CFD Online Discussion Forums - FOAM FATAL ERROR Maximum number of iterations exceeded

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - FOAM FATAL ERROR Maximum number of iterations exceeded (https://www.cfd-online.com/Forums/openfoam-solving/59816-foam-fatal-error-maximum-number-iterations-exceeded.html)

Hi Francis,

Thank you for your advice. It also lets me solve my problem.

BR.

Hi,

I am using a Cht K epsion model using Openfoam and I keep getting this error.

I have tried changing the maxiter to 10000 and still get the problem too. Did anyone get to the bottom of this? I completely remade my mesh and still get this same error although I have a few overly skewed faces (64 failed skewness faces) and 900 faces failing nonOrthag check, however due to the geometry even if I used SHM these errors would still occur.

I tried Francis's method and this has't solved it.

I have noticed a sharp (impossible) rise in density in certain regions of the fluid, this was so sharp that it shouted alarm. However I am unfamiliar with this type of modelling so thought I would ask for some advice.

I previously attended the Advanced Openfoam training course and have emailed the guy who ran it (as has my work mate) regarding problems which he encouraged. Unfortunately he does not respond to emails, which has left me a bit discouraged.

Cheers

Hey everyone,

I recently ran into the same issue using the sprayFoam solver with version OF2.4 and an implemented ignition. The error especially ocurrs when I ignite more than one cell and I think it must be due to the Newton solver used to calculate the temperature. Eventually it ocurrs with only one ingiting cell as well though. Has anyone solved this issue so far?

@sahul could you provide the implented brent solver?

Thanks in advance

Moritz

Hi Moritz,

Have you had any luck on this one?

I have noticed that my temperatures are diverging too for no reason. I riginally solved the issue by switching to the plane wall 2d solver, however I have got the error again now.

Maximum number of iterations exceeded

I've been having a lot of trouble tracing the source of this error. I know it happens in the thermoI.H file, but I can't trace what is calling that, or figure out any reason why this is happening. I've had no luck trying to fix this on my own for a while now.

The case i am running is a simple wedge (meshed with snappy hex mesh) inside a blockmesh region using rhoCentral foam.

any help would be really appreciated

this is the error log file

Code:

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  3.0.1                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : 3.0.1-119cac7e8750

Exec   : rhoCentralFoam -parallel

Date   : Jul 01 2016

Time   : 12:54:38

Host   : "cfd01"

PID    : 30359

Case   : /----/wedge15maxIterError

nProcs : 36

Slaves : 

35

(

"cfd01.30360"

"cfd01.30361"

"cfd01.30362"

"cfd01.30363"

"cfd01.30364"

"cfd01.30365"

"cfd01.30366"

"cfd01.30367"

"cfd01.30368"

"cfd01.30369"

"cfd01.30370"

"cfd02.26571"

"cfd02.26572"

"cfd02.26573"

"cfd02.26574"

"cfd02.26575"

"cfd02.26576"

"cfd02.26577"

"cfd02.26578"

"cfd02.26579"

"cfd02.26580"

"cfd02.26581"

"cfd02.26582"

"cfd03.29133"

"cfd03.29134"

"cfd03.29135"

"cfd03.29136"

"cfd03.29137"

"cfd03.29138"

"cfd03.29139"

"cfd03.29140"

"cfd03.29141"

"cfd03.29142"

"cfd03.29143"

"cfd03.29144"

)

Pstream initialized with:

    floatTransfer      : 0

    nProcsSimpleSum    : 0

    commsType          : nonBlocking

    polling iterations : 0

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster

allowSystemOperations : Allowing user-supplied system call operations



// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time



Create mesh for time = 0



Reading thermophysical properties



Selecting thermodynamics package 

{

    type            hePsiThermo;

    mixture         pureMixture;

    transport       const;

    thermo          hConst;

    equationOfState perfectGas;

    specie          specie;

    energy          sensibleInternalEnergy;

}



Reading field U



Creating turbulence model



Selecting turbulence model type laminar

fluxScheme: Kurganov



Starting time loop



Mean and max Courant Numbers = 0.00521015 0.119072

deltaT = 2.4e-06

Time = 2.4e-06



diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

diagonal:  Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0

diagonal:  Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0

diagonal:  Solving for rhoUz, Initial residual = 0, Final residual = 0, No Iterations 0

smoothSolver:  Solving for Ux, Initial residual = 0.999285, Final residual = 0.00389594, No Iterations 5

smoothSolver:  Solving for Uy, Initial residual = 0.999999, Final residual = 8.69665e-17, No Iterations 5

smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 8.81879e-17, No Iterations 5

diagonal:  Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0

smoothSolver:  Solving for e, Initial residual = 1.46977e-11, Final residual = 1.46977e-11, No Iterations 0

