[NickG]

I think that this may have been because I hadn't separated the patches and specified the domain interfaces

Sorry to waste anyone's time

Nick

[mbeaudoin]

No problem.

Usually, you can safely discard the warnings about the presence QUAD and TRI polygons in your CGNS file.

Those 2D elements are sometimes exported in the CGNS file, but as separate 2D entities. They are not part of the 3D mesh nor of the BCs definitions.
At least this was the case in all the valid CGNS files we have converted with this converter.

Martin

Originally Posted by NickG

I think that this may have been because I hadn't separated the patches and specified the domain interfaces

Sorry to waste anyone's time

Nick

[NickG]

Hi

Could someone help me understand how to debug this please:


#0 Foam::error:rintStack(Foam::Ostream&) in "/home/nick/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/nick/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam:olyMesh:olyMesh(Foam::IOobject const&, Foam::Field<Foam::Vector<double> > const&, Foam::List<Foam::cellShape> const&, Foam::List<Foam::List<Foam::face> > const&, Foam::List<Foam::word> const&, Foam::List<Foam::word> const&, Foam::word const&, Foam::word const&, Foam::List<Foam::word> const&, bool) in "/home/nick/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#3 CGNSBoundaryConditions::buildFoamMesh(Foam::Time const&) const in "/home/nick/OpenFOAM/nick-1.5/applications/bin/linuxGccDPOpt/cgnsToFoam"
#4 main in "/home/nick/OpenFOAM/nick-1.5/applications/bin/linuxGccDPOpt/cgnsToFoam"
#5 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#6 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/nick/OpenFOAM/nick-1.5/applications/bin/linuxGccDPOpt/cgnsToFoam"

Thanks in advance

Nick

P.S.If anyone knows how to stop the automatic generation of smilies/emoticons/moronicons when pasting could you tell me how. Thanks

[hamcer]

hi foamers,
is there a difference between a of-1.4.1-dev et OF-1.4.1 concerning the cgns convertor, et specialy in face zones,
any confirmation!!

[NickG]

Hi

I seem to be getting the same error on different meshes that I'm trying to import from CFX or Ansys ICEM.

Trying to specify a boundary face 4(13569 13567 13561 13563) on the face on cell 6456 which is either an internal face or already belongs to some other patch. This is face 12922 of patch 3 named SymT.

Each time I get a similar message aborting at the same line 483 of polyMeshFromShapeMesh.C but don't know how to change it or import it first and then change it.

Any suggestions please?

Nick

[NickG]

Hi y'all

Am still hoping for responses to the previous two posts but meanwhile could someone tell me how to start the adfViewer bundled with the converter.

Thanks

Nick

[mbeaudoin]

Hello,

@adfviewer:
This is part of the cgnstools package, an optional suite of CGNS tools that you can compile if you like. See the file cgnstools_2.5/Allwmake for more details.

@your conversion problem:
I have no clue. Without getting access to your CGNS file, it is difficult to pinpoint the problem, the error message simply reports a problem with some boundary condition definitions in your CGNS file.

What kind of BCs are you using, especially for the patch called SymT?

Most probably, you are using a type of BC in your CGNS file that we have not encounter ourselves while developping the CGNS converters.

Martin

[ashishnedungadi]

Originally Posted by ep4

Hello Martin,

thank you very much for your detailed answer.
The meshes i'm trying to convert contain 3D cells as 2D cells, for the boundaries. Actually, i can see the geometry made of 3D cells which are well converted. The problem i have is that i lose the bidimensional boundaries where i will have to impose conditions in order to run an OpenFOAM simulation. Typically, it creates one "defaultWall" in place of my boundary surfaces.
I don't understand how you define boundary conditions if you export only 3D elements. Do you recreate the boundaries surfaces after the conversion?

Generally, the CGNS files we have have been generated by different software. In this case, i think they have been generated with IcemCFD. I don't know which commercial software you are using.

Thank you again.

Eric

Hello Martin,
First off, thanks for developing this cgns <--> OpenFOAM converter; it is invaluable. The install instructions were perfectly clear and I was able to install with no problems at all.

I am experiencing the same problems as Eric. I followed this thread, but am not sure if this got resolved or not. I get similar errors and when I look at the constant/polyMesh/boundary file I see all the bounday names, but they all have zero faces. All faces get lumped into one default patch. The grid itself looks fine in paraFoam, but now I cannot set any BCs on the individual patches. I tried the -separatePatchesoption, but to no avail.

