Hi all I'm running a case in which I use cfdemSolverIB with dynamicMesh. I used the twoSpheresGlowinskiMPI tutorial as a base case .
Everithing seems to be OK but suddenly the simulation crashes, below is the error message. I tried adjusting many parameters but nothing seems to solve the problem, if somebody can give me a hand would be great!
You can find attached the case.
Cheers,
Mauro
Time = 0.01315
Selected 0 cells for refinement out of 2421.
Selected 7 split points out of a possible 174.
Unrefined from 2421 to 2372 cells.
Courant Number mean: 0.00404559 max: 0.124786
- evolve()
evolve done.
DILUPBiCG: Solving for Ux, Initial residual = 0.000827412, Final residual = 1.01208e-06, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.00315116, Final residual = 2.68304e-06, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.007329, Final residual = 6.10856e-06, No Iterations 1
suppressing ddt(voidfraction)
DICPCG: Solving for p, Initial residual = 0.627976, Final residual = 9.4635e-07, No Iterations 78
suppressing ddt(voidfraction)
DICPCG: Solving for p, Initial residual = 0.0532128, Final residual = 5.75454e-07, No Iterations 72
time step continuity errors : sum local = 2.1314e-11, global = -5.13077e-14, cumulative = 1.31698e-09
suppressing ddt(voidfraction)
DICPCG: Solving for p, Initial residual = 0.022663, Final residual = 8.5752e-07, No Iterations 73
suppressing ddt(voidfraction)
DICPCG: Solving for p, Initial residual = 0.00188636, Final residual = 6.26946e-07, No Iterations 65
time step continuity errors : sum local = 2.27735e-11, global = 2.17278e-13, cumulative = 1.3172e-09
suppressing ddt(voidfraction)
DICPCG: Solving for p, Initial residual = 0.00068614, Final residual = 7.75048e-07, No Iterations 65
suppressing ddt(voidfraction)
DICPCG: Solving for p, Initial residual = 7.83894e-05, Final residual = 9.20358e-07, No Iterations 7
time step continuity errors : sum local = 3.34571e-11, global = 8.62715e-14, cumulative = 1.31729e-09
suppressing ddt(voidfraction)
DICPCG: Solving for p, Initial residual = 2.9474e-05, Final residual = 8.74119e-07, No Iterations 8
suppressing ddt(voidfraction)
DICPCG: Solving for p, Initial residual = 4.13558e-06, Final residual = 7.44615e-07, No Iterations 2
time step continuity errors : sum local = 2.70691e-11, global = 9.22155e-14, cumulative = 1.31738e-09
particleCloud.calcVelocityCorrection()
DICPCG: Solving for phiIB, Initial residual = 0.632598, Final residual = 6.90708e-07, No Iterations 72
*** Error in `cfdemSolverIB': free(): invalid next size (normal): 0x000000000204c020 ***
[dell-03:10789] *** Process received signal ***
[dell-03:10789] Signal: Aborted (6)
[dell-03:10789] Signal code: (-6)
[dell-03:10789] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x350e0) [0x7efc621aa0e0]
[dell-03:10789] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x37) [0x7efc621aa067]
[dell-03:10789] [ 2] /lib/x86_64-linux-gnu/libc.so.6(abort+0x148) [0x7efc621ab448]
[dell-03:10789] [ 3] /lib/x86_64-linux-gnu/libc.so.6(+0x731b4) [0x7efc621e81b4]
[dell-03:10789] [ 4] /lib/x86_64-linux-gnu/libc.so.6(+0x7898e) [0x7efc621ed98e]
[dell-03:10789] [ 5] /lib/x86_64-linux-gnu/libc.so.6(+0x79696) [0x7efc621ee696]
[dell-03:10789] [ 6] cfdemSolverIB(_ZN4Foam14GeometricFieldINS_6VectorIdEENS_12fvPatchFieldENS_7volMeshEEaSERKNS_3tmpIS5_EE+0x6c) [0x43958c]
[dell-03:10789] [ 7] /home/mauro/OpenFOAM/mauro-2.4.0/platforms/linux64GccDPOpt/lib/liblagrangianCFDEM-PUBLIC-2.4.0.so(_ZN4Foam12cfdemCloudIB22calcVelocityCorrectionERNS_14GeometricFieldIdNS_12fvPatchFieldENS_7volMeshEEERNS1_INS_6VectorIdEES2_S3_EES5_S5_+0x2b7) [0x7efc63d5d0e7]
[dell-03:10789] [ 8] cfdemSolverIB() [0x41db40]
[dell-03:10789] [ 9] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf5) [0x7efc62196b45]
[dell-03:10789] [10] cfdemSolverIB() [0x41f22c]
[dell-03:10789] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 1 with PID 10789 on node dell-03 exited on signal 6 (Aborted).
--------------------------------------------------------------------------
| Attachment | Size |
|---|---|
 dp2_forum.tar_.gz | 56.75 KB |
alice | Mon, 01/09/2017 - 10:51
Hello Mauro,
Hello Mauro,
is it possible that particles left the domain? This case was not covered until now, but will be in the upcoming release.
