Hi,

I still get the following error message when running the pimpleDyMFoam solver of OF-2.1.x.

I attach the residuals and forces curves. Force curve is doing towards the experimental value. And the computation crashes suddently.

Modifying the maxCo (=2 in propeller example) doesn't help.

I need help to solve it ! Thanks.

Courant Number mean: 0.00403827 max: 1.98918
deltaT = 2.7027e-05
Time = 0.00810811

solidBodyMotionFunctions::rotatingMotion::transfor mation(): Time = 0.00810811 transformation: ((0 0 0) (0.927889 (-0.372856 0 0)))
AMI: Creating addressing and weights between 23788 source faces and 23788 target faces
AMI: Patch source weights min/max/average = 4.97804e-08, 1.62573, 1.00003
AMI: Patch target weights min/max/average = 0, 1.30524, 0.999857
PIMPLE: iteration 1
[3] #0 Foam::error::printStack(Foam::Ostream&) in "/shared/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #1 Foam::sigFpe::sigHandler(int) in "/shared/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #2 in "/lib64/libc.so.6"
[3] #3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) in "/shared/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/shared/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
[3] #5
[3] in "/shared/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
[3] #6 __libc_start_main in "/lib64/libc.so.6"
[3] #7
[3] at /home/abuild/rpmbuild/BUILD/glibc-2.14.1/csu/../sysdeps/x86_64/elf/start.S:116
[cfs10:04034] *** Process received signal ***
[cfs10:04034] Signal: Floating point exception (8)
[cfs10:04034] Signal code: (-6)
[cfs10:04034] Failing at address: 0x45f00000fc2
[cfs10:04034] [ 0] /lib64/libc.so.6(+0x34e10) [0x2af5d1ef4e10]
[cfs10:04034] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x2af5d1ef4d95]
[cfs10:04034] [ 2] /lib64/libc.so.6(+0x34e10) [0x2af5d1ef4e10]
[cfs10:04034] [ 3] /shared/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKdRK NS_5UListIdEE+0x24) [0x2af5d117fe44]
[cfs10:04034] [ 4] pimpleDyMFoam(_ZN4FoamdvINS_12fvPatchFieldENS_7vol MeshEEENS_3tmpINS_14GeometricFieldIdT_T0_EEEERKNS_ 11dimensionedIdEERKS8_+0x2a0) [0x43f120]
[cfs10:04034] [ 5] pimpleDyMFoam() [0x419cdb]
[cfs10:04034] [ 6] /lib64/libc.so.6(__libc_start_main+0xed) [0x2af5d1ee123d]
[cfs10:04034] [ 7] pimpleDyMFoam() [0x41d9dd]
[cfs10:04034] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 3 with PID 4034 on node cfs10 exited on signal 8 (Floating point exception)

Regards,

Stephane.

Hi,

I don't know why at a certain point the computation crashes despite good convergence (residuals and forces).

Any idea ?

Stephane.

Unfortunately, I guess it is the same problem I encountered.
Your mesh is rotating and at some point a part of the domain is not covered by any cell, or something like that which results in a crash.

I only did a new mesh with small changes in the generation process and the problem disappeared. But I did not manage to find guidelines to avoid the problem. :(

Hi Vincent,

what kind of modifications in the mesh generation process have you done ?

Did you do something special ?

Regards,

Stephane.

Vincent,

I have used the same process as the propeller tutorial (blockMesh and sHM).

I have tried to have a finer mesh between the rotating part and the stationary part, but the case crashes a bit sooner !

Do you use GridPro for the base grid instead of blockMesh ?

Stephane.

No for this case, I only used SnappyHexMesh.
Actually I made it coarser at the interface and it ran fine. But as I said I do not know the exact settings which will give a good mesh for each case.

When things do not work out it is normal to think that we are doing some mistake, BUT in this case my guess is that the GGI algorithm is broken and needs fixing. Most of the people who have complained here would be able to run their simulation just fine if they used fluent or starccm+ . If they run fine of commercial code then grid is alright.

My opinion is that most probably the issue is with implementation and this could not be removed by fixing mesh.

Could you post your broken case with a 'Allrun' script, it might be easier to see if it's some mistake in the mesh generation if you share your case.

Hi,

I'm still trying to understand why my case crashes.

Hereafter is the logfile of the checkMesh command:
----------------------------------------------------------------------
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.x-500b378f6ba9
Exec : checkMesh
Date : Feb 14 2012
Time : 14:19:40
Host : "cfs10"
PID : 6797
Case : /shared/sanchi/OpenFOAM/sanchi-2.1.x/SMP11_pimpleDyMFoam_7_skew
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: 1660241
faces: 4421588
internal faces: 4219206
cells: 1397571
boundary patches: 8
point zones: 0
face zones: 2
cell zones: 1

Overall number of cells of each type:
hexahedra: 1191559
prisms: 36641
wedges: 0
pyramids: 0
tet wedges: 104
tetrahedra: 0
polyhedra: 169267