ExecutionTime = 0.68 s  ClockTime = 1 s



Mean and max Courant Numbers = 0.00625242 0.142579

deltaT = 2.88e-06

Time = 5.28e-06



diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

diagonal:  Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0

diagonal:  Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0

diagonal:  Solving for rhoUz, Initial residual = 0, Final residual = 0, No Iterations 0

smoothSolver:  Solving for Ux, Initial residual = 6.23273e-10, Final residual = 6.23273e-10, No Iterations 0

smoothSolver:  Solving for Uy, Initial residual = 1.24042e-05, Final residual = 6.5351e-18, No Iterations 5

smoothSolver:  Solving for Uz, Initial residual = 0.00028774, Final residual = 4.85118e-17, No Iterations 5

diagonal:  Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0

smoothSolver:  Solving for e, Initial residual = 5.7298e-12, Final residual = 5.7298e-12, No Iterations 0

[0] [1] 

[1] 

[1] --> FOAM FATAL ERROR: 

[1] Maximum number of iterations exceeded

[1] 

[1]     From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar)const) const [with Thermo = Foam::hConstThermo<Foam::perfectGas<Foam::specie> >; Type = Foam::sensibleInternalEnergy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy>]

[1]     in file /home/openfoam/OpenFOAM/OpenFOAM-3.0.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.

[1] 

FOAM parallel run aborting

[1] 

[2] 

[2] 

[2] --> FOAM FATAL ERROR: [3] 

[3] 

[3] --> FOAM FATAL ERROR: 

[3] Maximum number of iterations exceeded

[3] 

[3]     From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar)const) const [with Thermo = Foam::hConstThermo<Foam::perfectGas<Foam::specie> >; Type = Foam::sensibleInternalEnergy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy>]

[3]     in file /home/openfoam/OpenFOAM/OpenFOAM-3.0.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66[7] 

[7] 

[7] --> FOAM FATAL ERROR: 

[7] Maximum number of iterations exceeded

[7] 

.

for reference, my P/T/U files are here:

p:

Code:

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 18822.7;

boundaryField

{

    inlet

    {

        type            fixedValue;

        value           uniform 18822.7;

    }

    outlet

    {

        type            zeroGradient;

    }

    airplane

    {

        type                zeroGradient;

    }

    bottom

    {

        type            zeroGradient;

    }

    top

    {

        type            zeroGradient;

    }

    symmetry

    {

        type                symmetryPlane;

    }

    left

    {

        type                 zeroGradient;

    }

    defaultFaces

    {

        type            zeroGradient;

    }

}

Code:

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 216.65;

boundaryField

{

    inlet

    {

        type            fixedValue;

        value           uniform 216.65;

    }

    outlet

    {

        type            zeroGradient;

    }

    airplane

    {

        type                zeroGradient;

    }

    bottom

    {

        type            zeroGradient;

    }

    top

    {

        type            zeroGradient;

    }

    left

    {

        type                zeroGradient;

    }

    symmetry

    {

        type                symmetryPlane;

    }

    defaultFaces

    {

        type            zeroGradient;

    }

}

Code:

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (400 0 0); //(246.933 0 0);

boundaryField

{

    inlet

    {

        type                fixedValue;

        value           uniform (400 0 0); //(246.933 0 0);

    }

    outlet

    {

        type            zeroGradient;

    }

    airplane

    {

        type                slip;

    }

    bottom

    {

        type            zeroGradient; 

    }

    top

    {

        type            zeroGradient; 

    }

    left

    {

        type                zeroGradient;

    }

    symmetry

    {

        type                symmetryPlane;

    }

    defaultFaces

    {

        type            zeroGradient;

    }

}

Hi Henry,

Most probably your T value is going to negative or extremely high. To see in into T.Eqn file add Info << T.min() << " " << T.min() <<endl;

then you can understand reason.

hope it helps you.

Baris

It looks like that was the problem, but I'm lost as to how to go about solving it. What can I do to prevent T from going out of control like that?

Hey together,

could anyone please explain me how I can compile the thermo files if I want for example some output debugging in the thermoI.H file??? I somehow don't understand where these files are included in any Make/files...

Any help would be sincerely appreciated

Thanks and cheers

moritz

go to the directory that includes the thermoI.H file, and once you edit whatever debugging code you want into that file, type "wclean" and then "wcompile", which should recompile all the files in that directory for you

Hi henry,

I didnt want to do it as root but I guess it is easier. But still it's not giving me the info in my logfile I acutally wrote in the code. Why?