Best regards,
Alice
mbaldini | Mon, 01/09/2017 - 11:55
Hi Alice, no I'm using
Hi Alice, no I'm using periodic bc so when particles cross the outlet bc are inserted again at the inlet.
Regards,
Mauro
alice | Mon, 01/09/2017 - 13:58
Hello Mauro,
Hello Mauro,
well that might be the source of the error as well. Does the error occur when the first particle leaves (and re-enters) the domain or ? This might not have been tested in the currently available version... I would suggest to use the new release as soon as it is available (this will be announced on the homepage, but will take place within the next weeks), as some improvements were made in that field.
Best regards,
Alice
mbaldini | Tue, 01/10/2017 - 13:01
Hello Alice, I've checked and
Hello Alice, I've checked and the simulation crashes before any particle leaves the domain.
I also turned off the mesh refinement and the simulation runs smooth. Does that makes sense to you? I pasted below the mesh refinement coefficients that I'm using.
Regards,
Mauro
------------------------------------------------------------------------------------------------------------------------------------------------------------------
dynamicRefineFvMeshCoeffs
{
refineInterval 1;//refine every refineInterval timesteps
field interFace; //field to base the refinement
lowerRefineLevel .0001; // mesh refinement trigger
upperRefineLevel 0.99; // mesh coarsening trigger
unrefineLevel 10; // coarsening ratio 2^n
nBufferLayers 2;//1; // number of layers arround a refined cell, gives smooth transition
maxRefinement 2; // refinement level 2^n maximum refinement level (starts from 0)
maxCells 1000000; // max cells in the domain
correctFluxes // fluxes to be corrected due to mesh refinement
(
(phi U)
(phi_0 U)
);
dumpLevel false; // dump the refinement level for debugging
}
------------------------------------------------------------------------------------------------------------------------------------------------------------------
cgoniva | Thu, 01/19/2017 - 12:59
cfdemSolverIB - dynamicMesh
Hello Mauro,
can you please upgrade to CFDEMcoupling 3.6.0 and test again.
as described in the Version History (on this website) there were some changes related to IB particles leaving the domain.
Please let us know the outcome.
Best regards,
Christoph Goniva
mbaldini | Mon, 05/08/2017 - 22:39
Hi Christoph, I finally
Hi Christoph, I finally updated to CFDEMcoupling 3.6.0. and adapted the case. But I am still having the same problems, below you can see the log with the error message:
----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
Time = 0.00053
Selected 0 cells for refinement out of 27193.
Selected 22 split points out of a possible 1384.
Unrefined from 27193 to 27039 cells.
Courant Number mean: 0.000913363 max: 0.10145
- evolve()
evolve done.
DILUPBiCG: Solving for Ux, Initial residual = 0.00115654, Final residual = 1.31886e-06, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.00375824, Final residual = 7.11311e-06, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.00476253, Final residual = 4.69137e-08, No Iterations 2
DICPCG: Solving for p, Initial residual = 0.688986, Final residual = 9.84055e-07, No Iterations 263
time step continuity errors : sum local = 3.14696e-11, global = -1.01118e-13, cumulative = 5.17094e-11
DICPCG: Solving for p, Initial residual = 0.170721, Final residual = 9.93603e-07, No Iterations 261
time step continuity errors : sum local = 6.82889e-12, global = 3.36173e-14, cumulative = 5.1743e-11
DICPCG: Solving for p, Initial residual = 0.023005, Final residual = 9.94789e-07, No Iterations 234
time step continuity errors : sum local = 6.27419e-12, global = -5.03998e-14, cumulative = 5.16926e-11
DICPCG: Solving for p, Initial residual = 0.00540764, Final residual = 8.83428e-07, No Iterations 65
time step continuity errors : sum local = 5.53183e-12, global = -7.20161e-13, cumulative = 5.09725e-11
particleCloud.calcVelocityCorrection()
DICPCG: Solving for phiIB, Initial residual = 0.446333, Final residual = 8.7997e-07, No Iterations 255
ExecutionTime = 25.81 s ClockTime = 26 s
Time = 0.00054
*** Error in `cfdemSolverIB': corrupted double-linked list: 0x0000000002c8d280 ***
[dell-03:50726] *** Process received signal ***
[dell-03:50726] Signal: Aborted (6)
[dell-03:50726] Signal code: (-6)
----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
I checked using different base meshes (from coarse to fine) but I get the same error. But if use a static mesh instead of a dynamic mesh the simulation runs smoothly. I don't what could be the problem. Does anybody has an idea? Thanks in advance.
Regards,
Mauro
medvedeg | Wed, 05/10/2017 - 15:31
couplingInterval
Hallo Mauro,
I tried your setup and have the same error message.
what I see, coupling interval is set to 20. It must be exactly the ratio of CFD time step to that for DEM. It must be 10 (or 1 if you use equal CFD and DEM time steps).
Regards,
mbaldini | Wed, 05/10/2017 - 22:01
Hi Alexander thanks for
Hi Alexander thanks for downloading and testing the case, I really I appreciate that. I don't know why I didn’t check that. Thanks.
Regards,
Mauro