[mesh manipulation] CreatePatch to create cyclic boundary

sbence · January 21, 2009, 18:23

Hi All!

I would need some help on the usage of the i{createPatch} utility.
I am calculating a straight pipe. I would like to create cyclic boundary conditions for the inlet and outlet. I have existing patches for the inlet "in", and outlet "out". I have created the mesh with CalculiX, so the files in the polyMesh directory (boundary, cells, faces, etc.) are existing already and there is no blockMeshDict file.

Here is the boundary file:
FoamFile
{
version 2.0;
format ascii;

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

class polyBoundaryMesh;
object boundary;
}

3
(
in
{
type cyclic;
nFaces 768;
startFace 224160;
}

out
{
type cyclic;
nFaces 768;
startFace 224928;
}

wall
{
type wall;
nFaces 6336;
startFace 225696;
}

)

Here is the createPatchDict file:
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.0 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "/home/bence/OpenFOAM/bence-1.5/run/practice/tube3/";
case "tube_turbulent_kEpsilon_HighRe-cyclic";
instance "system";
local "";

class dictionary;
object createPatcheDict;
}

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

// Tolerance used in matching faces. Absolute tolerance is span of
// face times this factor.
matchTolerance 1E-3;

// Do a synchronisation of coupled points.
pointSync true;

// Patches to create.
// If no patches does a coupled point and face synchronisation anyway.
patches
(
{
// Name of new patch
name io_cyclic;

// Type of new patch
type cyclic;

// How to construct: either 'patches' or 'set'
constructFrom patches;

// If constructFrom = patches : names of patches
patches (in out);

// If constructFrom = set : name of faceSet
//set f0;
}
);

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

Could somebody have a look at them?

Thanks in advance!

BR,
Bence

sbence · January 21, 2009, 18:54

I have changed the boundary file:
FoamFile
{
version 2.0;
format ascii;

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

class polyBoundaryMesh;
object boundary;
}

3
(
in
{
type patch;
nFaces 768;
startFace 224160;
}

out
{
type patch;
nFaces 768;
startFace 224928;
}

wall
{
type wall;
nFaces 6336;
startFace 225696;
}

)

Now my createPatch output looks the following:
Create time

Reading createPatchDict.

Using relative tolerance 0.001 to match up faces and points

Create polyMesh for time = 0

Adding new patch io_cyclic of type cyclic as patch 3

Moving faces from patch in to patch 3
Moving faces from patch out to patch 3

Doing topology modification to order faces.

#0 Foam::error::printStack(Foam:

stream&) in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xb7f80420]
#3 Foam::face::normal(Foam::Field<foam::vector<double > > const&) const in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/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/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 Foam::cyclicPolyPatch::order(Foam::PrimitivePatch< foam::face,> > const&, Foam::Vector<double> > const&, Foam::List<int>&, Foam::List<int>&) const in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/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/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/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/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so"
#8 Foam::polyTopoChange::changeMesh(Foam::polyMesh&, bool, bool, bool, bool) in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so"
#9 main in "/home/bence/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/createPatch"
#10 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#11 __gxx_personality_v0 in "/home/bence/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/createPatch"
Segmentation fault

Any help is appreciated!

BR,
Bence

sbence · January 27, 2009, 04:36

Solved meanwhile...

Bence

eriklarsson · February 12, 2009, 03:47

Dear Foamers

I also have problems with setting up my cyclic boundaries. I'm using 1.5-dev.

My mesh is simple and was made in ANSA and exported as a .msh. The case runs well with simpleFoam with both wall and symmetry BCs.

My /constant/polymesh/boundary is:
5
(
Right
{
type patch;
nFaces 2121;
startFace 122699;
}
wall
{
type patch;
nFaces 4040;
startFace 124820;
}
Left
{
type patch;
nFaces 2121;
startFace 128860;
}
Out
{
type patch;
nFaces 420;
startFace 130981;
}
In
{
type patch;
nFaces 420;
startFace 131401;
}
)}

And my createPatchDict is

matchTolerance 1E-7;
pointSync true;
patches
(
{
name LR_cyclic;
type cyclic;
constructFrom patches;
patches (Right Left);

}
);

This simply returns
Create time

Reading createPatchDict.

