CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   Hanging pointer (

fabianpk January 9, 2006 08:41

Hello, I have a problem reco
I have a problem reconstructing parallel cases, and I do not use any cyclic boundaries. I have a wedge mesh, with wall, wedge, symmetryPlane and patch as boundaries. When I try to reconstructPar I get:

Reconstructing volScalarFields


--> FOAM FATAL ERROR : hanging pointer, cannot dereference

From function PtrList::operator[] const
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/lnInclude/PtrListI.H at line 76.

This just turned up one day as I was reconstructing a mesh. I use uncompressed, binary, but I don't think this matters because the error even turns up for the 0 time directory.


eugene January 9, 2006 09:58

Wedges and cyclics are quite s
Wedges and cyclics are quite similar to each other. I imagine the bug fix posted in the bug forum will take care of your problem.

fabianpk January 10, 2006 03:01

Unfortunately it did not work,
Unfortunately it did not work, the only difference is taht the reference to PtrListI.H refers to the one in my home directory and not the one in /home/dm2/henry


mattijs January 10, 2006 05:24

Can you report it as a bug and
Can you report it as a bug and add a simple testcase?

fabianpk January 10, 2006 06:38

Yes, here's a wedge if I decom
Yes, here's a wedge if I decompose this using decomposePar, and then try to reconstruct it, I get the error. So I don't have to create some new data to do it.


hjasak January 10, 2006 06:57

Reproduced it. You've got a
Reproduced it.

You've got a patch called axis with zero faces in it in the original mesh and the code does not handle it. For my taste, you should get rid of the zero-sized patch because you don't need it.


#4 0x4053b75c in Foam::error::abort (this=0x40b31720) at error.C:224
#5 0x0806dbfe in Foam::operator<<> (os=@0x8105650, m={fPtr_ = {__pfn = 0x4053b4ca <foam::error::abort()>, __delta = 0}, err_ = @0x40b31720}) at errorManip.H:85
#6 0x08083d32 in Foam::PtrList<foam::fvpatchfield<double> >::operator[] (this=0xbf8dff70, i=5) at PtrListI.H:76
#7 0x0808d631 in GeometricBoundaryField (this=0x9510f64, bmesh=@0xbf8e0a94, field=@0x9510f10, ptfl=@0xbf8dff70) at GeometricBoundaryField.C:200
#8 0x0809ef47 in GeometricField (this=0x9510ed8, io=@0xbf8dfff8, mesh=@0xbf8e01f8, ds=@0x950fc60, iField=@0xbf8dff7c, ptfl=@0xbf8dff70) at GeometricField.C:277
#9 0x0809fbb6 in Foam::geometricFvFieldReconstructor::reconstructFv VolumeField<double> (this=0xbf8e0f14, fieldIoObject=@0x950f648)
at geometricFvFieldReconstructorReconstructFields.C:2 24
#10 0x0809fe6d in Foam::geometricFvFieldReconstructor::reconstructFv VolumeFields<double> (this=0xbf8e0f14, objects=@0xbf8e0ec0)
at geometricFvFieldReconstructorReconstructFields.C:4 64
#11 0x0807936a in main (argc=3, argv=0xbf8e14b4) at reconstructPar.C:241

fabianpk January 10, 2006 08:10

You mean that the axis patch o
You mean that the axis patch of a wedge should not be set and just left empty?


hjasak January 10, 2006 08:32

Yes - I've deleted the axis pa
Yes - I've deleted the axis patch from the mesh before the decomposition and it works.


sandy January 28, 2011 11:29

Hi eugune, in my case I use the cyclic boundaries. Now I meet the same problem "... hanging pointer, cannot dereference ...", you think, what should I do? Please help out.

All times are GMT -4. The time now is 00:56.