I was trying to make a cyclic
 

I was trying to make a cyclic boundary out of two patches on a mesh converted from FLUENT mesh. And createPatch crashed, giving segmentation error as shown below.


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

Reading createPatchDict.

Using relative tolerance 0.001 to match up faces and points

Create polyMesh for time = 0

Adding new patch periodic-wake of type cyclic as patch 20

Moving faces from patch periodic_wake to patch 20
Moving faces from patch periodic_wake_shadow to patch 20

Doing topology modification to order faces.

#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/home/sek/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/sek/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt in "/lib64/tls/libc.so.6"
#3 Foam::face::normal(Foam::Field<foam::vector<double > > const&) const in "/home/sek/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::cyclicPolyPatch::getCentresAndAnchors(Foam:: PrimitivePatch<foam::face,> > const&, Foam::Vector<double> > const&, Foam::List<foam::face> const&, Foam::List<foam::face> const&, Foam::Field<foam::vector<double> >&, Foam::Field<foam::vector<double> >&, Foam::Field<foam::vector<double> >&, Foam::Field<double>&) const in "/home/sek/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#5 Foam::cyclicPolyPatch::order(Foam::PrimitivePatch< foam::face,> > const&, Foam::Vector<double> > const&, Foam::List<int>&, Foam::List<int>&) const in "/home/sek/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#6 Foam::polyTopoChange::reorderCoupledFaces(bool, Foam::polyBoundaryMesh const&, Foam::List<int> const&, Foam::List<int> const&, Foam::Field<foam::vector<double> > const&) in "/home/sek/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#7 Foam::polyTopoChange::compactAndReorder(Foam::poly Mesh const&, bool, bool, bool, int&, Foam::Field<foam::vector<double> >&, Foam::List<int>&, Foam::List<int>&, Foam::List<foam::objectmap>&, Foam::List<foam::objectmap>&, Foam::List<foam::objectmap>&, Foam::List<foam::objectmap>&, Foam::List<foam::objectmap>&, Foam::List<foam::objectmap>&, Foam::List<foam::objectmap>&, Foam::List<foam::objectmap>&, Foam::List<foam::map<int> >&, Foam::List<int>&, Foam::List<int>&, Foam::List<foam::map<int> >&) in "/home/sek/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#8 Foam::polyTopoChange::changeMesh(Foam::polyMesh&, bool, bool, bool, bool) in "/home/sek/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#9 main in "/home/sek/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPatch"
#10 __libc_start_main in "/lib64/tls/libc.so.6"
#11 __gxx_personality_v0 in "/home/sek/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPatch"
Segmentation fault

Could you try the 1.5.x versio
 

Could you try the 1.5.x version and let us know if it works? 1.5.x should have some fixes regarding matching. If still persists could you post the case or send it directly to me?

createPatch does not work to make cyclic patch
 

hello

I do not why making a cyclic patch with createPatch is impossible for me. I made a simple box in blockMeshDict just to test createPatch. I tried to patch front and back with both version 1.5 and 1.5-x but both gave me the same error:

Create time
Reading createPatchDict.
Using relative tolerance 0.001 to match up faces and points
Create polyMesh for time = 0
Adding new patch Z of type cyclic as patch 5
Moving faces from patch maxZ to patch 5
Moving faces from patch minZ to patch 5

Doing topology modification to order faces.

#0 Foam::error::printStack(Foam::Ostream&) in "/home/mou/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/mou/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
.
.
.
#10 __libc_start_main in "/lib/libc.so.6"
#11 _start in "/home/mou/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPatch"
Segmentation fault

I attached the case directory.
I appreciate any comments.

Mou

Hi

I had the same/similar problem a while ago.
I was able to solve it by removing all additional entries in the controlDict file, e.g. libs() or other probe/averaging functions.

Markus

Thank you Markus for your reply. I checked the controlDict file but there is not any of extra things that you mentioned. Would you post a sample case that createPatch can work for that?

Thank you
mou

Switch off pointSync in the createPatchDict and it works for me in 1.5.x.

(the point synchronisation doesn't handle points being on multiple cyclics)

As you said mattijs, I put "false" for pointSync in the createPatchDict, and checked it by 1.5-x. I faced the same error. I just copied the createPatch directory from 1.5-x in .../utilities/mesh/manipulation/ of OpenFOAM-1.5 and compile it. Do I need to compile whole 1.5-x package?