Using relative tolerance 1e-07 to match up faces and points

Create polyMesh for time = 0

Adding new patch LR_cyclic of type cyclic as patch 5

Moving faces from patch Right to patch 5
Moving faces from patch Left to patch 5

Doing topology modification to order faces.

Segmentation fault

I also tried setting /constant/polyMesh/boundary
Right
{
type cyclic;
separationOffset (0 0 0);
rotationAxis (1 0 0);
rotationAngle -60;
shadowPatch Left;
nFaces 2121;
startFace 122699;
}
Left
{
type cyclic;
separationOffset (0 0 0);
rotationAxis (1 0 0);
rotationAngle 60;
shadowPatch Right;
nFaces 2121;
startFace 128860;}

However, this only causes the soloution to diverge.

Can someone please give me some hints?

Bence, can you post your fix to the your problem?

Regards
Erik Larsson

mbeaudoin · February 12, 2009, 10:11

Hello Erik,

For your second example of the file /constant/polyMesh/boundary:

You are using a patch definition appropriate for a cyclicGgi, and not for a "standard" cyclic patch.

You might want to try using a cyclicGgi instead of the cyclic patch for your problem. The cyclicGgi can handle conformal patches as well.

Just make sure your rotation axis and rotation angle are properly defined. And also replace cyclic with cyclicGgi where needed.

Martin

saasebo · February 19, 2009, 06:33

Hello Bence,

Could I ask what the solution was to the segmentation fault error from createPatch above?

BR, Steinar

eriklarsson · February 19, 2009, 08:51

Dear Foamers,

I would just like to add that my rotation sngles in the cyclicGgi case were defined with the wrong sign, just as Beaudoin suggested. The cyclicGgi is working now.

Apparently, even with the rotation angles badly defined, OpenFOAM still solves for the velocities. In my case, it was not until the pressure loop that OpenFOAM returned "Floating exception".

Regards
Erik Larsson

obraun · February 20, 2009, 11:21

I would be interested in the solution of the segmentation fault too, it's just what happens to me... I will let you know if I find out...

obraun · February 20, 2009, 11:24

Hi all,

I would be interested in the solution of the segmentation fault too, it's just what happens to me... I will let you know if I find out...

Cheers

Olivier

crazysumi · February 24, 2009, 09:45

Dear Mr Somogyi,

In respect to your post dated "Wednesday, January 21, 2009" regarding the createPatch utility. I am also getting the same error 'segmentation fault' as you have reported.

Could you tell us how you resolved it.

Thanks
SK

mattijs · February 24, 2009, 17:46

Hello Erik,

createPatch should be able to create a cyclic from two non-cyclic patches and worked last time I tried in 1.5.x.
The faces have to match but don't have to be ordered. Report a bug in OpenFOAM-bugs if you have a testcase.

crazysumi · February 25, 2009, 05:27

Dear Mr Somogyi,

In respect to your post dated "Wednesday, January 21, 2009" regarding the createPatch utility. I am also getting the same error 'segmentation fault' as you have reported.

Could you tell us how you resolved it.

Thanks
SK

crazysumi · February 25, 2009, 06:24

My createPatchDict File :-
matchTolerance 1E-6;

// Do a synchronisation of coupled points.
pointSync true;

// Patches to create.
// If no patches does a coupled point and face synchronisation anyway.
patches
(
{
// Name of new patch
name periodic;

// Type of new patch
type cyclic;

// How to construct: either 'patches' or 'set'
constructFrom patches;

// If constructFrom = patches : names of patches
patches (periodic2 periodic1);

// If constructFrom = set : name of faceSet
//set f0;
}

On running the createPatch utility, the error messages I received:-

sm.kumar@linux:~/OpenFOAM/sm.kumar-1.5/Sumeet/Nozzle/Of_Nozzle> 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 : Feb 25 2009
Time : 16:41:47
Host : linux
PID : 27071
Case : /home/sm.kumar/OpenFOAM/sm.kumar-1.5/Sumeet/Nozzle/Of_Nozzle
nProcs : 1

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

Reading createPatchDict.

Using relative tolerance 1e-06 to match up faces and points

Create polyMesh for time = 0

Adding new patch periodic of type cyclic as patch 9

Moving faces from patch periodic2 to patch 9
Moving faces from patch periodic1 to patch 9

Doing topology modification to order faces.

