 |
 |
 |
|
|
|
[Sponsors] | ||||
icoFoam - Floating point exception (core dumped) |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 18, 2013, 11:00
|
icoFoam - Floating point exception (core dumped)
|
#1 |
|
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:
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:
|
|
|
|
|
|
June 19, 2013, 03:19
|
|
#2 |
|
Member
Join Date: Nov 2012
Posts: 58
Rep Power: 13 |
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, 04:03
|
|
#3 | |
|
New Member
Filip Gjetvaj
Join Date: Mar 2013
Location: Montpellier, FR
Posts: 17
Rep Power: 13 |
Quote:
|
||
|
|
|
||
|
June 20, 2013, 05:07
|
|
#4 |
|
Member
Nicklas Linder
Join Date: Jul 2012
Location: Germany
Posts: 35
Rep Power: 13 |
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, 09:46
|
|
#5 |
|
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, 05:45
|
|
#6 |
|
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 |
|
|
|
|
|
|
July 17, 2013, 05:33
|
|
#7 |
|
Member
Amin
Join Date: May 2013
Posts: 76
Rep Power: 12 |
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) 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)
I could not upload all the files , the size of constant folds exceed the limitation. thx for support
Last edited by Mirage12; July 17, 2013 at 07:52. |
|
|
|
|
|
|
July 17, 2013, 08:12
|
|
#8 |
|
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 26 |
__________________
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, 08:37
|
|
#9 |
|
Senior Member
zaynah K.
Join Date: Jun 2012
Location: Mauritius
Posts: 138
Rep Power: 13 |
your courant number is too high..
|
|
|
|
|
|
|
July 17, 2013, 08:41
|
|
#10 |
|
Senior Member
zaynah K.
Join Date: Jun 2012
Location: Mauritius
Posts: 138
Rep Power: 13 |
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 |
|
|
|
|
|
|
July 17, 2013, 08:49
|
|
#11 |
|
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, 08:57
|
|
#12 |
|
Member
Amin
Join Date: May 2013
Posts: 76
Rep Power: 12 |
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, 08:57
|
|
#13 |
|
Senior Member
zaynah K.
Join Date: Jun 2012
Location: Mauritius
Posts: 138
Rep Power: 13 |
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?
|
|
|
|
|
|
|
July 17, 2013, 09:05
|
|
#14 |
|
Member
Amin
Join Date: May 2013
Posts: 76
Rep Power: 12 |
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
|
|
|
|
|
|
|
July 17, 2013, 09:15
|
|
#15 |
|
Member
Amin
Join Date: May 2013
Posts: 76
Rep Power: 12 |
||
|
|
|
|
|
July 17, 2013, 09:43
|
|
#16 |
|
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 17, 2013, 14:35
|
|
#17 | |
|
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
Quote:
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 equationP.S. i did not look your case, and these are general suggestion
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
||
|
|
|
||
|
July 17, 2013, 16:21
|
|
#18 |
|
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
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, 04:51
|
|
#19 |
|
Member
Amin
Join Date: May 2013
Posts: 76
Rep Power: 12 |
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. ....
|
|
|
|
|
|
|
July 18, 2013, 04:59
|
|
#20 |
|
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
if you want a final steady-state solution, why dont u use simpleFoam?
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
|
|
|
|
|
| Tags |
| (core dumped), floating point exception, icofoam |
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| Superlinear speedup in OpenFOAM 13 | msrinath80 | OpenFOAM Running, Solving & CFD | 18 | March 3, 2015 05:36 |
| simpleFoam Floating point exception error -help | sudhasran | OpenFOAM Running, Solving & CFD | 3 | March 12, 2012 16:23 |
| Pipe flow in settlingFoam floating point exception | jochemvandenbosch | OpenFOAM Running, Solving & CFD | 4 | February 16, 2012 03:24 |
| block-structured mesh for t-junction | Robert@cfd | ANSYS Meshing & Geometry | 20 | November 11, 2011 04:59 |
| Finished simulation doesn't start: floating point exception [Divide by zero] | MaxCFD | STAR-CCM+ | 3 | June 26, 2011 10:31 |
4Likes
Linear Mode
