icoFoam - Floating point exception (core dumped)

File · June 18, 2013, 12:00

Hi to everyone,

I have a problem with running a icoFoam on my own mesh. It is a simple model with one inlet and one outlet. The intention is to make a pressure driven flow as I use a very small mesh 1.4x1.4x1.4 mm pressure difference is 5 Pa

Most of the files are copied from icoFoam tutorial case (cavity) of course I adopted them to my case.

Mesh is generated in Avizo and then imported to enGrid and from there to openFoam. I must point that the same mesh works in Fluent without any problem.

Case loads all the input files and starts the caluculation but after the first step it brakes. Here is the log.

PHP Code:


			
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : icoFoam
Date   : Jun 18 2013
Time   : 16:43:15
Host   : "zeus"
PID    : 7484
Case   : /home/filip/OpenFOAM/proba/moje_2
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create mesh for time = 0

Reading transportProperties

Reading field p

Reading field U

Reading/calculating face flux field phi


Starting time loop

Time = 0.0005

Courant Number mean: 0 max: 0
DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 9.00268e-06, No Iterations 606
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 9.63275e-06, No Iterations 600
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 9.85118e-06, No Iterations 609
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#9  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/icoFoam"
#10  
 at icoFoam.C:0
#11  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/icoFoam"
#12  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#13  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/icoFoam"
Floating point exception (core dumped)

Here are my input files if somebody wants to take a look
0:
https://dl.dropboxusercontent.com/u/122319307/0.tar.gz
constant:
https://dl.dropboxusercontent.com/u/...onstant.tar.gz
system:
https://dl.dropboxusercontent.com/u/.../system.tar.gz

Also I runned checkMesh and I had some warning which I don't know how to fix so here is the output:

PHP Code:


			
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : checkMesh
Date   : Jun 18 2013
Time   : 16:57:33
Host   : "zeus"
PID    : 7664
Case   : /home/filip/OpenFOAM/proba/moje_2
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           95290
    faces:            947476
    internal faces:   875052
    cells:            455632
    faces per cell:   4
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    455632
    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: 4
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    Inlet               1966     1143     ok (non-closed singly connected)  
    Outlet              1962     1132     ok (non-closed singly connected)  
    wall                68496    34516    multiply connected (shared edge)  
  <<Writing 8 conflicting points to set nonManifoldPoints

Checking geometry...
    Overall domain bounding box (-5.2703e-07 -5.57384e-07 -5.82047e-07) (0.00141052 0.0014106 0.00141059)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (1.4271e-17 4.92582e-17 -2.06799e-17) OK.
    Max cell openness = 2.7799e-16 OK.
    Max aspect ratio = 15.936 OK.
    Minimum face area = 1.72258e-11. Maximum face area = 1.07184e-09.  Face area magnitudes OK.
    Min volume = 5.78296e-17. Max volume = 1.01736e-14.  Total volume = 6.68254e-10.  Cell volumes OK.
    Mesh non-orthogonality Max: 78.3513 average: 21.5589
   *Number of severely non-orthogonal faces: 6.
    Non-orthogonality check OK.
  <<Writing 6 non-orthogonal faces to set nonOrthoFaces
    Face pyramids OK.
    Max skewness = 3.02936 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

tnx

startingWithCFD · June 19, 2013, 04:19

I have no idea why your case fails, don't have time or much experience to check; what I do know is that you should take into account that your Knudsen is of the order of unity and you may have significant deviation from reality. If this is your final project and not a toy problem, you could/should try dsmcFoam, if you have time and patience.

File · June 20, 2013, 05:03

Quote:

Originally Posted by startingWithCFD

I have no idea why your case fails, don't have time or much experience to check; what I do know is that you should take into account that your Knudsen is of the order of unity and you may have significant deviation from reality. If this is your final project and not a toy problem, you could/should try dsmcFoam, if you have time and patience.

I deal with liquid (water) and therefore Knudsen number isn't relevant in this case, also this is just a toy case but thank you a lot far taking time to look at my case

nlinder · June 20, 2013, 06:07

Hello Filip,

ich could reproduce your error. I don't know how you can get rid of the checkMesh Error - I never used the softwares you used.

But I think the error is similar to the one discussed here (although it is a diffenrent solver)
http://www.cfd-online.com/Forums/ope...mbit-mesh.html
Maybe you can try this analogously in icoFoam? Maybe it is also a problem in the pEqn? In your case it might derive from the error in the mesh..

regards
Nicklas

File · June 24, 2013, 10:46

Thank you Nicklas,

I made some tests and it definitely seems like the problem is with mesh, also in my solver there isn't the part which you commented out of the solver that you used. Nevertheless thank you very much for taking time and looking at my case

Regards
Filip

File · July 5, 2013, 06:45

So I finally solved this problem, there were several things to solve.