#0 Foam::error::printStack(Foam:

stream&) 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,> > 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,> > 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::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/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#8 Foam::polyTopoChange::changeMesh(Foam::polyMesh&, 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/createPat ch"
#10 __libc_start_main in "/lib64/libc.so.6"
#11 __gxx_personality_v0 in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPat ch"
Segmentation fault

obraun · February 25, 2009, 08:36

Hi all,

http://www.cfd-online.com/OpenFOAM_D...tml?1222760531

http://www.cfd-online.com/OpenFOAM_D...s/1/10743.html

and as told by Mattijs this is supposed to be fixed in 1.5.x I am just having it compiled and looking forward to the problem being solved. I'll keep you informed.

Olivier

P.S.: The trickky thing was I did not get into this trouble with a rather coarse grid after declaring periodic/shadow pair in fluent and remerging this first as a normal patch and then decalring it as cyclic, must have been luck that no renumbering took place. So I thought it should work with a fine one, but for some spurious reasons the same procedure ended up in badly ordered faces and the segfault with the finer mesh.

obraun · February 25, 2009, 12:21

Confirm everything is fine with 1.5.x

waterboy · March 25, 2009, 07:10

Hi,
As I am using SHM to create a propeller mesh I can hardly guarantee that the two patches are equal when it comes to face size. In general it should be possible to interpolate from one patch to the other although there are different face sizes, just like mapFields does it, or not?
Has anyone already tried and succeeded in using "different" patches? Bence tried it according to his boundary file, right?
Any hints welcome,
Pal

Fonss · July 26, 2009, 15:51

It looks like I have that problem.

$ 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 : Jul 26 2009
Time : 11:38:16
Host : Studio
PID : 14494
Case : /home/alfo/Desktop/Foam_run/test_1
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 fan1 of type cyclic as patch 3

Moving faces from patch fan_in to patch 3
Moving faces from patch fan_out to patch 3

Doing topology modification to order faces.

cyclicPolyPatch::getGeometricHalves : Writing half0 faces to OBJ file "/home/alfo/Desktop/Foam_run/test_1/fan1_half0_faces.obj"
cyclicPolyPatch::getGeometricHalves : Writing half1 faces to OBJ file "/home/alfo/Desktop/Foam_run/test_1/fan1_half1_faces.obj"
cyclicPolyPatch::getGeometricHalves : Writing half0 face centres to OBJ file "/home/alfo/Desktop/Foam_run/test_1/fan1_half0.obj"
cyclicPolyPatch::getGeometricHalves : Writing half1 face centres to OBJ file "/home/alfo/Desktop/Foam_run/test_1/fan1_half1.obj"
--> FOAM Serious Error :
From function cyclicPolyPatch::getGeometricHalves(const primitivePatch&, labelList&, labelList&) const
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 362
Patch fan1 gets decomposed in two zones ofinequal size: 347 and 377
This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp.
Please adapt the featureCos setting.
Continuing with incorrect face ordering from now on!

face 0 area does not match neighbour 362 by 2.06188% -- possible face ordering problem.
patch:fan1 my area:5.01411 neighbour area:5.11857 matching tolerance:0.001
Mesh face:26040 vertices:3((0 0 -50.9467) (0 0 -47.6196) (3.0141 0 -49.577))
Neighbour face:26402 vertices:3((3.136 3 -22.1557) (2.19942 3 -26.0631) (4.92856 3 -25.6075))
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

alfo@Studio:~/Desktop/Foam_run/test_1$ couplePatches
bash: couplePatches: command not found

I was just trying to use this command because some people suggested that couplePatches might do something... maybe but its not there. I'm going to have to try to recompile the 1.5.x again. The first time it did not work.

ouafa · August 17, 2009, 09:35

Quote:

Originally Posted by obraun

Confirm everything is fine with 1.5.x

Hi,

I have modified the cavity case to a real cube with front and back patches in order to make a cyclic condition with the createPatch tool later. The mesh seems to be fine.
The createPatchDict looks like this:

matchTolerance 1E-3;
pointSync true;

patches
({name inout;
type cyclic;
constructFrom patches;
patches (inlet outlet);
});

I am also getting the same error 'segmentation fault' as you have reported. i try to use developpement version but i can't see any difference between the two createPatch files.