Regards
Mou

Yes, the changes are also to the libraries, not just to the createPatch application. You will need to compile the whole 1.5.x.

Cyclic BC's
 

Hi Foamers,

I am also struggling with the cyclic buondaries.

I created a mesh in gambit with inlet and outet face meshes linked. Now I imported the ascii mesh in OF-1.5 and tried to couple the inlet and outlet face boundaries into a single patch of type cyclic using createPatch utility.

However the utillity crashes giving the similar segmentation fault error as posted in the topic. I also removed the custom libraries libs( ...) and any function objects from controldict system file as suggested by Markus in this topic.

I also tried to switch off the pointsyn flag as suggested by mattijs, but its giving the same segmentation fault error.

I am posting the error messages I received :-

--------------------------------------------------------------------------------------------------------------------------------
sm.kumar@linux-3:~/OpenFOAM/sm.kumar-1.5/Sumeet/annulus/annulus_case> createPatch
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : createPatch
Date : Mar 23 2009
Time : 14:52:57
Host : linux-3
PID : 19511
Case : /home/sm.kumar/OpenFOAM/sm.kumar-1.5/Sumeet/annulus/annulus_case
nProcs : 1

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

Reading createPatchDict.

Using relative tolerance 0.001 to match up faces and points

Create polyMesh for time = 0

Adding new patch perd of type cyclic as patch 4

Moving faces from patch symmetry-3 to patch 4
Moving faces from patch periodic to patch 4

Sumeet Chechk1
Doing topology modification to order faces.

Sumeet Chechk2
#0 Foam::error::printStack(Foam::Ostream&) in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::face::normal(Foam::Field<Foam::Vector<double > > const&) const in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::cyclicPolyPatch::getCentresAndAnchors(Foam:: PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::List<Foam::face> const&, Foam::List<Foam::face> const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<Foam::Vector<double> >&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) const in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#5 Foam::cyclicPolyPatch::order(Foam::PrimitivePatch< Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::List<int>&, Foam::List<int>&) const in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#6 Foam::polyTopoChange::reorderCoupledFaces(bool, Foam::polyBoundaryMesh const&, Foam::List<int> const&, Foam::List<int> const&, Foam::Field<Foam::Vector<double> > const&) in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#7 Foam::polyTopoChange::compactAndReorder(Foam::poly Mesh const&, bool, bool, bool, int&, Foam::Field<Foam::Vector<double> >&, Foam::List<int>&, Foam::List<int>&, Foam::List<Foam:bjectMap>&, Foam::List<Foam:bjectMap>&, Foam::List<Foam:bjectMap>&, Foam::List<Foam:bjectMap>&, Foam::List<Foam:bjectMap>&, Foam::List<Foam:bjectMap>&, Foam::List<Foam:bjectMap>&, Foam::List<Foam:bjectMap>&, Foam::List<Foam::Map<int> >&, Foam::List<int>&, Foam::List<int>&, Foam::List<Foam::Map<int> >&) in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#8 Foam:olyTopoChange::changeMesh(Foam:olyMesh&, bool, bool, bool, bool) in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#9 main in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPatch"
#10 __libc_start_main in "/lib64/libc.so.6"
#11 __gxx_personality_v0 in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPatch"
Segmentation fault
--------------------------------------------------------------------------------------------------------------------------------

I tried to go through the createPatch source to find out the step causing errors


Code snippet :-
Line numbers 545-555
--------------------------------------------------------------------------------------------------------------------------------

// Change mesh, use inflation to reforce calculation of transformation
// tensors.

Info<< " Sumeet Chechk1 " << endl; // Debug statements
Info<< "Doing topology modification to order faces." << nl << endl;
Info<< " Sumeet Chechk2 " << endl; // Debug statements

autoPtr<mapPolyMesh> map = meshMod.changeMesh(mesh, true);

Info<< " Sumeet Chechk3 " << endl; // Debug statements
Info<< "mapping done " << nl << endl;
-----------------------------------------------------------------------------------------------------------------------------

However I could not figure out the sources of error caused during the mapping process. Please someone help me to find out what could be the possible source of error. Also share your previous similar experiences and how you resolved it.

Thanks
SK

You seem to be using 1.5. Have you tried 1.5.x? It contains fixes to do with cyclic patch matching.

openFOAM 1.5.x installation
 

Hi mattijs,

I am quite new to OF. I started with OF-1.5 and it works gr8 on my linux terminal.