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
*Number of regions: 2
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 1496 1660 ok (non-closed singly connected)
outlet 448 465 ok (non-closed singly connected)
outerCylinder_PATCH 3328 3392 ok (non-closed singly connected)
blades_PATCH 106518 137882 ok (non-closed singly connected)
hub_PATCH 12592 15805 ok (non-closed singly connected)
shaft_PATCH 30424 30664 ok (non-closed singly connected)
AMI1 23788 23905 ok (non-closed singly connected)
AMI2 23788 23905 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-571 -600 -600) (2030 600 600)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (1.25554e-16 3.29472e-17 -2.55368e-16) OK.
Max cell openness = 3.71866e-16 OK.
Max aspect ratio = 5.74628 OK.
Minumum face area = 0.032093. Maximum face area = 3797.06. Face area magnitudes OK.
Min volume = 0.0464591. Max volume = 168535. Total volume = 2.93458e+09. Cell volumes OK.
Mesh non-orthogonality Max: 65.511 average: 10.0911
Non-orthogonality check OK.
Face pyramids OK.
***Max skewness = 5.21337, 5 highly skew faces detected which may impair the quality of the results
<<Writing 5 skew faces to set skewFaces
Coupled point location match (average 0) OK.

Failed 1 mesh checks.

End
----------------------------------------------------------------------

Could someone explains me the following lines:
*Number of regions: 2
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"

And the max skewness error appears only after I did the command:
createBaffles -internalFacesOnly -overwrite innerCylinderSmall '(AMI1 AMI2)'

I need help to eliminate these errors and improve the mesh.

Regards,
Stephane.

Vincent,

What format do you use for geometry parts (stl, obj or other) ?
Each part has a separate file or all parts are together into 1 unique file ?

Is your shaft divide in 3 parts (like the propeller tutorial) or is it a unique part ? I ask you this because my intersections between the shaft and the cylinders (innerCylinder and innerSmallCylinder) is not very clean.

Regards,

Stephane.

>Overall domain bounding box (-571 -600 -600) (2030 600 600)
Big domain?

The geometry file that you use for snapping to the AMI cylinder, does it have high enough resolution compared to the edge length of the final mesh?

I don't know about your problems with unclean intersections, sounds strange. Any picture?

Hi,

Now my geometry has only the blades and a small hub. I don't have the shaft. So there is no more intersections between shaft and AMI regions. The case still crashes.

I think the problem is linked with the AMI surfaces. Maybe with my STL surfaces of the innerSmallSurface.

I will try to take the propeller tutorial and only replace the blades with mine and see what happens.

Regards,
Stephane

Hi Stephane,

I don't have access to the files right now, but I think I was using only one stl file for the blades and the shaft. However, it was a specific case since my shaft was short with a finite length (not going out of the domain like in the tutorial) and could be integrated fully into the cylinder part.

Hi Johan, hi Vincent,

Now I run the propeller case with my own propeller inside (without shaft). Til now it is running ... I will be happy when 1 root will be finished.

So the problem could be my innerSurfaceSmall.stl file, which is used for creating the AMI1 and AMI2 surfaces.

Which CAD software are you using to create STL file ?
I have found in the OF-forum that it is better to work with OBJ files because there is no discretization in triangles. In the propeller tutorial only OBJ files are used. Do you know how to create these OBJ files ?

Regards,
Stephane

Hi Stephane

you could try this

http://meshlab.sourceforge.net/

It can import stl and export obj.

I haven't found any cad (free) that can do direct to obj

Greetings to all!

But... OpenFOAM can do that since 2.0.0!! Well, not do CAD directly, but can convert directly!
If I remember correctly, you can do this with either surfaceFeatureConvert or surfaceTransformPoints! It can actually convert between several formats! Simply use a dud extension and it will tell you what extensions it supports.

Best regards,
Bruno

Hi Niels, hi Bruno,

thanks for your messages.

I have improved the mesh.
Nevertheless the case still crashes after:

AMI: Patch source weights min/max/average = 4.38449e-09, 1.09515, 0.999895
AMI: Patch target weights min/max/average = 0, 1.06587, 0.999773

I think I will leave this case aside because I am not able to fix what's wrong.

Regards,
Stephane.

Hi again

A colleague of mine just had the same error and specifically the 0(zero) value in this line is the culprit.

This means (from what I can gather) that there is a(some) cell(s) that has no overlapping of a neighbor face.

What he found was that the layers in the mesh made some cells way too fine just at the AMI interface. He lowered the amount of layers and everything was working.

I urge you to post a bug on the openfoam.com mantis.

At least if they could implement a check for uncovered faces at the AMI and inform the user that the mesh/setup is bad/wrong and exit the solver gracefully instead of showing the garbage it shows now.

Best

If you post your case it will be easier to help, skip the propeller if it's confidential (as long as the case will still crash without it).

Hi again,

Now my propeller case runs. The problem was the AMI1/AMI2 interface.

I have done my background mesh using ICEM hexa. See attached pictures. The pink/blue line is the AMI interface. I don't do any kind of refinement on this interface.

During my siimulation time I often have:
AMI: Patch source weights min/max/average = 1, 1.00001, 1
AMI: Patch target weights min/max/average = 1, 1.00001, 1

Soon I will post a move.

Regards,
Stephane.