[jeanpinto24|]

When running the simulation of the geometry and mesh created in Salome and then imported into the cavity case, the terminal throws me the following error:

Courant Number mean: 1.89451 max: 43.117
smoothSolver: Solving for Ux, Initial residual = 0.618674, Final residual = 9.04474e-06, No Iterations 80
smoothSolver: Solving for Uy, Initial residual = 0.600398, Final residual = 9.843e-06, No Iterations 71
DICPCG: Solving for p, Initial residual = 0.963709, Final residual = 7.70104e-07, No Iterations 110
time step continuity errors : sum local = 7.77346e-06, global = 1.8948e-17, cumulative = 1.64322e-17
DICPCG: Solving for p, Initial residual = 0.847767, Final residual = 6.34184e-07, No Iterations 109
time step continuity errors : sum local = 1.09063e-05, global = -1.64853e-17, cumulative = -5.30717e-20
ExecutionTime = 0.26 s ClockTime = 0 s

Time = 0.025

Courant Number mean: 13.4014 max: 328.638
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::symGaussSeidelSmoother::smooth(Foam::word const&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::Field<double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, unsigned char, int) at ??:?
#4 Foam::symGaussSeidelSmoother::smooth(Foam::Field<d ouble>&, Foam::Field<double> const&, unsigned char, int) const at ??:?
#5 Foam::smoothSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#6
at ??:?
#7
at ??:?
#8
at ??:?
#9
at ??:?
#10 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11
at ??:?
Excepción de coma flotante (`core' generado)

[Joshua14]

Hello,

Icofoam is a transient solver. It appears that your time steps are to large causing your Courant number to explode. Try running smaller time steps and that should fix it.

You can also run the simulation as steady using simpleFoam and then you will not have to worry about the Courant number.

Joshua

[jeanpinto24|]

I'm using a different geometry to the cavity case by doing a mesh with Salome and then imported to OpenFoam through the necessary commands. Modified the file "controlDict", but I still get the mentioned error. I attached the file "controlDict" used:

application icoFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 0.5;

deltaT 0.005;

writeControl timeStep;

writeInterval 20;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression off;

timeFormat general;

timePrecision 6;

runTimeModifiable true;

Geometry image:

https://drive.google.com/open?id=0B8...2ZldkZXeHdRTnc

[jeanpinto24|]

Modify the nu file of the constant folder to a value of: 0.001, I kept the "movingWall" speed of 1 m / s. The file "controlDict" is as follows:

Application icoFoam;

StartFrom startTime;

StartTime 0;

StopAt endTime;

EndTime 2;

DeltaT 0.0005;

WriteControl timeStep;

WriteInterval 20;

PurgeWrite 0;

WriteFormat ascii;

WritePrecision 6;

WriteCompression off;

General timeFormat;

TimePrecision 6;

RunTimeModifiable true;

Finally I ran the simulation with the mesh made in Salome.

Thanks very much.

Jean.

[Joshua14]

What is your latest error output? Is your courant number still blowing up?

Joshua

[jeanpinto24|]

The simulation ran without any problem, I attach some images when running icoFoam in the terminal:

https://drive.google.com/open?id=0B8...0piQU5TOXVEX0U

https://drive.google.com/open?id=0B8...zRuVlpLaXNFdU0

Thanks very much.

Jean.

[jeanpinto24|]

When changing the geometry of the cavity (solver icoFoam) case to a box with a cylindrical inlet and outlet like the attached image, I get the following error:

https://drive.google.com/open?id=0B8...1F1U1JkUko1cDQ

-> FOAM FATAL ERROR:
Continuity error can not be removed by adjusting the outflow.
Please check the velocity boundary conditions and / or run potentialFoam to initialise the outflow.
Total flux: 0.284255
Specified mass inflow: 1246.79
Specified mass outflow: 0
Adjustable mass outflow: 0


From function adjustPhi (surfaceScalarField &, const volVectorField &, volScalarField &)
In file cfdTools / general / adjustPhi / adjustPhi.C at line 118.

The entrance is by the lower cylinder.

I attach the files 0 / U and 0 / p:

FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
inlet
{
type fixedValue;
value uniform (0 0 1);
}

exit
{
type fixedValue;
value uniform (0 0 0);
}

walls
{
type fixedValue;
value uniform (0 0 0);
}
}





FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0;

boundaryField
{
inlet
{
type zeroGradient;
}

exit
{
type zeroGradient;
}

walls
{
type zeroGradient;
}
}

[KateEisenhower]

Hi,

you have no outflow. In an incompressible case, it is not working like that:

Continuity error can not be removed by adjusting the outflow.

One possible solution is:

0/U:

inlet: fixedValue
outlet: zeroGradient

0/p:

inlet: zeroGradient
outlet: fixedValue

Best regards,

Kate