Here are the messages from cgnsToFoam:
--> FOAM Warning : Cell type "QUAD_4" found in zone 0, section 2 has no OpenFOAM equivalence - skipping
--> FOAM Warning : Cell type "TRI_3" found in zone 0, section 3 has no OpenFOAM equivalence - skipping
--> FOAM Warning : BC "nose" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning : BC "mid-body" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning : BC "stern" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning : BC "farfield" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning : BC "symmetry" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning :
From function polyMesh:olyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 581
Found 54924 undefined faces in mesh; adding to default patch.


I would appreciate it if you could lend me some help with this. Thanks very much for your time and look forward to hearing from you.

Regards
Ashish

[mbeaudoin]

Hello Ashish,

I would suspect those Warning messages first:

--> FOAM Warning : BC "nose" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning : BC "mid-body" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning : BC "stern" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning : BC "farfield" : patch defined by a unsupported PointSetType_t - skipped.
--> FOAM Warning : BC "symmetry" : patch defined by a unsupported PointSetType_t - skipped.

If you take a look at the CGNS SIDS reference document:
http://www.grc.nasa.gov/WWW/cgns/sids/bc.html#BC , Notes #2

You will see that a CGNS BC can be defined by either 1 of 4 types of PointSetType_t:

PointRange
PointList
ElementRange
ElementList

Now, if you take a look at the file CGNSBoundaryConditions.C, starting at line 205, you will see that the cgnsToFoam converter currently only supports the first 2 types, PointRange and PointList.

So your CGNS file was probably generated with BCs defined as either ElementRange or ElementList.

While developing the cgnsToFoam converter, we've basically never encountered such type of BCs definition in our own CGNS files, that why the code is not supporting it.

I would suggest that you check with your CGNS file generator in order to see if you have some control on how the BC patches are exported. PointRange and PointList would be the information cgnsToFoam needs for converting your BCs.

Regards,

Martin

[ashishnedungadi]

Martin,
Thanks for the very prompt response and the CGNS details. I will pass this on to the other developers and perhaps they can do something.

In the meantime, is there anything that can be done via adfviewer or adfedit (not that I would know how to do it) to fix this? Alternatively, and I realize this would be a great imposition on your time, how easy would it be for you to support those other types you mentioned. I can make this grid file available to you if that is of interest. Incidentally, I tried converting some of the sample cases that are on the CGNS (I think sourceforge) website, and those exhibit similar problems.

So in your case, how is your CGNS grid written out such that you can detect the boundary elements? Don't the boundary elements always have to be 2D elements? Curious.

Thanks again for your help. If there is anything I can do with the data file, I would appreciate any pointers from you. Thank you again for being so gracious with your time.

Regards
Ashish

[marico]

Hi,

trying to compile CGNS converters with 1.5-dev, I receive the following message:
...
+ cd utilities
+ wmake all
Making dependency list for source file addSwirlAndRotation.C
Making dependency list for source file foamToCGNS.C
could not open file structure_t.H for source file foamToCGNS.C
could not open file cgnsmll.H for source file foamToCGNS.C
could not open file checkerror.H for source file foamToCGNS.C
Making dependency list for source file logFile.C
...
The compilation of /src seemed to work fine, no errors came after I installed several needed packages... The needed files exist!

Thanks for help,
Marco

[mbeaudoin]

Yeah, I know, I got the same messages too.

Somehow, I have not find a proper way to get rid of this. Probably something to do with the construction of the dependency list by wmake.

You can safely discard those messages.

I will do my best to get rid of those when I will find the time.

Martin

Originally Posted by marico

Hi,

trying to compile CGNS converters with 1.5-dev, I receive the following message:
...
+ cd utilities
+ wmake all
Making dependency list for source file addSwirlAndRotation.C
Making dependency list for source file foamToCGNS.C
could not open file structure_t.H for source file foamToCGNS.C
could not open file cgnsmll.H for source file foamToCGNS.C
could not open file checkerror.H for source file foamToCGNS.C
Making dependency list for source file logFile.C
...
The compilation of /src seemed to work fine, no errors came after I installed several needed packages... The needed files exist!

Thanks for help,
Marco

[marico]

Hi Martin,

thanks for your quick response! So far I only have one missing error: it complains about missing libPstream.so... But that seems to be an other topic?!

One question: In first post you said: "converters not for dynamic mesh"... If I have now a valid converted CFX mesh (ONLY MESH): is it possible to use it with dynamic mesh solver?

