 |
 |
 |
|
|
|
[Sponsors] | ||||
May 28, 2013, 13:02
|
simpleFoam crushes at 1st Time loop.
|
#1 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14  |
Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : simpleFoam
Date : May 28 2013
Time : 17:49:50
Host : "seav-eME730G"
PID : 17447
Case : /home/seav/oFOAM/c1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create mesh for time = 0
Reading field p
Reading field U
Reading/calculating face flux field phi
Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}
Creating finite volume options
No finite volume options present
SIMPLE: no convergence criteria found. Calculations will run for 100 steps.
Starting time loop
Time = 1
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#11 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#13
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#14 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p
{
solver GAMG;
tolerance 1e-08;
relTol 0.05;
smoother GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
}
U
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.1;
}
k
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.1;
}
epsilon
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.1;
}
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
convergenceCriterion 1.0e-6;
}
relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.5;
k 0.5;
epsilon 0.5;
}
}
// ************************************************************************* //
As I`ve posted up I have strange error and i dont have clue how to repair it. I seek for help in this case. Arthur. Last edited by seav; May 29, 2013 at 11:43. |
|
|
|
|
|
May 28, 2013, 13:49
|
|
#2 |
|
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 24 |
Hello Arthur,
Welcome to the forum! You will need to post a bit more information about your case before anyone can really help you out. Else it will be just guessing for the cause of the error (boundary conditions, initial conditions, mesh quality, ...) So briefly explain what you are simulating, give a description of the mesh (e.g. using checkMesh-output), summarize your boundary conditions and initial conditions, ... Cheers, Lieven |
|
|
|
|
|
|
May 28, 2013, 14:20
|
|
#3 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
Code:
$checkMesh Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : checkMesh
Date : May 28 2013
Time : 18:56:29
Host : "seav-eME730G"
PID : 19145
Case : /home/seav/oFOAM/c1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 0
Time = 0
Mesh stats
points: 198319
faces: 491700
internal faces: 402300
cells: 149000
faces per cell: 6
boundary patches: 14
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 149000
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0
Checking topology...
Boundary definition OK.
***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
*Number of regions: 149
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
in_gora 100 121 ok (non-closed singly connected)
out_gora 100 121 ok (non-closed singly connected)
in_dol 100 121 ok (non-closed singly connected)
out_dol 100 121 ok (non-closed singly connected)
bloki_obliczeniowe 11800 14278 ok (non-closed singly connected)
podstawaDol1 100 121 ok (non-closed singly connected)
podstawaDol2 100 121 ok (non-closed singly connected)
metalStripDol 100 121 ok (non-closed singly connected)
metalStripGora 100 121 ok (non-closed singly connected)
metalStripS1 100 121 ok (non-closed singly connected)
metalStripS2 100 121 ok (non-closed singly connected)
podstawaGora1 100 121 ok (non-closed singly connected)
podstawaGora2 100 121 ok (non-closed singly connected)
defaultFaces 76400 78908 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (0 0 0) (0.45 0.0115 0.14)
Mesh (non-empty, non-wedge) directions (0 0 0)
Mesh (non-empty) directions (0 0 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (5.85253e-18 -1.13453e-16 1.21199e-18) OK.
Max cell openness = 1.32349e-16 OK.
Max aspect ratio = -1 OK.
Minimum face area = 5e-08. Maximum face area = 0.00063. Face area magnitudes OK.
Min volume = 1.11665e-10. Max volume = 3.36e-08. Total volume = 0.0007236. Cell volumes OK.
Mesh non-orthogonality Max: 0 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 2.23882e-05 OK.
Coupled point location match (average 0) OK.
Mesh OK.
