[xneop]

Hi,

i am new in OpenFOAM and i set up fvSolution file for PIMPLE, but i am getting an error message :


Build : 4.0-244e6aa02817
Exec : interFoam
Date : Dec 04 2018
Time : 08:33:34
Host : foam
PID : 3632
CtrlDict : "/home/foam/Desktop/Simulations/Model3/Model3Sim/system/controlDict"
Case : /home/foam/Desktop/Simulations/Model3/Model3Sim
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0.0001


PIMPLE: max iterations = 50
field pd : relTol 0, tolerance 0.0001
field U : relTol 0, tolerance 0.0001


Reading g
Reading field pd

Reading field alpha1

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Calculating field g.h



--> FOAM FATAL IO ERROR:
keyword PISO is undefined in dictionary "/home/foam/Desktop/Simulations/Model3/Model3Sim/system/fvSolution"

file: /home/foam/Desktop/Simulations/Model3/Model3Sim/system/fvSolution at line 21.

From function dictionary::subDict(const word& keyword) const
in file db/dictionary/dictionary.C at line 456.

FOAM exiting


this is fvSolution file:
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}

solvers
{
"alpha1.*"
{
nAlphaCorr 1;
nAlphaSubCycles 4;
cAlpha 2;

MULESCorr yes;
nLimiterIter 2;

solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-07;
relTol 0;

}

pcorr
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0;
}

pd
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0.1;
}

pdFinal
{
solver PCG;
preconditioner DIC;
tolerance 1e-07;
relTol 0;
}

U
{
solver BiCGStab;
preconditioner DILU;
tolerance 1e-06;
relTol 0;
}
}

/*PISO
{
cAlpha 2; // alpha correctures
}*/

PIMPLE
{
nOuterCorrectors 50;
nCorrectors 2;
nNonOrthogonalCorrectors 2; // skewness
//nAlphaCorr 1;
//nAlphaSubCycles 4;
pRefCell 0;
pRefValue 0;

residualControl
{
pd
{
tolerance 1e-4;
relTol 0;
}

U
{

tolerance 1e-4;
relTol 0;

}

}
}

relaxationFactors
{
fields
{
pd 0,4;
pdFinal 0,4;
}

equations
{
U 0,6;

".*" 1;
}
}



i don't understand why he is still asking for PISO
could anyone has an idea pls?

[allenjohngeorge]

Did you notice the symbols /* and */ on the fvSolution code:



/*PISO
{
cAlpha 2; // alpha correctures
}*/


this means that this part of the code wont be executed while running. Remove those symbols and try again.

[xneop]

Hi Allen,


yes i noticed, i commented it out, because i want to run PIMPLE. Actually with nOuterCorrectors > 1, i am not suppose to have this error

[Daniel_Khazaei]

Originally Posted by xneop

Hi Allen,


yes i noticed, i commented it out, because i want to run PIMPLE. Actually with nOuterCorrectors > 1, i am not suppose to have this error

if you are running the extend version, that's because interfaceProperties library reads cAlpha value from PISO sub-dict! you need to un-comment it! It doesn't mean that the solver is going to run using PISO algorithm...

[xneop]

Hi Daniel,
ok i will retry again


thx

[xneop]

Hi Daniel,
i have tried, but for large time step it crashes, i had to choose 1e-6 . i am simulating multiphase flow interFOAM VOF. i have read that with PIMPLE Large time step is not a big deal

[allenjohngeorge]

Originally Posted by xneop

Hi Daniel,
i have tried, but for large time step it crashes, i had to choose 1e-6 . i am simulating multiphase flow interFOAM VOF. i have read that with PIMPLE Large time step is not a big deal

What is your courant number in the iterations before crashing ?


Although it says that PIMPLE can handle courant numbers above 1, from my experience, when the courant number goes above 1, the solution crashes after few time steps. I would suggest to keep the courant number close to 0.5 for stable solutions.

[Daniel_Khazaei]

Originally Posted by xneop

Hi Daniel,
i have tried, but for large time step it crashes, i had to choose 1e-6 . i am simulating multiphase flow interFOAM VOF. i have read that with PIMPLE Large time step is not a big deal

well with interFoam and multiphase simulations, I don't suggest using large time step although you are using PIMPLE! For better stability don't go beyond Co 1 and for better accuracy for complex multiphase problems limit the Co to 0.2 using auto-time stepping!

you may want to turn MULESCorr on, it will allow for larger time steps with semi-implicit volume fraction formulation!

[xneop]

Originally Posted by allenjohngeorge

What is your courant number in the iterations before crashing ?


Although it says that PIMPLE can handle courant numbers above 1, from my experience, when the courant number goes above 1, the solution crashes after few time steps. I would suggest to keep the courant number close to 0.5 for stable solutions.

my courant is 5, but i will change it to 1 and see what happens. thx

[xneop]

Originally Posted by Daniel_Khazaei

well with interFoam and multiphase simulations, I don't suggest using large time step although you are using PIMPLE! For better stability don't go beyond Co 1 and for better accuracy for complex multiphase problems limit the Co to 0.2 using auto-time stepping!

you may want to turn MULESCorr on, it will allow for larger time steps with semi-implicit volume fraction formulation!

Hi
i have tried using the suggested adjustement, but it only works without crashing with time step starting from 1e-6 and i have to simulate up to 60s with a velocity of 4e-6 m/s