Doing topology modification to order faces.

#0 Foam::error: rintStack(Foam::Ostream&) in "/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"

#1 Foam::sigSegv::sigSegvHandler(int) in "/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"

#2 __restore_rt at sigaction.c:0

#3 Foam::face::normal(Foam::Field<Foam::Vector<double > > const&) const in "/ 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 "/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"

#5 Foam::cyclicPolyPatch:rder(Foam::PrimitivePatch<Fo am::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::List<int>&, Foam::List<int>&) const in /OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"

#6 Foam

lyTopoChange::reorderCoupledFaces(bool, Foam

lyBoundaryMesh const&, Foam::List<int> const&, Foam::List<int> const&, Foam::Field<Foam::Vector<double> > const&) in "/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"

#7 Foam:

olyTopoChange::compactAndReorder(Foam:

oly 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 /OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"

#8 Foam:

olyTopoChange::changeMesh(Foam:

olyMesh&, bool, bool, bool, bool) in "/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"

#9 main in "/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPatch"
#10 __libc_start_main in "/lib64/libc.so.6"

#11 __gxx_personality_v0 in "/home/flurec/commun/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPatch"

Erreur de segmentation

Thanks in advance for help!
Ouafa

JackW · August 30, 2012, 06:51

Hi,

Probably not much help, but when I get a seg fault at the topology stage when I run createPatch, It is because I am trying to create it from the wrong patches or ones that I have already used (an artifact from copying and pasting carelessness), so the topology doesn't match.

January 21, 2009, 18:54	I have changed the boundary fi	#2
sbence New Member Bence Somogyi Join Date: Mar 2009 Location: Mattighofen, Austria Posts: 11 Rep Power: 17	I have changed the boundary file: FoamFile { version 2.0; format ascii; root ".."; case "."; instance "constant"; local "polyMesh"; class polyBoundaryMesh; object boundary; } 3 ( in { type patch; nFaces 768; startFace 224160; } out { type patch; nFaces 768; startFace 224928; } wall { type wall; nFaces 6336; startFace 225696; } ) Now my createPatch output looks the following: Create time Reading createPatchDict. Using relative tolerance 0.001 to match up faces and points Create polyMesh for time = 0 Adding new patch io_cyclic of type cyclic as patch 3 Moving faces from patch in to patch 3 Moving faces from patch out to patch 3 Doing topology modification to order faces. #0 Foam::error::printStack(Foam:stream&) in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigSegv::sigSegvHandler(int) in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0xb7f80420] #3 Foam::face::normal(Foam::Field<foam::vector<double > > const&) const in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/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/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #5 Foam::cyclicPolyPatch::order(Foam::PrimitivePatch< foam::face,> > const&, Foam::Vector<double> > const&, Foam::List<int>&, Foam::List<int>&) const in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/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/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/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/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so" #8 Foam::polyTopoChange::changeMesh(Foam::polyMesh&, bool, bool, bool, bool) in "/home/bence/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so" #9 main in "/home/bence/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/createPatch" #10 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #11 __gxx_personality_v0 in "/home/bence/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/createPatch" Segmentation fault Any help is appreciated! BR, Bence

February 12, 2009, 10:11	Hello Erik, For your second	#5
mbeaudoin Senior Member Martin Beaudoin Join Date: Mar 2009 Posts: 332 Rep Power: 22	Hello Erik, For your second example of the file /constant/polyMesh/boundary: You are using a patch definition appropriate for a cyclicGgi, and not for a "standard" cyclic patch. You might want to try using a cyclicGgi instead of the cyclic patch for your problem. The cyclicGgi can handle conformal patches as well. Just make sure your rotation axis and rotation angle are properly defined. And also replace cyclic with cyclicGgi where needed. Martin zxj160 likes this.