End
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class polyBoundaryMesh;
location "constant/polyMesh";
object boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
14
(
in_gora
{
type patch;
nFaces 100;
startFace 402300;
}
out_gora
{
type patch;
nFaces 100;
startFace 402400;
}
in_dol
{
type patch;
nFaces 100;
startFace 402500;
}
out_dol
{
type patch;
nFaces 100;
startFace 402600;
}
bloki_obliczeniowe
{
type empty;
inGroups 1(empty);
nFaces 11800;
startFace 402700;
}
podstawaDol1
{
type wall;
nFaces 100;
startFace 414500;
}
podstawaDol2
{
type wall;
nFaces 100;
startFace 414600;
}
metalStripDol
{
type wall;
nFaces 100;
startFace 414700;
}
metalStripGora
{
type wall;
nFaces 100;
startFace 414800;
}
metalStripS1
{
type wall;
nFaces 100;
startFace 414900;
}
metalStripS2
{
type wall;
nFaces 100;
startFace 415000;
}
podstawaGora1
{
type wall;
nFaces 100;
startFace 415100;
}
podstawaGora2
{
type wall;
nFaces 100;
startFace 415200;
}
defaultFaces
{
type empty;
inGroups 1(empty);
nFaces 76400;
startFace 415300;
}
)
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) Gauss linear;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss limitedLinearV 1;
div(phi,k) bounded Gauss limitedLinear 1;
div(phi,epsilon) bounded Gauss limitedLinear 1;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
}
interpolationSchemes
{
default linear;
interpolate(U) linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p ;
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p
{
solver GAMG;
tolerance 1e-08;
relTol 0.05;
smoother GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
}
U
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.1;
}
k
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.1;
}
epsilon
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.1;
}
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
convergenceCriterion 1.0e-6;
}
relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.5;
k 0.5;
epsilon 0.5;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application simpleFoam;
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 100;
deltaT 1;
writeControl timeStep;
writeInterval 50;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
RASModel kEpsilon;
turbulence on;
printCoeffs on;
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1e-05;
CrossPowerLawCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
m m [ 0 0 1 0 0 0 0 ] 1;
n n [ 0 0 0 0 0 0 0 ] 1;
}
BirdCarreauCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
k k [ 0 0 1 0 0 0 0 ] 0;
n n [ 0 0 0 0 0 0 0 ] 1;
}
// ************************************************************************* //
I want to solve numerical simulation of convection heat transfer. To do this I use blockMesh and simpleFoam. However I got error which i posted in my last and first post in the same time  . For now long I am out off ideas what goes wrong.If you need anything else to analyse my problem, just say. Arthur. |
|
|
|
|
|
|
May 28, 2013, 15:01
|
|
#4 |
|
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 24 |
Hi Arthur,
There is something strange going on in your mesh. The checkMesh-utility reports that the mesh is 3D (i.e. not 1D or 2D), yet you define an empty patch somewhere... This is only used for 2D cases (maybe it also works for 1D, don't know, anyway not the point). So could be post your blockmesh-file and a sketch of the geometry you want to draw cause I have the strong impression it is a mesh-related issue. Cheers, L |
|
|
|
|
|
|
May 28, 2013, 19:28
|
|
#5 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
Hi Leiven, thank you for your response.
My blockMeshDict file is heavy one and excceds line limit. Sketch won`t show main problem with geometry, I mean the geometery is "sticky". I will try to show this file. I do define empty patch. I looked up into pitzDaily tutorial from simpleFoam tutorials folder. Cheers, Arthur. |
|
|
|
|
|
|
May 29, 2013, 09:32
|
|
#6 |
|
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 24 |
Normally you should be able to attach the file to the post without having to embed it in the text.
Can you explain a bit why you define the empty patch? It is indeed done in the simpleFoam tutorial but this is simply cause the tutorial is 2D. Cheers, L |
|
|
|
|
|
|
May 29, 2013, 11:06
|
|
#7 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
Hi, Lieven.
Yes I did attachment. Here is a file, however its with *.c extension. I assume you have change it. I think I didnt understand documentation properly. And you have right about difference 1D 2D and 3D with empty patch. To notice what problem comes with geometery please use paraFoam -block and uncheck first three blocks before creating mesh. Cheers, Arthur. |
|
|
|
|
|
|
May 29, 2013, 11:12
|
|
#8 |
|
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 24 |
That's a very big blockMeshDict file
 But this confirms a bit my suspicion, the empty-patch should be defined for a 3D mesh. So I would recommend you to read the manual and try to correct the file. Good luck, Lieven |
|
|
|
|
|
|
May 29, 2013, 11:41
|
|
#9 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
I did change empty patch to wall. In fact I dont know why I didnt do this at first.