Marco

[marico]

Hi Martin,

first of all thanks for that tool. I just managed to convert a mesh to Foam. Unfortunately I recieved the same error message as above:

Trying to specify a boundary face .. on the face on cell ... which is either an internal face or already belongs to some other patch. This is face ... of patch 2 named IntakeWall.

The mesh contains 3 regions, one structured and 2 unstructured, of which only 1 can be converted. The other one creates the error. The boundary type of the concerned boundary is wall. The mesh was exported from CFX and as far as I can see (in CFX-Post) without errors. I'm not allowed to share the mesh... Is it possible that small orthogonality angles cause this error? Is there a way to localize the reported face in the mesh?

Thanks in advance
Marco

[DSpreitz]

Hi all, Bonjour Martin,

I'm trying to install the CGNS tools, as described on the WIKI. I managed to install the CGSN converter, but I fail compiling the CGNS tools:

Please see my compile log below:
================================================== ====
~/OpenFOAM/user-1.5-dev/TurboMachinery/src/cgnstools_2.5/cgnstools ~/OpenFOAM/user-1.5-dev/TurboMachinery/src/cgnstools_2.5
loading cache ./config.cache
checking if gcc is requested... no
checking for cc... (cached) cc
checking whether the C compiler (cc ) works... yes
checking whether the C compiler (cc ) is a cross-compiler... no
checking whether we are using GNU C... (cached) yes
checking if compiler supports prototyping... yes
checking for object suffix... (cached) o
checking for Cygwin environment... (cached) no
checking for mingw32 environment... (cached) no
checking for executable suffix... (cached) no
checking if debugging is enabled... no
checking for ranlib... (cached) ranlib
checking for strip... (cached) strip
checking if CGNS directory was specified... ../../cgnslib_2.5
checking if system was specified... no
checking if 64bit support is requested... no
checking cgsystem... LINUX
checking if cutting plane is requested... yes
checking if mesh boundaries is requested... yes
checking for matherr in -lm... (cached) yes
checking return type of signal handlers... (cached) void
checking if ADFH directory was specified... not used
checking how to run the C preprocessor... (cached) cc -E
checking for X... (cached) libraries , headers
checking if Tcl directory was specified... no
checking if Tk directory was specified... no
checking for installed version of Tk... /usr/lib
checking for GL/gl.h... (cached) yes
checking for a BSD compatible install... (cached) /usr/bin/install -c
checking if multi-platform support is requested... no
checking where to install executables... /home/user/OpenFOAM/user-1.5-dev/TurboMachinery/src/cgnstools_2.5/cgnstools/platforms/linuxGccDPOpt/bin
checking where to install Tcl scripts... /home/user/OpenFOAM/user-1.5-dev/TurboMachinery/src/cgnstools_2.5/cgnstools/platforms/linuxGccDPOpt/share/cgnstools
checking whether make sets ${MAKE}... (cached) yes
Makefile already exists - renamed to Makefile.bak
make.defs already exists - renamed to make.defs.bak
cgconfig already exists - renamed to cgconfig.bak
creating ./config.status
creating Makefile
creating make.defs
creating cgconfig
----- adfviewer -----
make[1]: Entering directory `/home/user/OpenFOAM/user-1.5-dev/TurboMachinery/src/cgnstools_2.5/cgnstools/adfviewer'
cc -DPROTOTYPE -O2 -I../common -I/home/user/OpenFOAM/user-1.5-dev/TurboMachinery/src/cgnslib_2.5 -I/home/user/OpenFOAM/user-1.5-dev/TurboMachinery/src/cgnslib_2.5/adf -c adfwish.c
adfwish.c:15:16: error: tk.h: No such file or directory
--- snip --- snip --- snip ---
================================================== =============
I have following dependencies installed:
- autoconf (GNU Autoconf) 2.63
- automake (GNU automake) 1.10.2
- libtool 2.2.6
- tk8.4 & tk8.4-dev
- tcl8.4 & tcl8.4-dev
- tclx8.4 & tclx8.4-dev

The file tk.h resided in /usr/include/tcl8.4/tk.h and
user@pelican:/usr$ find /usr/ -name tkConfig.sh gives me
/usr/lib/tk8.4/tkConfig.sh
/usr/lib/tkConfig.sh
/usr/share/tcltk/tk8.4/tkConfig.sh

As I am running on a 32-bit machine, I changed following line in the Allwmake
make TKLIBS="-L/usr/lib -ltcl8.4 -ltk8.4" TKOGLXLIB="-L/usr/X11R6/lib -lXmu -lXext"
replacing lib64 by lib.
As a side note: I don't have a dir called /usr/X11R6/lib, but I do have the libx11-dev package installed and in the compile log I get "checking for X... libraries , headers".