I did a search to find out the topics on 1.5.x installation. On link "http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/release/" I found two compressed archives
OpenFOAM-1.5-de.r1094.tgz (30Mb)
ThirdParty.General_2008-12-11.tgz (125Mb)Could you specify which link to continue with?

I am using openSUSE 10.3 (x86_64)

Thanks in adv
SK

Found!
 

Hi mattijs,

I just found the installation webpage the git repository. for OF 1.5.x

http://www.opencfd.co.uk/openfoam/do....html#download

Ignore the previous msg.

Thanks!
SK

Face Area Matching
 

Hi mattijs,

The segmentation fault error is fixed in OF-1.5.x. it works fine. However it still posts errors:-

--------------------------------------------------------------------------------------------------------------------------------
Patch:per_final : Cannot match vectors to faces on both sides of patch
Perhaps your faces do not match? The obj files written contain the current match.
Continuing with incorrect face ordering from now on!

face 6 area does not match neighbour 5006 by 0.108917% -- possible face ordering problem.
patch:per_final my area:0.0102764 neighbour area:0.0102876 matching tolerance:0.001
Mesh face:55406 vertices:4((-9.82281 -1.87413 10) (-9.92119 -1.25298 10) (-9.93765 -1.25488 10) (-9.8386 -1.87729 10))
Neighbour face:60406 vertices:4((-9.92124 -1.25262 0) (-9.82275 -1.87446 0) (-9.83854 -1.87762 0) (-9.93769 -1.25453 0))
Rerun with cyclic debug flag set for more information.

From function cyclicPolyPatch::calcTransforms()
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at l ine 158.

FOAM exiting

--------------------------------------------------------------------------------------------------------------------------------
I have set the writeprecision to be 12 in ControlDict. I also used utilities to output the face centers of both the patches. Both the face centers differ by 9th dec place onwards. Any suggestions??

Incase I change the tol value to 0.01, it may end up in incorrect face matching. However, same tol levels would be different when running the simulations.

So what happens if you increase the matchTolerance and enable pointSync? It should still pick the closest match to couple to and the pointSync will snap the points such that there are no future errors.

Hi Again,

I started increasing the matchTol from 0.001 and finally ended up to 1 at which createPatch could finally order the faces and create a new merged cyclic patch. (pointsync set as false).

Then I tried with pointsync set as true. I got following messages :-

-----------------------------------------------------------------------------------------------------------------------
Create time
Reading createPatchDict.
Using relative tolerance 1 to match up faces and points
Create polyMesh for time = 0
Adding new patch per_final of type cyclic as patch 4

Moving faces from patch periodic to patch 4
Moving faces from patch symmetry-3 to patch 4

Doing topology modification to order faces.

cyclicPolyPatch::order : Writing half0 faces to OBJ file "per_final_half0_faces.obj"
cyclicPolyPatch::order : Writing half1 faces to OBJ file "per_final_half1_faces.obj"
cyclicPolyPatch::order : Dumping currently found cyclic match as lines between corresponding face centres to file "/home/lcfd/OpenFOAM/lcfd-1.5.x/Sumeet/annulus_case/per_final_faceCentres.obj"
--> FOAM Serious Error :
From function cyclicPolyPatch::order(const primitivePatch&, labelList&, labelList&) const
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 1257
Patch:per_final : Cannot match vectors to faces on both sides of patch
Perhaps your faces do not match? The obj files written contain the current match.
Continuing with incorrect face ordering from now on!

Synchronising points.
--> FOAM Warning :
From function syncTools<class T, class CombineOp>::syncPointList(const polyMesh&, UList<T>&, const CombineOp&, const T&, const bool)
in file /home/lcfd/OpenFOAM/OpenFOAM-1.5.x/src/OpenFOAM/lnInclude/syncToolsTemplates.C at line 1047
There are decomposed cyclics in this mesh with transformations.
This is not supported. The result will be incorrect
Points changed by average:0.174201962375 max:10.020097921

face 0 area does not match neighbour 5000 by 199.314% -- possible face ordering problem.
patch:per_final my area:0.0161796 neighbour area:9.41746 matching tolerance:1
Mesh face:55400 vertices:4((-9.98025 -0.628118 10) (-9.99742 0.628969 10) (-9.99741 -0.629182 10) (-9.92119 -1.25298 10))
Neighbour face:60400 vertices:4((-9.98025 -0.628118 -1.77636e-15) (-9.92119 -1.25298 10) (-9.99741 -0.629182 10) (-9.99742 0.628969 10))
Rerun with cyclic debug flag set for more information.