However, it didnt solve my problem : Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : simpleFoam
Date : May 29 2013
Time : 16:20:43
Host : "seav-eME730G"
PID : 3462
Case : /home/seav/oFOAM/c1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create mesh for time = 0
Reading field p
Reading field U
Reading/calculating face flux field phi
Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}
Creating finite volume options
No finite volume options present
SIMPLE: no convergence criteria found. Calculations will run for 100 steps.
Starting time loop
Time = 1
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#11 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#13
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#14 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
Code:
No finite volume options present SIMPLE: no convergence criteria found. Calculations will run for 100 steps. .Arthur. |
|
|
|
|
|
|
May 29, 2013, 11:44
|
|
#10 |
|
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 24 |
This is no problem
Code:
No finite volume options present SIMPLE: no convergence criteria found. Calculations will run for 100 steps. Cheers, L |
|
|
|
|
|
|
May 29, 2013, 13:02
|
|
#11 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
I found this : http://www.cfd-online.com/Forums/ope...ion-1-6-a.html
With similar problem with mine... so I used ; Code:
refineMesh -overwrite checkMesh: Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : checkMesh
Date : May 29 2013
Time : 18:00:02
Host : "seav-eME730G"
PID : 4262
Case : /home/seav/oFOAM/c1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 0
Time = 0
Mesh stats
points: 1379889
faces: 3754800
internal faces: 3397200
cells: 1192000
faces per cell: 6
boundary patches: 14
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 1192000
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0
Checking topology...
Boundary definition OK.
***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
*Number of regions: 149
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
in_gora 400 441 ok (non-closed singly connected)
out_gora 400 441 ok (non-closed singly connected)
in_dol 400 441 ok (non-closed singly connected)
out_dol 400 441 ok (non-closed singly connected)
bloki_obliczeniowe 47200 52038 ok (non-closed singly connected)
podstawaDol1 400 441 ok (non-closed singly connected)
podstawaDol2 400 441 ok (non-closed singly connected)
metalStripDol 400 441 ok (non-closed singly connected)
metalStripGora 400 441 ok (non-closed singly connected)
metalStripS1 400 441 ok (non-closed singly connected)
metalStripS2 400 441 ok (non-closed singly connected)
podstawaGora1 400 441 ok (non-closed singly connected)
podstawaGora2 400 441 ok (non-closed singly connected)
defaultFaces 305600 310428 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (0 0 0) (0.45 0.0115 0.14)
Mesh (non-empty, non-wedge) directions (0 0 0)
Mesh (non-empty) directions (0 0 0)
***Number of edges not aligned with or perpendicular to non-empty directions: 36118
<<Writing 36321 points on non-aligned edges to set nonAlignedEdges
Boundary openness (6.90913e-18 4.22973e-17 -7.64549e-19) OK.
Max cell openness = 1.89637e-16 OK.
Max aspect ratio = -1 OK.
Minimum face area = 1.25e-08. Maximum face area = 0.0001575. Face area magnitudes OK.
Min volume = 1.395e-11. Max volume = 4.2e-09. Total volume = 0.0007236. Cell volumes OK.
Mesh non-orthogonality Max: 0.572747 average: 0.0218034
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.000223949 OK.
Coupled point location match (average 0) OK.
Failed 1 mesh checks.
End
Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : simpleFoam
Date : May 29 2013
Time : 18:01:17
Host : "seav-eME730G"
PID : 4263
Case : /home/seav/Pulpit/mgr/mgr
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create mesh for time = 0
Reading field p
Reading field U
Reading/calculating face flux field phi
Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}
Creating finite volume options
No finite volume options present
SIMPLE: no convergence criteria found. Calculations will run for 100 steps.