February 25, 2009, 05:27	Dear Mr Somogyi, In respect	#12
crazysumi New Member Sumeet Kumar Join Date: Mar 2009 Posts: 21 Rep Power: 17	Dear Mr Somogyi, In respect to your post dated "Wednesday, January 21, 2009" regarding the createPatch utility. I am also getting the same error 'segmentation fault' as you have reported. Could you tell us how you resolved it. Thanks SK

February 25, 2009, 06:24	My createPatchDict File :- ma	#13
crazysumi New Member Sumeet Kumar Join Date: Mar 2009 Posts: 21 Rep Power: 17	My createPatchDict File :- matchTolerance 1E-6; // Do a synchronisation of coupled points. pointSync true; // Patches to create. // If no patches does a coupled point and face synchronisation anyway. patches ( { // Name of new patch name periodic; // Type of new patch type cyclic; // How to construct: either 'patches' or 'set' constructFrom patches; // If constructFrom = patches : names of patches patches (periodic2 periodic1); // If constructFrom = set : name of faceSet //set f0; } On running the createPatch utility, the error messages I received:- sm.kumar@linux:~/OpenFOAM/sm.kumar-1.5/Sumeet/Nozzle/Of_Nozzle> 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 : Feb 25 2009 Time : 16:41:47 Host : linux PID : 27071 Case : /home/sm.kumar/OpenFOAM/sm.kumar-1.5/Sumeet/Nozzle/Of_Nozzle nProcs : 1 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Reading createPatchDict. Using relative tolerance 1e-06 to match up faces and points Create polyMesh for time = 0 Adding new patch periodic of type cyclic as patch 9 Moving faces from patch periodic2 to patch 9 Moving faces from patch periodic1 to patch 9 Doing topology modification to order faces. #0 Foam::error::printStack(Foam:stream&) 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,> > 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,> > 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::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/sm.kumar/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so" #8 Foam::polyTopoChange::changeMesh(Foam::polyMesh&, 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/createPat ch" #10 __libc_start_main in "/lib64/libc.so.6" #11 __gxx_personality_v0 in "/home/sm.kumar/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/createPat ch" Segmentation fault

February 25, 2009, 08:36	Hi all, http://www.cfd-onl	#14
obraun New Member olivier braun Join Date: Mar 2009 Location: Lausanne, Switzerland Posts: 19 Rep Power: 17	Hi all, http://www.cfd-online.com/OpenFOAM_D...tml?1222760531 http://www.cfd-online.com/OpenFOAM_D...s/1/10743.html and as told by Mattijs this is supposed to be fixed in 1.5.x I am just having it compiled and looking forward to the problem being solved. I'll keep you informed. Olivier P.S.: The trickky thing was I did not get into this trouble with a rather coarse grid after declaring periodic/shadow pair in fluent and remerging this first as a normal patch and then decalring it as cyclic, must have been luck that no renumbering took place. So I thought it should work with a fine one, but for some spurious reasons the same procedure ended up in badly ordered faces and the segfault with the finer mesh.

January 21, 2009, 18:23	CreatePatch to create cyclic boundary	#1
sbence New Member Bence Somogyi Join Date: Mar 2009 Location: Mattighofen, Austria Posts: 11 Rep Power: 17	Hi All! I would need some help on the usage of the i{createPatch} utility. I am calculating a straight pipe. I would like to create cyclic boundary conditions for the inlet and outlet. I have existing patches for the inlet "in", and outlet "out". I have created the mesh with CalculiX, so the files in the polyMesh directory (boundary, cells, faces, etc.) are existing already and there is no blockMeshDict file. Here is the boundary file: FoamFile { version 2.0; format ascii; root ".."; case "."; instance "constant"; local "polyMesh"; class polyBoundaryMesh; object boundary; } 3 ( in { type cyclic; nFaces 768; startFace 224160; } out { type cyclic; nFaces 768; startFace 224928; } wall { type wall; nFaces 6336; startFace 225696; } ) Here is the createPatchDict file: /---------------------------------------------------------------------------\ \| ========= \| \| \| \ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \ / O peration \| Version: 1.0 \| \| \ / A nd \| Web: http://www.openfoam.org \| \| \/ M anipulation \| \| \---------------------------------------------------------------------------/ FoamFile { version 2.0; format ascii; root "/home/bence/OpenFOAM/bence-1.5/run/practice/tube3/"; case "tube_turbulent_kEpsilon_HighRe-cyclic"; instance "system"; local ""; class dictionary; object createPatcheDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Tolerance used in matching faces. Absolute tolerance is span of // face times this factor. matchTolerance 1E-3; // Do a synchronisation of coupled points. pointSync true; // Patches to create. // If no patches does a coupled point and face synchronisation anyway. patches ( { // Name of new patch name io_cyclic; // Type of new patch type cyclic; // How to construct: either 'patches' or 'set' constructFrom patches; // If constructFrom = patches : names of patches patches (in out); // If constructFrom = set : name of faceSet //set f0; } ); // ************************************************ ********************* // Could somebody have a look at them? Thanks in advance! BR, Bence