First the mesh was bad so when you run check mesh this shouldn't appear

*Number of regions: 4
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"

and regarding the problem with high Courant number that occurred after solving mesh problems I referd to this thread and solved everything

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

Filip

Mirage12 · July 17, 2013, 06:33

Hello

I have the same problem

but your last suggestion is not working in my case.

I am still in the learning phase and want to learn a lot about OpenFOAM.

I try to simulate a laminar flow around around a semi-cylinder.
The mesh was built using Fluent and the solver is icoFoam and i added the temperature in the solver.

here is the link, that i followed :
http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

the time step is 0.0003 s (i would like to use 0.003 s)
the U-inlet is 0.36 m/s.

My Problem is, that icofoam is not stable and crash after 0.0054 s.

Output:

Code:

Time = 0.0051

Courant Number mean: 1.136713534e+69 max: 1.19078826e+73
DILUPBiCG:  Solving for Ux, Initial residual = 0.9999667566, Final residual = 0.755877927, No Iterations 1001
DILUPBiCG:  Solving for Uy, Initial residual = 0.9999479784, Final residual = 0.9360618957, No Iterations 1001
DICPCG:  Solving for p, Initial residual = 1, Final residual = 4533181.225, No Iterations 1001
time step continuity errors : sum local = 1.749270357e+97, global = -1.187219428e+95, cumulative = -1.187219428e+95
DICPCG:  Solving for p, Initial residual = 3.335096097e-27, Final residual = 3.335096097e-27, No Iterations 0
time step continuity errors : sum local = 6.990833057e+97, global = -2.513212123e+97, cumulative = -2.525084317e+97
DILUPBiCG:  Solving for T, Initial residual = 1.612052638e-18, Final residual = 1.612052638e-18, No Iterations 0
ExecutionTime = 391.56 s  ClockTime = 398 s

Time = 0.0054

Courant Number mean: 7.770867293e+97 max: 7.744252838e+101
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  
 in "/home/abm5kor/OpenFOAM/abm5kor-2.2.0/platforms/linux64GccDPOpt/bin/my_icoFoam"
#6  
 in "/home/abm5kor/OpenFOAM/abm5kor-2.2.0/platforms/linux64GccDPOpt/bin/my_icoFoam"
#7  
 in "/home/abm5kor/OpenFOAM/abm5kor-2.2.0/platforms/linux64GccDPOpt/bin/my_icoFoam"
#8  
 in "/home/abm5kor/OpenFOAM/abm5kor-2.2.0/platforms/linux64GccDPOpt/bin/my_icoFoam"
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  
 in "/home/abm5kor/OpenFOAM/abm5kor-2.2.0/platforms/linux64GccDPOpt/bin/my_icoFoam"
Floating point exception (core dumped)

I tried to follow the same logic as in the previous case, but i could not start the solver.

Output:

Code:

Time = 0.36

Courant Number mean: 1.482960672e+29 max: 2.33573784e+37
--> FOAM Warning : 
    From function linearUpwindV(const fvMesh&, const surfaceScalarField& faceFlux, Istream&)
    in file interpolation/surfaceInterpolation/schemes/linearUpwind/linearUpwindV.H at line 153
    Reading "/home/abm5kor/Desktop/validation/my/phi90/Re120/system/fvSchemes.divSchemes.div(phi,U)" at line 32
    unexpected additional entries in stream.
    Only the name of the gradient scheme in the 'gradSchemes' dictionary should be specified.
smoothSolver:  Solving for Ux, Initial residual = 0.6462707961, Final residual = 118182562.6, No Iterations 1000
smoothSolver:  Solving for Uy, Initial residual = 0.7644650429, Final residual = 322775611.9, No Iterations 1000
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/abm5kor/OpenFOAM/abm5kor-2.2.0/platforms/linux64GccDPOpt/bin/my_icoFoam"
#8  
 at my_icoFoam.C:0
#9  
 in "/home/abm5kor/OpenFOAM/abm5kor-2.2.0/platforms/linux64GccDPOpt/bin/my_icoFoam"
#10  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11  
 in "/home/abm5kor/OpenFOAM/abm5kor-2.2.0/platforms/linux64GccDPOpt/bin/my_icoFoam"
Floating point exception (core dumped)

In the attachment please find my system file , without the edit

I could not upload all the files , the size of constant folds exceed the limitation.

thx for support

immortality · July 17, 2013, 09:12

Hi
send me your case to have a look into it:
force.of.love@gmail.com
which university you study in?

zaynah04 · July 17, 2013, 09:37

your courant number is too high..

zaynah04 · July 17, 2013, 09:41

as you are relatively new to Open foam. @Amin, i suggest you start learning it by doing the tutorials. example start with cavity and then proceed with elbow.
Then after doing those tutorials you can proceed with others example the ones with pisoFoam and simpleFoam...

gradually you will get the hang of it.

