CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

pisoFOAM not converged

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By cryabroad
  • 1 Post By peterhess

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 6, 2019, 00:32
Default pisoFOAM not converged
  #1
New Member
 
Join Date: Feb 2010
Posts: 26
Rep Power: 11
Virtual-iCFD is on a distinguished road
Hi Foamers,

I attempt to solve transient laminar flow with pimplefoam.

During the simulation, the solver says not converged after 5 iterations (see below message).

I am wondering if something i set wrong (tolerance, relTol, etc..)

Below are my fvSolution and fvSchemes files.


HTML Code:
Courant Number mean: 0 max: 0
deltaT = 1e-06
Time = 1e-06

PIMPLE: iteration 1
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.00596631, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.00898104, Final residual = 7.7366e-05, No Iterations 11
time step continuity errors : sum local = 2.89319e-06, global = 2.036e-08, cumulative = 2.036e-08
GAMG:  Solving for p, Initial residual = 0.53187, Final residual = 0.00265644, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.0064018, Final residual = 7.237e-07, No Iterations 40
time step continuity errors : sum local = 2.73227e-08, global = 1.78046e-09, cumulative = 2.21404e-08
PIMPLE: iteration 2
GAMG:  Solving for p, Initial residual = 0.539447, Final residual = 0.00538843, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.00812699, Final residual = 6.43329e-05, No Iterations 13
time step continuity errors : sum local = 2.50622e-06, global = 1.0398e-07, cumulative = 1.2612e-07
GAMG:  Solving for p, Initial residual = 0.318756, Final residual = 0.00307184, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.0055863, Final residual = 6.78875e-07, No Iterations 47
time step continuity errors : sum local = 2.63915e-08, global = -2.57425e-10, cumulative = 1.25863e-07
PIMPLE: iteration 3
GAMG:  Solving for p, Initial residual = 0.314438, Final residual = 0.00192229, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.00504608, Final residual = 4.54241e-05, No Iterations 14
time step continuity errors : sum local = 1.73605e-06, global = 1.91983e-08, cumulative = 1.45061e-07
GAMG:  Solving for p, Initial residual = 0.197118, Final residual = 0.00105657, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.00334511, Final residual = 8.51928e-07, No Iterations 53
time step continuity errors : sum local = 3.24481e-08, global = 2.8933e-09, cumulative = 1.47954e-07
PIMPLE: iteration 4
GAMG:  Solving for p, Initial residual = 0.192587, Final residual = 0.00101836, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.00324218, Final residual = 2.77573e-05, No Iterations 13
time step continuity errors : sum local = 1.04059e-06, global = 3.65136e-08, cumulative = 1.84468e-07
GAMG:  Solving for p, Initial residual = 0.12529, Final residual = 0.000974064, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.00237622, Final residual = 8.42289e-07, No Iterations 30
time step continuity errors : sum local = 3.14838e-08, global = 1.31643e-09, cumulative = 1.85784e-07
PIMPLE: iteration 5
GAMG:  Solving for p, Initial residual = 0.124905, Final residual = 0.000884491, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.0020957, Final residual = 2.03358e-05, No Iterations 16
time step continuity errors : sum local = 8.2739e-07, global = 5.32205e-08, cumulative = 2.39005e-07
GAMG:  Solving for p, Initial residual = 0.00243198, Final residual = 1.79189e-05, No Iterations 13
GAMG:  Solving for p, Initial residual = 0.000253813, Final residual = 8.22938e-07, No Iterations 20
time step continuity errors : sum local = 3.32897e-08, global = 1.18679e-09, cumulative = 2.40192e-07
PIMPLE: not converged within 5 iterations

HTML Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0.01;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    pFinal
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    "(U|k|epsilon)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-05;
        relTol          0.1;
    }

    "(U|k|epsilon)Final"
    {
        $U;
        tolerance       1e-05;
        relTol          0;
    }
}

PIMPLE
{
    momentumPredictor no;
    nOuterCorrectors 5;
    nCorrectors     2;
    nNonOrthogonalCorrectors 1;
    pRefCell        0;
    pRefValue       0;
    residualControl
    {
        "(U)"
        {
                tolerance  1e-3;
                relTol      0;
        }
        p
        {
                tolerance  1e-3;
                relTol      0;
        }
     }
}

relaxationFactors
{
    fields
    {
    	p                         0.3;
    }

     equations
    {
        "(U|k|epsilon)"           0.9;
        "(U|K|epsilon)Final"      1;
    }
}


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

HTML Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss limitedLinearV 1;
    div(phi,k)      Gauss limitedLinear 1;
    div(phi,epsilon) Gauss limitedLinear 1;
    div(phi,R)      Gauss limitedLinear 1;
    div(R)          Gauss linear;
    div(phi,nuTilda) Gauss limitedLinear 1;
    div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}


// ************************************************************************* //
Virtual-iCFD is offline   Reply With Quote

Old   August 6, 2019, 06:23
Default
  #2
Senior Member
 
Robert
Join Date: May 2015
Location: Bremen, GER
Posts: 295
Rep Power: 7
RobertHB is on a distinguished road
Are you running Pimple or PisoFoam? You are providing different information. If you want pisoFoam, your fvSolution uses a PIMPLE subdictionary, which is not read by PisoFoam. You'll want a PISO sub-dict.