I am running on Ubuntu 9.04 (Jaunty Jackalope).
As I am running out of ideas how to fix this problem, I would appreciate any help or suggestions, or feedback of people who managed to install the cgnstools on Ubuntu 9.04.

P.S.: I was able to successfully compile the cgnsToFoam converter and the tools and utilities in cgnstools as they don't depend on tk.h

Dominic

[marico]

Hi,

I had the same. You need to install the tcl/tk-things... Dont know how it works easiest on ubuntu, on openSuse I just could take Yast with one click.

Marco

[DSpreitz]

Hi Marco,
Thanks for you reply. Could you be a bit more specific in your reply?

Originally Posted by marico

Hi,
You need to install the tcl/tk-things...
Marco

I thought I had it all installed:
- tk8.4 & tk8.4-dev
- tcl8.4 & tcl8.4-dev
- tclx8.4 & tclx8.4-dev
What additional 'things' do you suggest? I made the installation of the CGNStools run under openSuse 10.3. Under Ubuntu I am still not able to install it. So help on this is still appreciated.

Regards
Dominic

[marico]

Hi,

sorry, I didnt read your post carefully.... Unfortunately I have no idea how to specify the directories for the compilation... Maybe you dont need the tools?!

Marco

[hamcer]

hello everyone,

I have a cgns file with 6 blocks, I have converted to OF with-separatePatches, the file boundary has shown that:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.4.1 |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "..";
case "case";
instance "constant";
local "polyMesh";

class polyBoundaryMesh;
object boundary;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

20
(
bc_3
{
type patch;
physicalType inlet;
nFaces 560;
startFace 195664;
}

bc_3
{
type patch;
physicalType inlet;
nFaces 560;
startFace 196224;
}

bc_4
{
type patch;
physicalType inlet;
nFaces 400;
startFace 196784;
}

bc_4
{
type patch;
physicalType outlet;
nFaces 560;
startFace 197184;
}

bc_4
{
type patch;
physicalType inlet;
nFaces 560;
startFace 197744;
}

bc_4
{
type patch;
physicalType inlet;
nFaces 400;
startFace 198304;
}

bc_4
{
type patch;
physicalType outlet;
nFaces 560;
startFace 198704;
}

bc_4
{
type patch;
physicalType inlet;
nFaces 560;
startFace 199264;
}

bc_5
{
type patch;
physicalType outlet;
nFaces 400;
startFace 199824;
}

bc_5
{
type patch;
physicalType outlet;
nFaces 560;
startFace 200224;
}

bc_5
{
type patch;
physicalType outlet;
nFaces 400;
startFace 200784;
}

bc_5
{
type patch;
physicalType outlet;
nFaces 560;
startFace 201184;
}

bc_6
{
type patch;
physicalType symmetryPlane;
nFaces 440;
startFace 201744;
}

bc_6
{
type wall;
physicalType wallFunctions;
nFaces 440;
startFace 202184;
}

bc_6
{
type patch;
physicalType symmetryPlane;
nFaces 440;
startFace 202624;
}

bc_6
{
type wall;
physicalType wallFunctions;
nFaces 440;
startFace 203064;
}

bc_7
{
type patch;
physicalType symmetryPlane;
nFaces 616;
startFace 203504;
}

bc_7
{
type wall;
physicalType wallFunctions;
nFaces 440;
startFace 204120;
}

bc_7
{
type wall;
physicalType wallFunctions;
nFaces 440;
startFace 204560;
}

bc_8
{
type patch;
physicalType symmetryPlane;
nFaces 616;
startFace 205000;
}
)

// ************************************************** *********************** //


After I put 20 patches by changing the names of bc_ as you can see:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.4.1 |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "..";
case "case";
instance "constant";
local "polyMesh";

class polyBoundaryMesh;
object boundary;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