Then in case when you do your semi cylinder and stil have problem then i will sent you mine. I have already done one same in the past..
Good luck
zaynah

File · July 17, 2013, 09:49

Hi Amin, there are multiple reasons for such a high Courant number, and it causes OpenFoam to brake. Please provide whole case and then somebody could help you

Good luck

Filip

Mirage12 · July 17, 2013, 09:57

Hello

Thx Thx Thx Thx Thx for your answer

your courant number is too high... i know

I am new in the world of OpenFoam, but did already the basic tutorials like ( cavity and airFoil2D...) and learned how to use blockMesh and built my own mesh and geometry

I built the mesh of this case using fluent, but i do not know, how to stabilize the solver

zaynah04 · July 17, 2013, 09:57

did you convert your fluent mesh to foam corectly? did you do a checkMesh? Did you check whether your velocoty lies in the laminar regime?

Mirage12 · July 17, 2013, 10:05

yes

here is the output :

Code:

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           227264
    internal points:  0
    faces:            451978
    internal faces:   224714
    cells:            112782
    faces per cell:   6
    boundary patches: 5
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     112782
    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                  
    WALL1               990      1984     ok (non-closed singly connected)  
    INLET               199      400      ok (non-closed singly connected)  
    OUTLET              199      400      ok (non-closed singly connected)  
    WALL2               312      624      ok (non-closed singly connected)  
    frontAndBackPlanes  225564   227264   ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-8 -8 -0.384838) (27 8 0.384838)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (5.8768e-18 5.49756e-18 2.84944e-19) OK.
    Max cell openness = 1.15957e-14 OK.
    Max aspect ratio = 830.394 OK.
    Minimum face area = 3.89985e-07. Maximum face area = 0.100453.  Face area magnitudes OK.
    Min volume = 3.00162e-07. Max volume = 0.0116522.  Total volume = 429.81.  Cell volumes OK.
    Mesh non-orthogonality Max: 56.0067 average: 11.5224
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.36576 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

Mirage12 · July 17, 2013, 10:15

Here is my case :

http://www.workupload.com/file/MamMd4k

thx a lot for ur support

File · July 17, 2013, 10:43

Just decrees your time step. I put 0.00003 in your case and it seems to work like a charm

I've read that you want to have time step 0.003 but this is simply impossible or I do not know how to do it

P.S not to forget I solved it without temperature, at the moment I don't have time and volition to do that

nimasam · July 17, 2013, 15:35

Quote:

Originally Posted by Mirage12

Here is my case :

http://www.workupload.com/file/MamMd4k

thx a lot for ur support

There are several Options:

1- you can use pisoFoam or simpleFoam for laminar flow too
2- use adjustTimeStep and limit courant number less than one, if you are using timeStep, then you need to choose your time step carefully

3- if you have problem, in temperature stability, please run your case with out solving for energy

, let flow get steady state, then apply your energy equation

P.S.
i did not look your case, and these are general suggestion

nimasam · July 17, 2013, 17:21

i check your case, i almost sure problem returns your mesh

, first try a coarse mesh to see weather you reach an stable result or not

Mirage12 · July 18, 2013, 05:51

the mesh around the geometry is very fine to capture the the boundary layer.
I tried to run the simulation with coarse mes, ant it is working fine.
However i need to use the mesh, which i uploaded (fine mesh).....
So i shouldnot change the mesh.
I tired to use dt=0.00001s the simulation is working, but it will take a lot of time to reach the 100 s. I think using the timestep is not the ideal idea for this case.

....

nimasam · July 18, 2013, 05:59

if you want a final steady-state solution, why dont u use simpleFoam?

