Incompatible dimensions for operation
 

I am getting an error as below. Can someone help me solving it?


Courant Number mean: 0 max: 0


--> FOAM FATAL ERROR:
incompatible dimensions for operation
[U[0 1 -2 0 0 0 0] ] == [-grad(p)[1 -2 -2 0 0 0 0] ]

From function checkMethod(const fvMatrix<Type>&, const GeometricField<Type, fvPatchField, volMesh>&)
in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/finiteVolume/lnInclude/fvMatrix.C at line 1356.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*) at ??:?
#3
at ??:?
#4
at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6
at ??:?
Aborted (core dumped)


Thank you.

Hi,

You have wrong pressure dimensions. Guess, the solver is incompressible, so equations are divided by density.

after changing dimensions of pressure
 

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
bounding k, min: 0 max: 0.0937 average: 0.0937
bounding epsilon, min: 0 max: 2.39 average: 2.39
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}


Starting time loop

Time = 0.0025

Courant Number mean: 0 max: 0
^[[BsmoothSolver: Solving for Ux, Initial residual = 1, Final residual = 9.33146, No Iterations 1000
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0823896, No Iterations 1000
smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 2.16149, No Iterations 1000
#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const at ??:?
#4 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const at ??:?
#5 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#6 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) at ??:?
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#8 Foam::fvMatrix<double>::solve() at ??:?
#9
at ??:?
#10 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11
at ??:?
Floating point exception (core dumped)

This indicates not quite correct initial/boundary conditions. k and epsilon could not be equal to 0.

And this usually means wrong boundary conditions. FPE during solution of pressure equation is just a consequence of diverged velocity equation.

there was mistake in the velocity. corrected it. but then, this.



Courant Number mean: 0.000837853 max: 0.179413
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 4.77775e-06, No Iterations 1
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 4.82191e-06, No Iterations 1
smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 2.96083e-12, No Iterations 1
#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const at ??:?
#4 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const at ??:?
#5 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#6 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) at ??:?
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#8 Foam::fvMatrix<double>::solve() at ??:?
#9
at ??:?
#10 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11
at ??:?
Floating point exception (core dumped)

Since you keep your case in secret (even solver you are using could only be guessed by output), suggestions will be generic:

- check your boundary conditions for pressure
- try PCG instead of GAMG
- try smoothSolver instead of GAMG (if PCG fails)
- relax more

file k:


dimensions [ 0 2 -2 0 0 0 0 ];

internalField uniform 0.0937;

boundaryField
{
inlet
{
type zeroGradient;
}
outlet
{
type zeroGradient;
}
wall
{
type kqRWallFunction;
value uniform 0.0937;
}
}



fvSolution file:

FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver GAMG;
tolerance 1e-04;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 10;
mergeLevels 1;
}

pFinal
{
$p;
tolerance 1e-04;
relTol 0;
}

"(U|k|epsilon|R|nuTilda)"
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-03;
relTol 0;
}
}

PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}

please let me know if any other file is required to figure out my mistakes.
thanks alot.

Then let's start with checkMesh output.

checkMesh output


Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 2568811
faces: 7618500
internal faces: 7531500
cells: 2525000
faces per cell: 6
boundary patches: 3
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 2525000
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: 1 (OK).

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
inlet 12500 12601 ok (non-closed singly connected)
outlet 12500 12601 ok (non-closed singly connected)
wall 62000 62200 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-0.10325 -0.10325 -4.1325) (0.10325 0.10325 4.1325)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (1.6254e-16 7.6806e-16 -7.61097e-17) OK.
***High aspect ratio cells found, Max aspect ratio: 7.13865e+195, number of cells 79032
<<Writing 79032 cells with high aspect ratio to set highAspectRatioCells
Minimum face area = 6.05538e-11. Maximum face area = 0.000153586. Face area magnitudes OK.
***Zero or negative cell volume detected. Minimum negative volume: -8.8737e-08, Number of negative volume cells: 77272
<<Writing 77272 zero volume cells to set zeroVolumeCells
Mesh non-orthogonality Max: 180 average: 24.3587
*Number of severely non-orthogonal (> 70 degrees) faces: 87760.
***Number of non-orthogonality errors: 225000.
<<Writing 312760 non-orthogonal faces to set nonOrthoFaces
***Error in face pyramids: 463928 faces are incorrectly oriented.
<<Writing 247308 faces with incorrect orientation to set wrongOrientedFaces
***Max skewness = 871.985, 1056 highly skew faces detected which may impair the quality of the results
<<Writing 1056 skew faces to set skewFaces
Coupled point location match (average 0) OK.

Failed 5 mesh checks.

End

Now you know what to do: fix your mesh first. Then you can try to proceed with simulation. Since I do not know where did you get your mesh, I can not suggest a way to fix it.

thanks. i hope i fix it.