Next up, for some reason your solver is not solving for solving for fluid part. You do not have a timestep. How do you expect to solve a transient problem without a time step? What ever you did, try here.
__________________
If you liked my answer to your question, please consider leaving a "Like" in return
RobertHB is offline   Reply With Quote

Old   August 6, 2019, 15:58
Default
  #3
New Member
 
Join Date: Feb 2010
Posts: 26
Rep Power: 11
Virtual-iCFD is on a distinguished road
Sorry, my title is wrong. It should be pimpleFOAM.
Here is my controlDict with timestep

HTML Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     pimpleFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime		0.00005;

deltaT		0.000005;

writeControl    adjustableRunTime;

writeInterval   0.00001;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable yes;

adjustTimeStep  yes;

maxCo           10;

// ************************************************************************* //
Virtual-iCFD is offline   Reply With Quote

Old   August 6, 2019, 16:21
Default
  #4
New Member
 
Join Date: Feb 2010
Posts: 26
Rep Power: 11
Virtual-iCFD is on a distinguished road
Here is my boundary condition. My intent is to apply inlet and outlet pressure BC.

HTML Code:
/*----------------------------------------------------------------------------------------------------*\
|                                                                                                      | 
| 
|                                                                                                      | 
\*----------------------------------------------------------------------------------------------------*/



FoamFile
{
	version 2.0;
	format binary;
	class volScalarField;
	location "";
	object p;
}
/*---------------------------------------------------------------------------*/
/*---------------------------------------------------------------------------*/


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

internalField uniform 0.;


boundaryField
{
	outlet
	{
		type            fixedValue;
        	value           uniform 0;
	}

	inlet
	{
		type            fixedValue;
        	value           uniform 865.470938;
	}

	post1
	{
		type zeroGradient;
	}

	post2
	{
		type zeroGradient;
	}

	post3
	{
		type zeroGradient;
	}

	post4
	{
		type zeroGradient;
	}

	post5
	{
		type zeroGradient;
	}

	post6
	{
		type zeroGradient;
	}

	wall1
	{
		type zeroGradient;
	}

	wall2
	{
		type zeroGradient;
	}


}

HTML Code:
FoamFile
{
	version 2.0;
	format binary;
	class volVectorField;
	location "";
	object U;
}
/*---------------------------------------------------------------------------*/
/*---------------------------------------------------------------------------*/


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

internalField uniform ( 0. 0. 0. );


boundaryField
{
	outlet
	{
		type zeroGradient;
	}

	inlet
	{
		type zeroGradient;
	}

	post1
	{
		type 		fixedValue;
		value		uniform (0 0 0);
	}

	post2
	{
		type            fixedValue;
                value           uniform (0 0 0);
	}

	post3
	{
		type            fixedValue;
                value           uniform (0 0 0);
	}

	post4
	{
		type            fixedValue;
                value           uniform (0 0 0);
	}

	post5
	{
		type            fixedValue;
                value           uniform (0 0 0);
	}

	post6
	{
		type            fixedValue;
                value           uniform (0 0 0);
	}

	wall1
	{
		type            fixedValue;
                value           uniform (0 0 0);
	}

	wall2
	{
		type            fixedValue;
                value           uniform (0 0 0);
	}


}
Virtual-iCFD is offline   Reply With Quote

Old   August 6, 2019, 18:57
Default
  #5
Senior Member
 
shereez234's Avatar
 
MS
Join Date: Jan 2014
Location: England
Posts: 299
Blog Entries: 1
Rep Power: 9
shereez234 is on a distinguished road
What happens if you try to increase the relTol of pressure from 0.01 to 0.1? and relTol of U to 0.01 or 0.001? also put minIter in U to something like 5 or 10. Just shooting some guesses
__________________
__________________________________________
Learn ICEM CFD and external aerodynamics through my youtube channel

https://www.youtube.com/watch?v=ELaJ...s4gf4sjzLYtBS-
shereez234 is offline   Reply With Quote

Old   August 11, 2019, 10:25
Default
  #6
Senior Member
 
Ruiyan Chen
Join Date: Jul 2016
Location: Hangzhou, China
Posts: 128
Rep Power: 5
cryabroad is on a distinguished road
It is telling you that in 5 iterations (the nOuterCorrectors entry you have in the fvSolutions file) the solution is not converged, simplest thing would be just increase this number, something between 5 ~ 50 is what I use frequently.

Note that sometimes this doesn't necessarily mean your solution is diverging. You set the relTol for both p and U to 1e-03, which means that their residuals have to drop three orders of magnitude. Sometimes this is not easy to achieve and if you don't reach 1e-03, it doesn't suggest that the solution is wrong. What you should do to make sure you have convergence is to 1. Check the residuals, normally for pressure it is every easy to have it drop two orders of magnitude; 2. Set up some probes in the flow field and check their pressure (velocity and so on), make sure they are not diverging.
Virtual-iCFD likes this.
cryabroad is offline   Reply With Quote

Old   August 11, 2019, 10:44
Default
  #7
Senior Member
 
Peter Hess
Join Date: Apr 2011
Location: Austria
Posts: 207
Rep Power: 11
peterhess is on a distinguished road
Changing the velocity at the outlet from:

zeroGradient

to

inletOutlet

also if you dont have back flow stabilizes the simulation much!
Virtual-iCFD likes this.
peterhess is offline   Reply With Quote

Reply

Tags
pimple transient, pimple. openfoam, pimplefoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
PisoFoam error: mpirun Exit Code Jinjolee OpenFOAM 3 April 29, 2019 08:10
Initializing transient analysis using static analysis in two-way FSI simulation Daniel_Khazaei ANSYS 50 September 12, 2017 11:56
Differences in solution method for pisoFoam and buoyantBoussinesqPisoFoam mchurchf OpenFOAM 6 September 11, 2013 00:24
New sixDoFRigidBody BC working with laplaceFaceDecomposition Ya_Squall2010 OpenFOAM Running, Solving & CFD 13 April 17, 2013 03:04
pisoFoam compiling error with OF 1.7.1 on MAC OSX Greg Givogue OpenFOAM Programming & Development 3 March 4, 2011 18:18


All times are GMT -4. The time now is 03:34.