20
(
bc_1
{
type patch;
physicalType inlet;
nFaces 560;
startFace 195664;
}

bc_2
{
type patch;
physicalType inlet;
nFaces 560;
startFace 196224;
}

bc_3
{
type patch;
physicalType inlet;
nFaces 400;
startFace 196784;
}

bc_4
{
type patch;
physicalType outlet;
nFaces 560;
startFace 197184;
}

bc_5
{
type patch;
physicalType inlet;
nFaces 560;
startFace 197744;
}

bc_6
{
type patch;
physicalType inlet;
nFaces 400;
startFace 198304;
}

bc_7
{
type patch;
physicalType outlet;
nFaces 560;
startFace 198704;
}

bc_8
{
type patch;
physicalType inlet;
nFaces 560;
startFace 199264;
}

bc_9
{
type patch;
physicalType outlet;
nFaces 400;
startFace 199824;
}

bc_10
{
type patch;
physicalType outlet;
nFaces 560;
startFace 200224;
}

bc_11
{
type patch;
physicalType outlet;
nFaces 400;
startFace 200784;
}

bc_12
{
type patch;
physicalType outlet;
nFaces 560;
startFace 201184;
}

bc_13
{
type symmetryPlane;
physicalType symmetryPlane;
nFaces 440;
startFace 201744;
}

bc_14
{
type wall;
physicalType wallFunctions;
nFaces 440;
startFace 202184;
}

bc_15
{
type symmetryPlane;
physicalType symmetryPlane;
nFaces 440;
startFace 202624;
}

bc_16
{
type wall;
physicalType wallFunctions;
nFaces 440;
startFace 203064;
}

bc_17
{
type symmetryPlane;
physicalType symmetryPlane;
nFaces 616;
startFace 203504;
}

bc_18
{
type wall;
physicalType wallFunctions;
nFaces 440;
startFace 204120;
}

bc_19
{
type wall;
physicalType wallFunctions;
nFaces 440;
startFace 204560;
}

bc_20
{
type symmetryPlane;
physicalType symmetryPlane;
nFaces 616;
startFace 205000;
}
)

// ************************************************** *********************** //



but when I start the calculation with simpleFoam it shows me this script:
(of course by completing the 0 files according the boundary file)

Exec : simpleFoam . case
Date : Jun 11 2009
Time : 10:53:38
Host : nrj1pc75
PID : 17854
Root : /home/users/hamdi/OpenFOAM/hamdi-1.4.1/run/tutorials/simpleFoam/grid6
Case : case
Nprocs : 1
Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model kEpsilon

Starting time loop

Time = 0.05

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xb7fc1400]
#3 void Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::Field<Foam::Vector<double> >&, Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so"
#4 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so"
#5 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::tmp<Foam::GeometricField<Foam::Vector<doub le>, Foam::fvsPatchField, Foam::surfaceMesh> > const&) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so"
#6 Foam::fv::gaussDivScheme<Foam::Tensor<double> >::fvcDiv(Foam::GeometricField<Foam::Tensor<double >, Foam::fvPatchField, Foam::volMesh> const&) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so"
#7 Foam::tmp<Foam::GeometricField<Foam::innerProduct< Foam::Vector<double>, Foam::Tensor<double> >::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div<Foam::Tensor<double> >(Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::word const&) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTurbulenceModels.so"
#8 Foam::tmp<Foam::GeometricField<Foam::innerProduct< Foam::Vector<double>, Foam::Tensor<double> >::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div<Foam::Tensor<double> >(Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh> const&) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTurbulenceModels.so"
#9 Foam::tmp<Foam::GeometricField<Foam::innerProduct< Foam::Vector<double>, Foam::Tensor<double> >::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div<Foam::Tensor<double> >(Foam::tmp<Foam::GeometricField<Foam::Tensor<doub le>, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTurbulenceModels.so"
#10 Foam::turbulenceModels::kEpsilon::divR(Foam::Geome tricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&) const in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTurbulenceModels.so"
#11 main in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/simpleFoam"
#12 __libc_start_main in "/lib/i686/cmov/libc.so.6"
#13 Foam::regIOobject::readIfModified() in "/home/users/hamdi/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/simpleFoam"
Exception en point flottant


any idea will be Welcome.

[DSpreitz]

Hey Hamdi,

Did you ever succeed in installing the CGNS tools under Ubuntu?
You did stop trying or did you find a solution? If so, could you please share your solution? I am stuck on the same problem.

Regards

Dominic

Originally Posted by mbeaudoin

Hello Hamdi,

The configure script for the cgnstools cannot find your local dev installation of Tcl/Tk.

From your previous post:


checking if Tcl directory was specified... no
checking if Tk directory was specified... no
checking for installed version of Tk... no
checking for local Tk distribution... no
configure: warning: couldn't find a tkConfig.sh
configure: warning: edit make.defs and set TKINCS and TKLIBS


This is why you get an error message about tk.h at compile time.

Please note that you don't need the cgnstools for running the cgns converters. The cgnstools are useful for viewing CGNS files. So you can safely skip that part.

If you really need the cgnstools, then let's try to run a couple of commands first:

find / -name tkConfig.sh
find / -name tk.h

Martin