time step continuity error, fvScheme
 

Hi,
I am working on a 3D Mesh(4 million cells-300MBsize).

I am using simpleFoam (turbulent modeling-similar to the one given in tutorials//incompressible/simpleFoam/pitzDaily ).

I have changed the Boundary conditions according to the problem statement.(NOTE: for modeling wall -'wedge' constraint is used..for rotational periodic).

I am getting the following error.
------------------------------------------------------------------------


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;
}


Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0897376, No
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0695567, No
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0733983, No
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00982204, No It
erations 951
time step continuity errors : sum local = 9.06009e-05, global = -6.32167e-06, cu
mulative = -6.32167e-06
#0 Foam::error::printStack(Foam::Ostream&) in "/usr/logau/expsm/OpenFOAM/OpenFO AM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/usr/logau/expsm/OpenFOAM/OpenFOAM-1.6/ lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 void Foam::magSqr<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMes h>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::Geome tricField<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh> const&) i n "/usr/logau/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleR ASModels.so"
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::magSqr<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh>(Foam:: tmp<Foam::GeometricField<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::vol Mesh> > const&) in "/usr/logau/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/l ibincompressibleRASModels.so"
#5 Foam::incompressible::RASModels::kEpsilon::correct () in "/usr/logau/expsm/Op enFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 main in "/usr/logau/expsm/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccD POpt/simpleFoam"
#7 __libc_start_main in "/lib64/libc.so.6"
#8 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start. S:116

floating decimal point exception
---------------------------------------------------------------------

Could anyone please tell what may the problem?

Thank You,
Achinta

Solution which I tried
 

Hi once again,
I tried following techniques..None of them worked.
1.Reduce time step.
2.Increase value of epsilon
3.Reduce relaxation factor.
4.Modify fvScheme.
5.Modify fvSolution.
6.reduce inlet velocity.

Please suggest anyother methods.

Thank You,
Achinta

I think you have something wrong with your setup - like the wrong kind of boundary conditions or something like that. The time step continuity is just the first error that's getting posted. First, make sure all the boundaries in the /0 directory files (U, p, epsilon ...) are the same type as what's stated in the /constant/polymesh/boundary file. For example, if in the boundary file you have a inlet patch called minX, and an outlet patch maxX, then /0/p needs to have the right conditions on these patches (typically zeroGradient at the inlet and uniform 0 at the outlet. Your error happened after the time step continuity check and before k and epsilon. I would check the k file boundaries first. The tutorial will help you figure this out.

Some errors in OF tell you exactly where the problem is, and some are a bit more cryptic. Make sure you are running simpleFoam from the main case directory and not /system or /constant - that will give you errors also.

If you want to temporarily simplify the solver, go in /constant/RASProperties and set turbulence off. The solver will skip k and epsilon, and might tell you exactly where the problem is - if the solver runs properly, then your k or epsilon files in /0 are the problem. So, I would start by checking boundary conditions, and if you don't find the problem turn turbulence off. If you need a 3d tutorial for an example, use motorBike (it runs simpleFoam with k-epsilon turbulence).

Good luck,

Alan

Make sure your epsilon is not initialized with 0.

Hi Santhosh,
K and epsilon are initialized to .000605 and .0003532 respectively.

Is there a probability of Boundary conditions mistake? or with the mesh ?

Thank you

Cheers,
Achinta

Hi Alan,
1) Boundary conditions in /0 are of the same type as stated in boundary file.
2)k values seems to be fine,,
---------------------------------------------------------------------------------
dimensions [0 2 -2 0 0 0 0];

internalField uniform 0.000605;

boundaryField
{
INLET_AIR
{
type fixedValue;
value uniform 0.000605;
}
OUTLET
{
type zeroGradient;
}
SYM1
{
type kqRWallFunction;
value uniform 0.000605;
}
SYM2
{
type kqRWallFunction;
value uniform 0.000605;
}
WALL
{
type kqRWallFunction;
value uniform 0.000605;
}
INLET_GAS
{
type fixedValue;
value uniform 0.000605;
}
--------------------------------------------------------------------------------------------------------