Starting time loop
Time = 1
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#11 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#13
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#14 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
Błąd w obliczeniach zmiennoprzecinkowych (core dumped)
|
|
|
|
|
|
|
May 29, 2013, 13:23
|
|
#12 |
|
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 24 |
Dear Arthur,
I still have the impressing a number of empty faces are defined in the blockMeshDict (based on the checkMesh output). Second, there is also the Code:
The mesh has multiple regions which are not connected by any face. Therefore, I would recommend you to start from a simplified blockMeshDict and gradually introduce the more complex parts. Make it as simplified as needed for simpleFoam to run. Cheers, Lieven |
|
|
|
|
|
|
May 29, 2013, 16:47
|
|
#13 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
Lieven, you have right.
I was so focused on initial and boundary conditions that I missed bugs in my blockMeshDict. I will fix this as fast as possible. If you are ok with that I am asking you to suscribe this thread. I dont want to create multiple threads. I just "smell" errors before they happened. I am start fixing mesh. I will post the results. A. Last edited by seav; May 29, 2013 at 21:24. |
|
|
|
|
|
|
May 29, 2013, 18:30
|
|
#14 |
|
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 24 |
Ok, have fun
|
|
|
|
|
|
|
June 1, 2013, 08:00
|
|
#15 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
blockMesh
Code:
Creating block mesh topology
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 901
Found 4 undefined faces in mesh; adding to default patch.
Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : checkMesh
Date : Jun 01 2013
Time : 12:46:19
Host : "seav-eME730G"
PID : 6380
Case : /home/seav/oFOAM/c1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 0
Time = 0
Mesh stats
points: 296329
faces: 770700
internal faces: 663300
cells: 239000
faces per cell: 6
boundary patches: 16
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 239000
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0
Checking topology...
Boundary definition OK.
***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
*Number of regions: 59
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
in_gora 100 121 ok (non-closed singly connected)
out_gora 100 121 ok (non-closed singly connected)
in_dol 100 121 ok (non-closed singly connected)
out_dol 100 121 ok (non-closed singly connected)
face_plyn 58000 63844 ok (non-closed singly connected)
face_plyn_zewnetrzne11800 14278 ok (non-closed singly connected)
face_przeszkody 36000 39600 ok (non-closed singly connected)
podstawaDol1 100 121 ok (non-closed singly connected)
podstawaDol2 100 121 ok (non-closed singly connected)
metalStripDol 100 121 ok (non-closed singly connected)
metalStripGora 100 121 ok (non-closed singly connected)
metalStripS1 100 121 ok (non-closed singly connected)
metalStripS2 100 121 ok (non-closed singly connected)
podstawaGora1 100 121 ok (non-closed singly connected)
podstawaGora2 100 121 ok (non-closed singly connected)
defaultFaces 400 484 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (0 0 0) (0.45 0.0115 0.14)
Mesh (non-empty, non-wedge) directions (0 1 1)
Mesh (non-empty) directions (0 1 1)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (-1.83771e-19 4.61985e-18 1.2634e-18) OK.
Max cell openness = 1.65436e-16 OK.
Max aspect ratio = 280 OK.
Minimum face area = 4e-08. Maximum face area = 0.00063. Face area magnitudes OK.
Min volume = 1e-11. Max volume = 3.36e-08. Total volume = 0.0007245. Cell volumes OK.
Mesh non-orthogonality Max: 0 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.000249975 OK.
Coupled point location match (average 0) OK.
Mesh OK.
I did reduce the number of undefined faces, but still there are four which I`ve missed. Is there any possibility to check which faces are undefined ? Cheers, Arthur |
|
|
|
|
|
|
June 4, 2013, 05:50
|
|
#16 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
simpleFoam:
Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : simpleFoam
Date : Jun 04 2013
Time : 10:40:17
Host : "seav-eME730G"
PID : 7212
Case : /home/seav/oFOAM/c1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create mesh for time = 0
Reading field p
Reading field U
Reading/calculating face flux field phi
Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}
Creating finite volume options
No finite volume options present
SIMPLE: no convergence criteria found. Calculations will run for 100 steps.