July 17, 2013, 17:21		#18
nimasam Senior Member Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,267 Blog Entries: 1 Rep Power: 25	i check your case, i almost sure problem returns your mesh , first try a coarse mesh to see weather you reach an stable result or not __________________ My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam)

July 18, 2013, 05:59		#20
nimasam Senior Member Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,267 Blog Entries: 1 Rep Power: 25	if you want a final steady-state solution, why dont u use simpleFoam? immortality likes this. __________________ My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam)

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Superlinear speedup in OpenFOAM 13	msrinath80	OpenFOAM Running, Solving & CFD	18	March 3, 2015 06:36
simpleFoam Floating point exception error -help	sudhasran	OpenFOAM Running, Solving & CFD	3	March 12, 2012 17:23
Pipe flow in settlingFoam floating point exception	jochemvandenbosch	OpenFOAM Running, Solving & CFD	4	February 16, 2012 04:24
block-structured mesh for t-junction	Robert@cfd	ANSYS Meshing & Geometry	20	November 11, 2011 05:59
Finished simulation doesn't start: floating point exception [Divide by zero]	MaxCFD	STAR-CCM+	3	June 26, 2011 11:31

June 18, 2013, 12:00	icoFoam - Floating point exception (core dumped)	#1
File New Member Filip Gjetvaj Join Date: Mar 2013 Location: Montpellier, FR Posts: 17 Rep Power: 13	Hi to everyone, I have a problem with running a icoFoam on my own mesh. It is a simple model with one inlet and one outlet. The intention is to make a pressure driven flow as I use a very small mesh 1.4x1.4x1.4 mm pressure difference is 5 Pa Most of the files are copied from icoFoam tutorial case (cavity) of course I adopted them to my case. Mesh is generated in Avizo and then imported to enGrid and from there to openFoam. I must point that the same mesh works in Fluent without any problem. Case loads all the input files and starts the caluculation but after the first step it brakes. Here is the log. PHP Code: /---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.2.0 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : 2.2.0-5be49240882f Exec : icoFoam Date : Jun 18 2013 Time : 16:43:15 Host : "zeus" PID : 7484 Case : /home/filip/OpenFOAM/proba/moje_2 nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading transportProperties Reading field p Reading field U Reading/calculating face flux field phi Starting time loop Time = 0.0005 Courant Number mean: 0 max: 0 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 9.00268e-06, No Iterations 606 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 9.63275e-06, No Iterations 600 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 9.85118e-06, No Iterations 609 #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #6 Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #7 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #8 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #9 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/icoFoam" #10 at icoFoam.C:0 #11 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/icoFoam" #12 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #13 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/icoFoam" Floating point exception (core dumped) Here are my input files if somebody wants to take a look 0: https://dl.dropboxusercontent.com/u/122319307/0.tar.gz constant: https://dl.dropboxusercontent.com/u/...onstant.tar.gz system: https://dl.dropboxusercontent.com/u/.../system.tar.gz Also I runned checkMesh and I had some warning which I don't know how to fix so here is the output: PHP Code: /---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: 2.2.0 \| \| \\ / A nd \| Web: www.OpenFOAM.org \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : 2.2.0-5be49240882f Exec : checkMesh Date : Jun 18 2013 Time : 16:57:33 Host : "zeus" PID : 7664 Case : /home/filip/OpenFOAM/proba/moje_2 nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 95290 faces: 947476 internal faces: 875052 cells: 455632 faces per cell: 4 boundary patches: 3 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 455632 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: 4 The mesh has multiple regions which are not connected by any face. <<Writing region information to "0/cellToRegion" Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology Inlet 1966 1143 ok (non-closed singly connected) Outlet 1962 1132 ok (non-closed singly connected) wall 68496 34516 multiply connected (shared edge) <<Writing 8 conflicting points to set nonManifoldPoints Checking geometry... Overall domain bounding box (-5.2703e-07 -5.57384e-07 -5.82047e-07) (0.00141052 0.0014106 0.00141059) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (1.4271e-17 4.92582e-17 -2.06799e-17) OK. Max cell openness = 2.7799e-16 OK. Max aspect ratio = 15.936 OK. Minimum face area = 1.72258e-11. Maximum face area = 1.07184e-09. Face area magnitudes OK. Min volume = 5.78296e-17. Max volume = 1.01736e-14. Total volume = 6.68254e-10. Cell volumes OK. Mesh non-orthogonality Max: 78.3513 average: 21.5589 Number of severely non-orthogonal faces: 6. Non-orthogonality check OK. <<Writing 6 non-orthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 3.02936 OK. Coupled point location match (average 0) OK. Mesh OK. End tnx

June 19, 2013, 04:19		#2
startingWithCFD Member Join Date: Nov 2012 Posts: 58 Rep Power: 14	I have no idea why your case fails, don't have time or much experience to check; what I do know is that you should take into account that your Knudsen is of the order of unity and you may have significant deviation from reality. If this is your final project and not a toy problem, you could/should try dsmcFoam, if you have time and patience.