January 27, 2009, 04:36	Solved meanwhile... Bence	#3
sbence New Member Bence Somogyi Join Date: Mar 2009 Location: Mattighofen, Austria Posts: 11 Rep Power: 17	Solved meanwhile... Bence

February 12, 2009, 03:47	Dear Foamers I also have pr	#4
eriklarsson New Member Erik Larsson Join Date: Mar 2009 Location: Göteborg, Sweden Posts: 2 Rep Power: 0	Dear Foamers I also have problems with setting up my cyclic boundaries. I'm using 1.5-dev. My mesh is simple and was made in ANSA and exported as a .msh. The case runs well with simpleFoam with both wall and symmetry BCs. My /constant/polymesh/boundary is: 5 ( Right { type patch; nFaces 2121; startFace 122699; } wall { type patch; nFaces 4040; startFace 124820; } Left { type patch; nFaces 2121; startFace 128860; } Out { type patch; nFaces 420; startFace 130981; } In { type patch; nFaces 420; startFace 131401; } )} And my createPatchDict is matchTolerance 1E-7; pointSync true; patches ( { name LR_cyclic; type cyclic; constructFrom patches; patches (Right Left); } ); This simply returns Create time Reading createPatchDict. Using relative tolerance 1e-07 to match up faces and points Create polyMesh for time = 0 Adding new patch LR_cyclic of type cyclic as patch 5 Moving faces from patch Right to patch 5 Moving faces from patch Left to patch 5 Doing topology modification to order faces. Segmentation fault I also tried setting /constant/polyMesh/boundary Right { type cyclic; separationOffset (0 0 0); rotationAxis (1 0 0); rotationAngle -60; shadowPatch Left; nFaces 2121; startFace 122699; } Left { type cyclic; separationOffset (0 0 0); rotationAxis (1 0 0); rotationAngle 60; shadowPatch Right; nFaces 2121; startFace 128860;} However, this only causes the soloution to diverge. Can someone please give me some hints? Bence, can you post your fix to the your problem? Regards Erik Larsson

February 19, 2009, 06:33	Hello Bence, Could I ask wh	#6
saasebo New Member Steinar Aasebø Join Date: Mar 2009 Posts: 13 Rep Power: 17	Hello Bence, Could I ask what the solution was to the segmentation fault error from createPatch above? BR, Steinar

February 19, 2009, 08:51	Dear Foamers, I would just	#7
eriklarsson New Member Erik Larsson Join Date: Mar 2009 Location: Göteborg, Sweden Posts: 2 Rep Power: 0	Dear Foamers, I would just like to add that my rotation sngles in the cyclicGgi case were defined with the wrong sign, just as Beaudoin suggested. The cyclicGgi is working now. Apparently, even with the rotation angles badly defined, OpenFOAM still solves for the velocities. In my case, it was not until the pressure loop that OpenFOAM returned "Floating exception". Regards Erik Larsson

February 20, 2009, 11:21	I would be interested in the s	#8
obraun New Member olivier braun Join Date: Mar 2009 Location: Lausanne, Switzerland Posts: 19 Rep Power: 17	I would be interested in the solution of the segmentation fault too, it's just what happens to me... I will let you know if I find out...

February 20, 2009, 11:24	Hi all, I would be interest	#9
obraun New Member olivier braun Join Date: Mar 2009 Location: Lausanne, Switzerland Posts: 19 Rep Power: 17	Hi all, I would be interested in the solution of the segmentation fault too, it's just what happens to me... I will let you know if I find out... Cheers Olivier

February 24, 2009, 09:45	Dear Mr Somogyi, In respect	#10
crazysumi New Member Sumeet Kumar Join Date: Mar 2009 Posts: 21 Rep Power: 17	Dear Mr Somogyi, In respect to your post dated "Wednesday, January 21, 2009" regarding the createPatch utility. I am also getting the same error 'segmentation fault' as you have reported. Could you tell us how you resolved it. Thanks SK

February 24, 2009, 17:46	Hello Erik, createPatch sho	#11
mattijs Senior Member Mattijs Janssens Join Date: Mar 2009 Posts: 1,419 Rep Power: 26	Hello Erik, createPatch should be able to create a cyclic from two non-cyclic patches and worked last time I tried in 1.5.x. The faces have to match but don't have to be ordered. Report a bug in OpenFOAM-bugs if you have a testcase.