3) I turned the turbulence off. It solved 1 time step completely(earlier it showed error while solving 1st time step. But there was error in 2nd time step..
-------------------------------------------
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;
}


Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0146234, No
Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.05305, No I
terations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.052276, No
Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00989021, No It
erations 664
time step continuity errors : sum local = 0.00162561, global = -0.000143816, cum
ulative = -0.000143816
ExecutionTime = 147.82 s ClockTime = 149 s

Time = 2

#0 Foam::error::printStack(Foam::Ostream&) in "/usr/defoe/expsm/OpenFOAM/OpenFO
AM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/
lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 void Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::Field<Foam::Ve
ctor<double> >&, Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField,
Foam::surfaceMesh> const&) in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux
64GccDPOpt/libfiniteVolume.so"
#4 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvPatchField, Foa
m::volMesh> > Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::Geometric
Field<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "
/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so"
#5 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvPatchField, Foa
m::volMesh> > Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::tmp<Foam:
:GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> >
const&) in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfinite
Volume.so"
#6 Foam::fv::gaussDivScheme<Foam::Tensor<double> >::fvcDiv(Foam::GeometricField <Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh> const&) in "/usr/defoe /expsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so"
#7 Foam::tmp<Foam::GeometricField<Foam::innerProduct< Foam::Vector<double>, Foam ::Tensor<double> >::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div<Fo am::Tensor<double> >(Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchFie ld, Foam::volMesh> const&, Foam::word const&) in "/usr/defoe/expsm/OpenFOAM/Open FOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#8 Foam::tmp<Foam::GeometricField<Foam::innerProduct< Foam::Vector<double>, Foam ::Tensor<double> >::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div<Fo am::Tensor<double> >(Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchFie ld, Foam::volMesh> const&) in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/lib/linux6 4GccDPOpt/libincompressibleRASModels.so"
#9 Foam::incompressible::RASModels::kEpsilon::divDevR eff(Foam::GeometricField<F oam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&) const in "/usr/defoe/e xpsm/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#10 main in "/usr/defoe/expsm/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64Gcc DPOpt/simpleFoam"
#11 __libc_start_main in "/lib64/libc.so.6"
#12 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start .S:116

Floating decimal point exception
-----------------------------------------------------------------------------------

Is k epsilon model good enough for 3D model(Gas turbine combustion model)?

Most of the errors mention /OpenFOAM-1.6/lib/linux64GccDPOpt dirctory.... Is there any mistake in set up files?

Or is there is anything wrong with mesh?

Thank You

Cheers,
Achinta

Hey,

There is probably something wrong with the physic of your flow but to visualize that you need more time steps. In order to perform more time step you can decrease your relaxation factor in system/fvSolution or better change your numerical schemes in system/fvSchemes for example switch your laplacianSchemes to Gauss linear limited 0.6 for all variables and your divSchemes for U to Gauss limitedLinearV 1.

Hope that it would be enough to get more time steps.

Best regards

Christian

Hi Christian,
I have used wedge boundary condition (for rotational periodic condition) for my cylinder wall. Could that be a source of the problem?
My mesh is 3D.

Thank You

Achinta

Hi Achinta,

I m sorry but it is out of my knowledge, I am currently working with MRFSimpleFoam (but without periodic condition) and I also have to deal with the floating point exception errors. But with more time steps you would be able to visualize the flow in Paraview (stay in the Euler case) and maybe you will find the problem.

Christian

Achinta,

Can you modify your setup to temporarily remove the rotational periodic boundary condition? I agree with Christian, there's probably something wrong with the physics of the flow. I would try the default fvSchemes first. I had many crashes while experimenting with non-default fvSchemes after the default setup worked well. The basic approach is to simplify everything - coarse mesh, simple boundaries, default solutions, etc. This might let you run more time steps so you can look at the flow in ParaView. Once you get the simple version to work, start adding complexity until you get to the simulation you want (rotating boundaries, etc.).