Code:

template<class Thermo, template<class> class Type>

inline Foam::scalar Foam::species::thermo<Thermo, Type>::T

(

    scalar f,

    scalar p,

    scalar T0,

    scalar (thermo<Thermo, Type>::*F)(const scalar, const scalar) const,

    scalar (thermo<Thermo, Type>::*dFdT)(const scalar, const scalar)

        const,

    scalar (thermo<Thermo, Type>::*limit)(const scalar) const

) const

{

    scalar Test = T0;

    scalar Tnew = T0;

    scalar Ttol = T0*tol_;

    int    iter = 0;

    

    Info<< "Test = " << Test << endl;

    Info<< "   f = " << f << endl;

    do

    {

        Test = Tnew;

        Tnew =

            (this->*limit)

            (Test - ((this->*F)(p, Test) - f)/(this->*dFdT)(p, Test));

            

            scalar Thilf = mag(Tnew - Test);

            Info<< "DeltaT = " << Thilf << endl;

        if (iter++ > maxIter_)

        {

            FatalErrorIn

            (

                "thermo<Thermo, Type>::T(scalar f, scalar T0, "

                "scalar (thermo<Thermo, Type>::*F)"

                "(const scalar) const, "

                "scalar (thermo<Thermo, Type>::*dFdT)"

                "(const scalar) const, "

                "scalar (thermo<Thermo, Type>::*limit)"

                "(const scalar) const"

                ") const"

            )   << "Maximum number of iterations exceeded"

                << abort(FatalError);

        }



    } while (mag(Tnew - Test) > Ttol);



    return Tnew;

}

Ok, sorry for the stupid question. You have to compile the whole thermophysical folder if anyone faces the same problem at some point.

Thanks anyway guys!

chtMultiRegionSimpleFoam - Solution suggestion

Hello Everybody,

Increasing the Mesh quality by increasing the number of cells solved my divergence problem and no error massage appeared anymore.

- My mesh is created by blockMesh

- chtMultiRegionSimpleFoam has been used as a test

- I left the maximum iterations by 100 (did not followed the suggestion above)

- in my test I gave: runTimeModifiable false

I hope it can helps

Regards

Peter

Dear foamer,

I solved the problem. In my case, the error occurred because of different values for T_common in the therm.dat file. Make sure that all reactants involved in the chemical reactions have the same value for T_common. But I think in the current version this bug is already fixed.

Cheers

Quote:

Originally Posted by Momo1805 (Post 611246)

Your suggestion is valuable and useful:D. By unify all T_common in chemistry, I solve the problem that the temperature show non-convergence in version 3.0 with reduced chemistry. And I found another post talking about this, which might be helpful to understand the cause.http://www.cfd-online.com/Forums/ope...ombustion.html

1) Reduce delta T to a order 10000 times lower than the current value.

2) Set Max Courant Number to 1

3) Set ´adjustTimeStep´ to yes

try running the solver again, if it crashes yet again, reduce the delta T even lower then try running again.

This worked for me.

The problem was with higher courant number and that leading to a diverged solution.

Quote:

Originally Posted by srahul (Post 554389)

Hi Michu,

You can find the the script in here
OpenFOAM-2.2.0/src/thermophysicalModels/specie/thermo/thermo/thermoI.H

In this file Newton solver (Line no. 41 - 88) is utilised to calculate the T. I implemented brent solver and now that problem is solved.

Dear Rahul,

We are also struggling with this issue of temperature update using N-R method. Can you share your brent method code implemented in thermoI.H file? We also feel that by using Brent method, this problem can be solved.

Hrushilesh

hi
Did you find a solution to your problem? I'm having the same problem with the compressible solver rhoSimpleFoam.
Thanks in advance!

Hi
I'm having the same ṕroblem you mentioned. Did you manage to solve it? what did you do?
Thanks in advance

Andrea

Quote:

Originally Posted by srahul (Post 554389)

Hi Michu,

You can find the the script in here
OpenFOAM-2.2.0/src/thermophysicalModels/specie/thermo/thermo/thermoI.H

In this file Newton solver (Line no. 41 - 88) is utilized to calculate the T. I implemented brent solver and now that problem is solved.

Hi srahul

I have some questions, How can make the thermoI.H file?
Can you send brent solver text in openFoam?

thanks

My mistake was...

Hello Everybody!

chtMultiRegionSimpleFoam has been used here!

I faced the problem also like many of you.

I tried almost everything has been written here without a success...

I increased the number of cells to a very high number (1 000 000) cells for 100 x 100 x 100 mm region(s).

That worked, but the results where very strange.

And I found the mistake I made!

I made the folowing:

- 3D Design FreeCAD then export as stl

- Used blockMesh to make my initial mesh

- In openFoam using snappyMesh to build my final mesh

The dimensions in my stl file were in mm. That means FreeCAD exports the 100...

snappyMesh read this 100 as 100 m instead of the 100 mm exported

My blockMesh mesh is also too big made (factor 1000)...

Reducing the dimensions in factor 1000 bei:

convertToMeters 0.001 in blockMeshDict

AND

in my exported stl file (FreeCAD)

Solved my problem!

Check up the dimensions (in your blockMeshDict as example) is my suggestion here.

Regards

Peter