Starting time loop
Time = 1
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0710741, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0699946, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0723841, No Iterations 2
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#11 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#13
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#14 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : checkMesh
Date : Jun 04 2013
Time : 10:43:13
Host : "seav-eME730G"
PID : 7444
Case : /home/seav/oFOAM/c1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 0
Time = 0
Mesh stats
points: 296329
faces: 770700
internal faces: 663300
cells: 239000
faces per cell: 6
boundary patches: 16
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 239000
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0
Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
*Number of regions: 59
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
in_gora 100 121 ok (non-closed singly connected)
out_gora 100 121 ok (non-closed singly connected)
in_dol 100 121 ok (non-closed singly connected)
out_dol 100 121 ok (non-closed singly connected)
face_plyn 58000 63844 ok (non-closed singly connected)
face_plyn_zewnetrzne11800 14278 ok (non-closed singly connected)
face_przeszkody 36000 39600 ok (non-closed singly connected)
podstawaDol1 100 121 ok (non-closed singly connected)
podstawaDol2 100 121 ok (non-closed singly connected)
metalStripDol 100 121 ok (non-closed singly connected)
metalStripGora 100 121 ok (non-closed singly connected)
metalStripS1 100 121 ok (non-closed singly connected)
metalStripS2 100 121 ok (non-closed singly connected)
podstawaGora1 100 121 ok (non-closed singly connected)
podstawaGora2 100 121 ok (non-closed singly connected)
defaultFaces 400 484 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (0 0 0) (0.45 0.0115 0.14)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (-1.83771e-19 4.61985e-18 1.2634e-18) OK.
Max cell openness = 1.65436e-16 OK.
Max aspect ratio = 900 OK.
Minimum face area = 4e-08. Maximum face area = 0.00063. Face area magnitudes OK.
Min volume = 1e-11. Max volume = 3.36e-08. Total volume = 0.0007245. Cell volumes OK.
Mesh non-orthogonality Max: 0 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.000249975 OK.
Coupled point location match (average 0) OK.
Mesh OK.
End
Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : blockMesh
Date : Jun 04 2013
Time : 10:46:09
Host : "seav-eME730G"
PID : 7636
Case : /home/seav/Pulpit/mgr/mgr
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Creating block mesh from
"/home/seav/Pulpit/mgr/mgr/constant/polyMesh/blockMeshDict"
Creating curved edges
Creating topology blocks
Creating topology patches
Creating block mesh topology
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 901
Found 4 undefined faces in mesh; adding to default patch.
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 919
Reusing existing patch 15 for undefined faces.
Check topology
Basic statistics
Number of internal faces : 180
Number of boundary faces : 1074
Number of defined boundary faces : 1074
Number of undefined boundary faces : 0
Checking patch -> block consistency
Creating block offsets
Creating merge list .
Creating polyMesh from blockMesh
Creating patches
Creating cells
Creating points with scale 0.001
Writing polyMesh
----------------
Mesh Information
----------------
boundingBox: (0 0 0) (0.45 0.0115 0.14)
nPoints: 296329
nCells: 239000
nFaces: 770700
nInternalFaces: 663300
----------------
Patches
----------------
patch 0 (start: 663300 size: 100) name: in_gora
patch 1 (start: 663400 size: 100) name: out_gora
patch 2 (start: 663500 size: 100) name: in_dol
patch 3 (start: 663600 size: 100) name: out_dol
patch 4 (start: 663700 size: 58000) name: face_plyn
patch 5 (start: 721700 size: 11800) name: face_plyn_zewnetrzne
patch 6 (start: 733500 size: 36000) name: face_przeszkody
patch 7 (start: 769500 size: 100) name: podstawaDol1
patch 8 (start: 769600 size: 100) name: podstawaDol2
patch 9 (start: 769700 size: 100) name: metalStripDol
patch 10 (start: 769800 size: 100) name: metalStripGora
patch 11 (start: 769900 size: 100) name: metalStripS1
patch 12 (start: 770000 size: 100) name: metalStripS2
patch 13 (start: 770100 size: 100) name: podstawaGora1
patch 14 (start: 770200 size: 100) name: podstawaGora2
patch 15 (start: 770300 size: 400) name: defaultFaces
End
I did a little trick. In my blockMeshDict file I added: Code:
defaultFaces
{
type wall;
faces ();
}
Arthur. |
|
|
|
|
|
|
June 4, 2013, 06:15
|
|
#17 |
|
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 24 |
Arthur, the blockMesh setup of the mesh is still not ok.