Alan

Hi,

Some hints,

1. check the quality of the mesh (checkMesh)
2. increase orthogonal correctors (system/fvSolution)
3. use potential foam to initialize
4. Reduce the relaxation factors (system/fvSolution)


Regards,
Santhosh.

Hi,
I am using default fvschemes..and default fvsolution...
The mesh is coarse too..and I have removed rotational periodic condition.. Same error this time too..
I am using prism cells near the wall.. Could that be a problem?..because its working fine for mesh without prism cells.. Isnt it strange? Is there a solution for this problem?

Thank You,

Kind regards,
Achinta

prism are always not good for CFD...what is your meshCheck is saying. As I already suggest increase the nonOrthogonalcorrector rather than default settings.

santhosh

How large is your time step and what is the corresponding Courant number?

Hi Santhosh,
I increased nonorthogonal corrector to 20. But it didnt give results.

I applied checkMesh. It gave 4 errors.
----------------------------------------
Mesh stats
points: 72486
faces: 631844
internal faces: 613931
cells: 298120
boundary patches: 4
point zones: 0
face zones: 1
cell zones: 1

Overall number of cells of each type:
hexahedra: 0
prisms: 53255
wedges: 0
pyramids: 30
tet wedges: 0
tetrahedra: 244825
polyhedra: 10

Checking topology...
Boundary definition OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
INLET 265 214 ok (non-closed singly connected)
WALL 10658 5502 ok (non-closed singly connected)
OUTLET 741 528 ok (non-closed singly connected)
SYM 6249 3973 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (0 -0.05 -0.0500799) (0.5 0.05 5.21766e-10)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
***Boundary openness (-5.64149e-13 1.37356e-13 -0.000140076) possible hole in boundary description.
***Open cells found, max cell openness: 1, number of open cells 46
<<Writing 46 non closed cells to set nonClosedCells
<<Writing 13 cells with high aspect ratio to set highAspectRatioCells
Minumum face area = 2.62005e-08. Maximum face area = 1.5983e-05. Face area magnitudes OK.
Min volume = 1.33333e-300. Max volume = 1.47396e-08. Total volume = 0.00122512. Cell volumes OK.
Mesh non-orthogonality Max: 179.193 average: 10.5934
*Number of severely non-orthogonal faces: 8.
***Number of non-orthogonality errors: 64.
<<Writing 72 non-orthogonal faces to set nonOrthoFaces
***Error in face pyramids: 138 faces are incorrectly oriented.
<<Writing 74 faces with incorrect orientation to set wrongOrientedFaces
Max skewness = 2.46137 OK.

Failed 4 mesh checks.
--------------------------------------------------------------

Could pyramids be the problem? What are the possible solutions?

Thank You

Regards,
Achinta

Hi Anton,
I am working on a steady-state problem. I am using default time-step of 1.( I had decreased it to .1 to see if it could work. But it failed.).

Thank You.

Regards,
Achinta

There is something wrong with your mesh. Read your blockMesh file carefully with the user manual page for axisymmetric meshes next to you. There shouldn't be no open cells and no incorrectly oriented faces.

And since it looks like you are trying to build a pipe: You'll need inlet, outlet, wall (the curved surface) and wedge (both planes that intersect at the symmetry axis).

Hi,
Is it necessary that the angle between the two wedge patches be 5 degrees? Can we use wedge boundary condition if the angle between the wedges is 180 degrees?

Thank You.

Regards,
Achinta

Why use a wedge if the angle is 180 degrees? Wouldn't symmetry be what you want in that case?

Apart from that, no the angle doesn't necessarily have to be 5 degrees, see:
http://www.cfd-online.com/Forums/ope...type-bcbs.html

Hi,
The physics of the problem requires rotational periodic condition which is not possible with 'symmetryPlane'. So I need 'wedge'. Is there any other way to implement the rotational periodic condition?

Regards,
Achinta