CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Error when I try a case with pimple instead of simple solver

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

Like Tree1Likes
  • 1 Post By jherb

Reply
 
LinkBack Thread Tools Display Modes
Old   June 4, 2013, 10:55
Default Error when I try a case with pimple instead of simple solver
  #1
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
Dear All,

I have a problem with a transient simulation. Actually, I do have a case with a steady solution and I have calculated it.
I am now trying to calculate the same solution as the limit of the unsteady counterpart.

But as soos as I run
Code:
buoyanPimpleFoam
instead of
Code:
buoyanSimpleFoam
I get this error message:

Code:
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient$ buoyantPimpleFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.0-0bc225064152
Exec   : buoyantPimpleFoam
Date   : Jun 04 2013
Time   : 16:30:09
Host   : "lab-laptop"
PID    : 4178
Case   : /home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create mesh for time = 0


Reading g
Reading thermophysical properties

Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
--> Upgrading k to employ run-time selectable wall functions
    Backup original k to k.old
    Writing updated k
--> Upgrading epsilon to employ run-time selectable wall functions
    Backup original epsilon to epsilon.old
    Writing updated epsilon
--> Creating mut to employ run-time selectable wall functions
    Writing new mut
--> Creating alphat to employ run-time selectable wall functions
    Writing new alphat
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.3;
    Prt             1;
}

Calculating field g.h

Reading field p_rgh

Creating field dpdt

Creating field kinetic energy K

Courant Number mean: 0 max: 0


--> FOAM FATAL ERROR: 
Residual data for p_rgh must be specified as a dictionary

    From function bool Foam::solutionControl::read()
    in file cfdTools/general/solutionControl/solutionControl/solutionControl.C at line 79.

FOAM exiting

lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient$
Could you please help?

Thanks a lot,
Samuele
samiam1000 is offline   Reply With Quote

Old   June 4, 2013, 11:11
Default
  #2
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
I forgot my fvSolution file. Here it is:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-06;
        relTol          0.01;
    }

    "(U|h|k|epsilon)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }

    G
    {
        $p_rgh;
        tolerance       1e-05;
        relTol          0.1;
    }
}

PIMPLE
{
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;

    residualControl
    {
        p_rgh           1e-2;
        U               1e-3;
        h               1e-3;
        G               1e-3;
    }
}

relaxationFactors
{
    fields
    {
        rho             1.0;
        p_rgh           0.7;
    }
    equations
    {
        U               0.2;
        h               0.2;
        "(k|epsilon|R)" 0.5;
        G               0.7;
    }
}


// ************************************************************************* //
samiam1000 is offline   Reply With Quote

Old   June 5, 2013, 02:36
Default
  #3
Ank
Member
 
ankur
Join Date: May 2012
Location: India
Posts: 50
Rep Power: 5
Ank is on a distinguished road
Hey

I did not understand the problem completely but you can make a small change in your fvSolution by this
PIMPLE
{
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;

residualControl
{
p_rgh 1e-2;
U 1e-3;
h 1e-3;
G 1e-3;
}
}

replace it by this

PIMPLE
{
momentumPredictor no;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
p 0.7;
U 0.3;
T 0.5;
k 0.5;
omega 0.5;
nut 0.5;
R 0.5;
nuTilda 0.5;
}


see if it works.
Ank is offline   Reply With Quote

Old   June 5, 2013, 02:47
Default
  #4
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
I get this error

Code:
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient$ buoyantPimpleFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.0-0bc225064152
Exec   : buoyantPimpleFoam
Date   : Jun 05 2013
Time   : 08:44:24
Host   : "lab-laptop"
PID    : 2367
Case   : /home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create mesh for time = 0


Reading g
Reading thermophysical properties

Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.3;
    Prt             1;
}

Calculating field g.h

Reading field p_rgh

Creating field dpdt

Creating field kinetic energy K

Courant Number mean: 0 max: 0

PIMPLE: Operating solver in PISO mode


Starting time loop

Courant Number mean: 0 max: 0
Time = 0.1

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/libc.so.6"
#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7  Foam::fvMatrix<double>::solve() in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/buoyantPimpleFoam"
#8  
 in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/buoyantPimpleFoam"
#9  __libc_start_main in "/lib/libc.so.6"
#10  
 in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/buoyantPimpleFoam"
Floating point exception
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient$
It is probably due to the BC. But using the steady solver it works fine and I can not und why.
samiam1000 is offline   Reply With Quote

Old   June 5, 2013, 02:52
Default
  #5
Ank
Member
 
ankur
Join Date: May 2012
Location: India
Posts: 50
Rep Power: 5
Ank is on a distinguished road
Can you describe your case a little bit? and the boundary conditions as welll
Ank is offline   Reply With Quote

Old   June 5, 2013, 04:16
Default
  #6
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
Sure. I can share it, if you agree. Please, send an email to samuele.zampini@gmail.com and I'll send the case back to you.
samiam1000 is offline   Reply With Quote

Old   July 29, 2013, 12:56
Default residualControl
  #7
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 291
Rep Power: 9
jherb is on a distinguished road
Hi,

I got the same error message as you and was able to fix it by adding this to my fvSolution file:

Code:
    residualControl
    {
        p_rgh           
        {
            relTol          0;
            tolerance       0.0001;
        }
        U
        {
            relTol          0;
            tolerance       0.0001;
        }
        h
        {
            relTol          0;
            tolerance       0.0001;
        }
        // possibly check turbulence fields
        "(k|epsilon|omega)"        {
            relTol          0;
            tolerance       0.0001;
        }
        
    }
I guess that buoyantPimpleFoam expects the residual control information in this way "as a dictionary", i.e. inside braces with the two entries relTol and tolerance (the latter is probably the absolute value of the residual whereas the first one is the change between two time steps). buoyantSimpleFoam does not need the relTol as there are no time steps.

Joachim


Quote:
Originally Posted by samiam1000 View Post
Code:
buoyantSimpleFoam
I get this error message:

Code:
...

Courant Number mean: 0 max: 0


--> FOAM FATAL ERROR: 
Residual data for p_rgh must be specified as a dictionary

    From function bool Foam::solutionControl::read()
    in file cfdTools/general/solutionControl/solutionControl/solutionControl.C at line 79.

FOAM exiting
nimasam likes this.

Last edited by jherb; July 31, 2013 at 04:00.
jherb is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
snappyMesh Motor Bike case for simpleFoam solver s.sivakumar OpenFOAM Pre-Processing 0 July 23, 2009 00:51
snappyMesh Motor Bike case for simpleFoam solver s.sivakumar OpenFOAM Running, Solving & CFD 0 July 22, 2009 08:00
Simple 2d Matlab Solver Gabriel Usera Main CFD Forum 7 May 14, 2007 00:11
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24
Swirl momentum in SIMPLE based FV solver oz Main CFD Forum 0 February 10, 2006 17:25


All times are GMT -4. The time now is 02:40.