00
Building OpenFOAM1.7.0 from source ata OpenFOAM Installation 42 May 14, 2012 20:48
How to install CGNS under windows xp? lzgwhy Main CFD Forum 1 January 11, 2011 19:44
checking the system setup and Qt version vivek070176 OpenFOAM Installation 22 June 1, 2010 12:34


All times are GMT -4. The time now is 07:12.