From function cyclicPolyPatch::calcTransforms()
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 158.

FOAM exiting
-------------------------------------------------------------------------------------------------------------------------------

This states that it is not able to sync points as again newpatch-face0 is not able to match with newpatch-face(n/2).(which it was able to when pointsync was switched off)

I have been rather successful with coarse grids with cyclic bc's in OF, but this is a fine mesh. Is this the cause of error and to check if there is a loss of significant digits while converting the meshes and writing new patches in OF etc etc.( leading to causing errors in calculating face areas by clipping significant digits of nodes and in face ordering) I tried setting the write precision IO in fluent3D.. mesh converter to 16.

However this did not resolve the problem. It continues with the same face matching errors.

Is something wrong with the calculation of transformation matrix. as far as i know it automatically calculates the rotation/translational translational matrix - is it correct. (mine is a translational cyclic)
Plz help

It has dumped the match so far to obj files : "per_final_half0_faces.obj" etc. Use objToVTK+paraview to visualise those. Are both halves correctly picked up? Do the faces exactly overlay?

Does anybody know what pointSync does exactly ?
It is said that: " Do a synchronisation of coupled points after creation of any patches".
Can anyone further explain ?
Thanks a lot.

createPatch segmentation fault with OF 1.6-x
 

Hi everyone,

I've tried to use the createPatch utility to create a cyclic patch along the same lines as the rest of the users have already posted here and as Sumeet has indicated above, I get the same segmentation fault.
I'm actually using OF 1.6-x , which I'm assuming has the bugs fixed which were there prior to 1.5-x.

So any advice on how to overcome this segmentation fault would be much appreciated.

Thanks in advance.

Best,
Vasu

If you have multiple cyclics make sure to have pointSync switched off - it will try to synchronise points on opposite sides but cannot yet handle points on multiple cyclics.

Just run checkMesh on the resulting mesh (dumped to a new time directory) to make sure the resulting mesh is ok.

If the problem persists please post a simple testcase here.

Hello again,

Sorry for the delay in following up, I've had some end of term exams :)

Ok I've attached a test case for createPatch. It's a wedge shaped cylinder using blockMeshDict. I've done the same case using wedge patch types for the "front" and "back" patches, and it works alright.

But I want to create a cylinder with a central core region that is empty, which is why I made the mesh externally with Gambit and am trying to use createPatch on the "front" and "back" patches to make them cyclic, for an axisymmetric case. I hope that makes sense.

Any ideas on how to do this without createPatch would also be very welcome.

Here is the error I'm getting when I run the attached test case:

Create time

Create polyMesh for time = 0

Reading createPatchDict.

Using relative tolerance 1 to match up faces and points

Adding new patch new_front_back as patch 6 from
{
type cyclic;
}


Moving faces from patch front to patch 6
#0 Foam::error::printStack(Foam:: Ostream&) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 changePatchID(Foam::polyMesh const&, int, int, Foam::polyTopoChange&) in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/createPatch"
#4 main in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/createPatch"
#5 __libc_start_main in "/lib64/libc.so.6"
#6 _start in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/createPatch"
Segmentation fault

Thanks in advance for any help.

Best regards,
Vasu

I changed matchTolerance to 1e-3 and it runs fine in 1.6.x. Don't see anything under valgrind either.

p.s. you have illegal patch fields on front and back for 0/p and 0/U.

Hi,

Thank you for checking it. I tried running it again with the tolerance 1e-3. And I still get the following errors:

bash-3.2$ #0 Foam::error::printStack(Foam::Ostream&) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::tmp<Foam::Field<double> > Foam::fvPatch::patchInternalField<double>(Foam::UL ist<double> const&) const in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/icoFoam"
#4 Foam::fvPatchField<double>::patchInternalField() const in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/icoFoam"
#5 Foam::wedgeFvPatchField<double>::evaluate(Foam::Ps tream::commsTypes) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#6 Foam::wedgeFvPatchField<double>::wedgeFvPatchField (Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#7 Foam::fvPatchField<double>::adddictionaryConstruct orToTable<Foam::wedgeFvPatchField<double> >::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#8 Foam::fvPatchField<double>::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/icoFoam"
#9 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::GeometricB oundaryField(Foam::fvBoundaryMesh const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/icoFoam"
#10 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readField(Foam::Istream&) in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/icoFoam"
#11 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/icoFoam"
#12 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/icoFoam"
#13 __libc_start_main in "/lib64/libc.so.6"
#14 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/icoFoam"

I need to know if this might be a problem with installing the new version, since we have changed to 1.6-x recently and I basically cannot understand most of these errors.