If everything is ok, it should not give any warning or error. Applying tricks like the defaultFaces-entry probably will change something but if you don't understand what it changes you should not apply it. I still stick to my initial advise, simplify the geometry, bring it back to the most basic setup you can think of (only a few blocks) and take that as a starting point for the further development. Good luck, Lieven |
|
|
|
|
|
|
June 4, 2013, 06:24
|
|
#18 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
Thank you Lieven for fast replay.
I have found those undefined faces. blockmesh Code:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.0-5be49240882f
Exec : blockMesh
Date : Jun 04 2013
Time : 11:18:15
Host : "seav-eME730G"
PID : 9839
Case : /home/seav/Pulpit/mgr/mgr
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Creating block mesh from
"/home/seav/Pulpit/mgr/mgr/constant/polyMesh/blockMeshDict"
Creating curved edges
Creating topology blocks
Creating topology patches
Creating block mesh topology
Check topology
Basic statistics
Number of internal faces : 180
Number of boundary faces : 1074
Number of defined boundary faces : 1074
Number of undefined boundary faces : 0
Checking patch -> block consistency
Creating block offsets
Creating merge list .
Creating polyMesh from blockMesh
Creating patches
Creating cells
Creating points with scale 0.001
Writing polyMesh
----------------
Mesh Information
----------------
boundingBox: (0 0 0) (0.45 0.0115 0.14)
nPoints: 296329
nCells: 239000
nFaces: 770700
nInternalFaces: 663300
----------------
Patches
----------------
patch 0 (start: 663300 size: 100) name: in_gora
patch 1 (start: 663400 size: 100) name: out_gora
patch 2 (start: 663500 size: 100) name: in_dol
patch 3 (start: 663600 size: 100) name: out_dol
patch 4 (start: 663700 size: 58000) name: face_plyn
patch 5 (start: 721700 size: 11800) name: face_plyn_zewnetrzne
patch 6 (start: 733500 size: 36000) name: face_przeszkody
patch 7 (start: 769500 size: 300) name: podstawaDol1
patch 8 (start: 769800 size: 100) name: podstawaDol2
patch 9 (start: 769900 size: 100) name: metalStripDol
patch 10 (start: 770000 size: 100) name: metalStripGora
patch 11 (start: 770100 size: 100) name: metalStripS1
patch 12 (start: 770200 size: 100) name: metalStripS2
patch 13 (start: 770300 size: 300) name: podstawaGora1
patch 14 (start: 770600 size: 100) name: podstawaGora2
patch 15 (start: 770700 size: 0) name: defaultFaces
End
Code:
Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
*Number of regions: 59
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"
This case demands such many blocks.. it sounds crazy but its the simplest form of this geometery. Arthur. |
|
|
|
|
|
|
June 4, 2013, 09:18
|
|
#19 |
|
Member
Join Date: May 2013
Posts: 51
Rep Power: 14 |
Lieven, I think I`ve found solution for my problem.
1. I did define all faces in my mesh. 2. I switched solver in my pressure, GAMG to PCG. I did try even on smoothSolver. Seems all works fine. I need to change my initial conditions and boundaries once again to solve this for proper values. I will post here the results when my calculations over. Cheers, A. |
|
|
|
|
|
 |
| Thread Tools | Search this Thread |
| Display Modes | |
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| Transient simulation not converging | skabilan | OpenFOAM Running, Solving & CFD | 14 | December 17, 2019 00:12 |
| Unable to get converged solution using SimpleFoam | jr33 | OpenFOAM Running, Solving & CFD | 6 | December 12, 2016 05:48 |
| pisoFoam with k-epsilon turb blows up - Some questions | Heroic | OpenFOAM Running, Solving & CFD | 26 | December 17, 2012 04:34 |
| plot over time | fferroni | OpenFOAM Post-Processing | 7 | June 8, 2012 08:56 |
| Orifice Plate with a fully developed flow - Problems with convergence | jonmec | OpenFOAM Running, Solving & CFD | 3 | July 28, 2011 06:24 |
Linear Mode