February 25, 2009, 12:21	Confirm everything is fine wit	#15
obraun New Member olivier braun Join Date: Mar 2009 Location: Lausanne, Switzerland Posts: 19 Rep Power: 17	Confirm everything is fine with 1.5.x

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Out File does not show Imbalance in %	Mmaragann	CFX	5	January 20, 2017 10:20
Wrong flow in ratating domain problem	Sanyo	CFX	17	August 15, 2015 06:20
Possible createPatch/createBaffles bug?	simpomann	OpenFOAM Bugs	2	July 15, 2014 07:07
Radiation interface	hinca	CFX	15	January 26, 2014 17:11
Question about heat transfer coefficient setting for CFX	Anna Tian	CFX	1	June 16, 2013 06:28

March 25, 2009, 07:10	Face size important for cyclic	#16
waterboy New Member Pal Schmitt Join Date: Mar 2009 Posts: 28 Rep Power: 17	Hi, As I am using SHM to create a propeller mesh I can hardly guarantee that the two patches are equal when it comes to face size. In general it should be possible to interpolate from one patch to the other although there are different face sizes, just like mapFields does it, or not? Has anyone already tried and succeeded in using "different" patches? Bence tried it according to his boundary file, right? Any hints welcome, Pal

July 26, 2009, 15:51		#17
Fonss New Member Poncho Join Date: Mar 2009 Posts: 6 Rep Power: 17	It looks like I have that problem. $ 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 : Jul 26 2009 Time : 11:38:16 Host : Studio PID : 14494 Case : /home/alfo/Desktop/Foam_run/test_1 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 fan1 of type cyclic as patch 3 Moving faces from patch fan_in to patch 3 Moving faces from patch fan_out to patch 3 Doing topology modification to order faces. cyclicPolyPatch::getGeometricHalves : Writing half0 faces to OBJ file "/home/alfo/Desktop/Foam_run/test_1/fan1_half0_faces.obj" cyclicPolyPatch::getGeometricHalves : Writing half1 faces to OBJ file "/home/alfo/Desktop/Foam_run/test_1/fan1_half1_faces.obj" cyclicPolyPatch::getGeometricHalves : Writing half0 face centres to OBJ file "/home/alfo/Desktop/Foam_run/test_1/fan1_half0.obj" cyclicPolyPatch::getGeometricHalves : Writing half1 face centres to OBJ file "/home/alfo/Desktop/Foam_run/test_1/fan1_half1.obj" --> FOAM Serious Error : From function cyclicPolyPatch::getGeometricHalves(const primitivePatch&, labelList&, labelList&) const in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 362 Patch fan1 gets decomposed in two zones ofinequal size: 347 and 377 This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp. Please adapt the featureCos setting. Continuing with incorrect face ordering from now on! face 0 area does not match neighbour 362 by 2.06188% -- possible face ordering problem. patch:fan1 my area:5.01411 neighbour area:5.11857 matching tolerance:0.001 Mesh face:26040 vertices:3((0 0 -50.9467) (0 0 -47.6196) (3.0141 0 -49.577)) Neighbour face:26402 vertices:3((3.136 3 -22.1557) (2.19942 3 -26.0631) (4.92856 3 -25.6075)) 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 alfo@Studio:~/Desktop/Foam_run/test_1$ couplePatches bash: couplePatches: command not found I was just trying to use this command because some people suggested that couplePatches might do something... maybe but its not there. I'm going to have to try to recompile the 1.5.x again. The first time it did not work.

August 30, 2012, 06:51		#19
JackW Member Jack Join Date: Aug 2012 Posts: 47 Rep Power: 13	Hi, Probably not much help, but when I get a seg fault at the topology stage when I run createPatch, It is because I am trying to create it from the wrong patches or ones that I have already used (an artifact from copying and pasting carelessness), so the topology doesn't match.