Sorry if my questions are trivial. But any information would be really appreciated.

Best regards,
Vasu

Your previous error was from createPatch. This error seems to be from icoFoam and from a wedge patchField. The createPatch case did not contain any wedges.

Hello,

Yes I'm so sorry, I'm running another case with wedge patch types, and I posted the wrong one.

This is the error with the create_patch_test_case:

Moving faces from patch front to patch 6
#0 Foam::error::printStack(Foam::Ostream&) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/local/gvasudha/OpenFOAM/gvasudha-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 changePatchID(Foam::polyMesh const&, int, int, Foam::polyTopoChange&) in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/createPatch"
#4 main in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/createPatch"
#5 __libc_start_main in "/lib64/libc.so.6"
#6 _start in "/opt/software/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/createPatch"
Segmentation fault


Again I'm really sorry for the mix-up.

Are you using an uptodate 1.6.x?

You could in $FOAM_UTILITIES/mesh/manipulation/createPatch add the debug flags to Make/options (see http://openfoamwiki.net/index.php/HowTo_debugging) and

wclean
wmake

and see where the error comes from.

similar problems
 

Hi al,l

I am using OF1.6.x, converted the mesh from ICEM, just two parallel surfaces need to be made cyclic, it worked for one of the mesh I created without any problem. another mesh i made is quite similar with the previous one, but it was just not able to get through when I run the same createPatchDict. The error is something like this ...
----------------------------------------
face 6 area does not match neighbour 5006 by 0.108917% -- possible face ordering problem.
patch:per_final my area:0.0102764 neighbour area:0.0102876 matching tolerance:0.001
___________________

Increased the tolerance to 1, cyclic boundary was created but with error messages like this:
------------------------
cyclicPolyPatch::order : Writing half0 faces to OBJ file "frontBack1_half0_faces.obj"
cyclicPolyPatch::order : Writing half1 faces to OBJ file "frontBack1_half1_faces.obj"
cyclicPolyPatch::order : Dumping currently found cyclic match as lines between corresponding face centres to file "/home/vela/yingchun/OpenFOAM/yingchun-1.6.x/run/lestry03/frontBack1_faceCentres.obj"
--> FOAM Serious Error :
From function cyclicPolyPatch::order(const primitivePatch&, labelList&, labelList&) const
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 1547
Patch:frontBack1 : Cannot match vectors to faces on both sides of patch
Perhaps your faces do not match? The obj files written contain the current match.
Continuing with incorrect face ordering from now on!
Dumping frontBack1 half0 faces to "coupled_frontBack1_half0.obj"
Dumping frontBack1 half1 faces to "coupled_frontBack1_half1.obj"
Dumping cyclic match as lines between face centres to "coupled_frontBack1_match.obj"
Synchronising points.
On coupled patch frontBack1 separation[0] was (1.37682718046e-07 -5.12042025335e-10 -1.1999999881)
On coupled patch frontBack1 forcing uniform separation of 1((-1.85957778909e-06 -2.09167501777e-08 -1.1999999881))
Synchronising points.
Points changed by average:8.78905215655e-07 max:0.0143106865778
Removing patches with no faces in them.
Removing empty patch frontBack at position 24
Removing patches.
Dumping frontBack1 half0 faces to "final_frontBack1_half0.obj"
Dumping frontBack1 half1 faces to "final_frontBack1_half1.obj"
Dumping cyclic match as lines between face centres to "final_frontBack1_match.obj"
Writing repatched mesh to 1e-05
__________________________________

checked the obj mesh with paraview, it seems fine, not sure if this mesh is going to be ok with this error message.

Have any of you who had the similar problem found a way to fix this now?

Thank you
Forrest

Looks like your opposite faces do not have the same area.

What does

checkMesh -time 1e-05

say about the resulting mesh?