June 20, 2013, 06:07		#4
nlinder Member Nicklas Linder Join Date: Jul 2012 Location: Germany Posts: 35 Rep Power: 14	Hello Filip, ich could reproduce your error. I don't know how you can get rid of the checkMesh Error - I never used the softwares you used. But I think the error is similar to the one discussed here (although it is a diffenrent solver) http://www.cfd-online.com/Forums/ope...mbit-mesh.html Maybe you can try this analogously in icoFoam? Maybe it is also a problem in the pEqn? In your case it might derive from the error in the mesh.. regards Nicklas

June 24, 2013, 10:46		#5
File New Member Filip Gjetvaj Join Date: Mar 2013 Location: Montpellier, FR Posts: 17 Rep Power: 13	Thank you Nicklas, I made some tests and it definitely seems like the problem is with mesh, also in my solver there isn't the part which you commented out of the solver that you used. Nevertheless thank you very much for taking time and looking at my case Regards Filip

July 5, 2013, 06:45		#6
File New Member Filip Gjetvaj Join Date: Mar 2013 Location: Montpellier, FR Posts: 17 Rep Power: 13	So I finally solved this problem, there were several things to solve. First the mesh was bad so when you run check mesh this shouldn't appear *Number of regions: 4 The mesh has multiple regions which are not connected by any face. <<Writing region information to "0/cellToRegion" and regarding the problem with high Courant number that occurred after solving mesh problems I referd to this thread and solved everything http://www.cfd-online.com/Forums/ope...-explodes.html Filip linyanx and linda Li like this.

July 17, 2013, 09:12		#8
immortality Senior Member Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,208 Rep Power: 27	Hi send me your case to have a look into it: force.of.love@gmail.com which university you study in? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

July 17, 2013, 09:37		#9
zaynah04 Senior Member zaynah K. Join Date: Jun 2012 Location: Mauritius Posts: 138 Rep Power: 14	your courant number is too high..

July 17, 2013, 09:41		#10
zaynah04 Senior Member zaynah K. Join Date: Jun 2012 Location: Mauritius Posts: 138 Rep Power: 14	as you are relatively new to Open foam. @Amin, i suggest you start learning it by doing the tutorials. example start with cavity and then proceed with elbow. Then after doing those tutorials you can proceed with others example the ones with pisoFoam and simpleFoam... gradually you will get the hang of it. Then in case when you do your semi cylinder and stil have problem then i will sent you mine. I have already done one same in the past.. Good luck zaynah nimasam likes this.

July 17, 2013, 09:49		#11
File New Member Filip Gjetvaj Join Date: Mar 2013 Location: Montpellier, FR Posts: 17 Rep Power: 13	Hi Amin, there are multiple reasons for such a high Courant number, and it causes OpenFoam to brake. Please provide whole case and then somebody could help you Good luck Filip

July 17, 2013, 09:57		#12
Mirage12 Member Amin Join Date: May 2013 Posts: 76 Rep Power: 13	Hello Thx Thx Thx Thx Thx for your answer your courant number is too high... i know I am new in the world of OpenFoam, but did already the basic tutorials like ( cavity and airFoil2D...) and learned how to use blockMesh and built my own mesh and geometry I built the mesh of this case using fluent, but i do not know, how to stabilize the solver

July 17, 2013, 10:15		#15
Mirage12 Member Amin Join Date: May 2013 Posts: 76 Rep Power: 13	Here is my case : http://www.workupload.com/file/MamMd4k thx a lot for ur support

July 17, 2013, 10:43		#16
File New Member Filip Gjetvaj Join Date: Mar 2013 Location: Montpellier, FR Posts: 17 Rep Power: 13	Just decrees your time step. I put 0.00003 in your case and it seems to work like a charm I've read that you want to have time step 0.003 but this is simply impossible or I do not know how to do it P.S not to forget I solved it without temperature, at the moment I don't have time and volition to do that

July 18, 2013, 05:51		#19
Mirage12 Member Amin Join Date: May 2013 Posts: 76 Rep Power: 13	the mesh around the geometry is very fine to capture the the boundary layer. I tried to run the simulation with coarse mes, ant it is working fine. However i need to use the mesh, which i uploaded (fine mesh)..... So i shouldnot change the mesh. I tired to use dt=0.00001s the simulation is working, but it will take a lot of time to reach the 100 s. I think using the timestep is not the ideal idea for this case. ....