CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   rhoSimpleFoam error (http://www.cfd-online.com/Forums/openfoam-solving/102895-rhosimplefoam-error.html)

mihaipruna June 5, 2012 18:39

rhoSimpleFoam error
 
I can't make heads or tails of this:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / 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 : rhoSimpleFoam
Date : Jun 05 2012
Time : 18:14:23
Host : "ubufoam"
PID : 2126
Case : /home/mihai/OpenFOAM/mihai-2.1.0/run/comprestud/sduct-vanes_100_inlet_vel_smoothallVG
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


SIMPLE: convergence criteria
field p tolerance 1e-05
field U tolerance 1e-05
field k tolerance 1e-05
field omega tolerance 1e-05

Reading thermophysical properties

Selecting thermodynamics package hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting RAS turbulence model kEpsilon
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam::compressible::RASModels::mutkWallFunctionFvP atchScalarField::calcMut() const in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#4 Foam::compressible::RASModels::mutkWallFunctionFvP atchScalarField::updateCoeffs() in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#5 Foam::fvPatchField<double>::evaluate(Foam::UPstrea m::commsTypes) in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/rhoSimpleFoam"
#6 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/rhoSimpleFoam"
#7 Foam::compressible::RASModels::kEpsilon::kEpsilon( Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&, Foam::word const&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#8 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::kEpsilo n>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#9 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#10
in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/rhoSimpleFoam"
#11 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#12
in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/rhoSimpleFoam"
Floating point exception


extract from my mut:

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      volScalarField;
    location    "0";
    object      mut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -1 0 0 0 0];

internalField  uniform 0;

boundaryField
{
    topYmax
    {
        type            calculated;
        value          nonuniform 0();
    }
    bottomYmin
    {
        type            calculated;
        value          nonuniform 0();
    }
    inletXmin
    {
        type            calculated;
        value          nonuniform 0();
    }
    outletXmax
    {
        type            calculated;
        value          nonuniform 0();
    }
    rightZmax
    {
        type            calculated;
        value          nonuniform 0();
    }
    leftZmin
    {
        type            symmetryPlane;
    }
    vol1face1
    {
        type            mutkWallFunction;
        Cmu            0.09;
        kappa          0.41;
        E              9.8;
        value          uniform 0;
    }
    SDuctOutlet
    {
        type            calculated;
        value          uniform 0;
    }
    SDuctInlet
    {
        type            calculated;
        value          uniform 0;
    }
    vol1face4
    {
        type            mutkWallFunction;
        Cmu            0.09;
        kappa          0.41;
        E              9.8;
        value          nonuniform 0();
    }
    vol1face5
    {
        type            mutkWallFunction;
        Cmu            0.09;
        kappa          0.41;
        E              9.8;
        value          uniform 0;
    }
    vol1face6
    {
        type            mutkWallFunction;
        Cmu            0.09;
        kappa          0.41;
        E              9.8;
        value          uniform 0;
    }
...

note that this occurs even when I delete the mut file to let openfoam create it

alberto June 6, 2012 02:07

What do you want to do with entries like

value nonuniform 0();

Shouldn't it be "uniform 0;". Note that 0() indicates a list with zero elements and the format would be different (using the List keyword).

fcollonv June 6, 2012 10:06

Hello,

As pointed out by Alberto, you probably have some troubles with your mesh. Try at least to check it with checkMesh. You should not have patches without faces.

A question: have you created mut yourself or was it generated by OpenFOAM?

Regards

mihaipruna June 6, 2012 12:10

Thanks for the replies.
Using the squarebend tutroial for inspiration I got it running and then ....

Time = 95

GAMG: Solving for Ux, Initial residual = 0.0114881, Final residual = 0.000226671, No Iterations 1
GAMG: Solving for Uy, Initial residual = 0.00116554, Final residual = 7.37184e-05, No Iterations 1
GAMG: Solving for Uz, Initial residual = 0.00832338, Final residual = 0.000335954, No Iterations 1
GAMG: Solving for p, Initial residual = 0.00431245, Final residual = 0.000296092, No Iterations 3
time step continuity errors : sum local = 0.520895, global = 0.309596, cumulative = -102.181
rho max/min : 1 0.1
GAMG: Solving for h, Initial residual = 0.00496736, Final residual = 0.000138371, No Iterations 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/x86_64-linux-gnu/libc.so.6"
#3 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::calculate() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::correct() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"



The crash coincides with a drop in rho min from 0.36 to 0.1

mihaipruna June 6, 2012 16:01

1 Attachment(s)
I introduced a cell limiter which has worked well before for a similar issue (see picture of rho at time 90 without cell limiter) and now it crashes at time 7 with rho min dropping precipitously.

Time = 6

GAMG: Solving for Ux, Initial residual = 0.145982, Final residual = 0.0052821, No Iterations 2
GAMG: Solving for Uy, Initial residual = 0.0834204, Final residual = 0.00275481, No Iterations 2
GAMG: Solving for Uz, Initial residual = 0.238371, Final residual = 0.00817188, No Iterations 2
GAMG: Solving for p, Initial residual = 0.0487939, Final residual = 0.00479841, No Iterations 4
time step continuity errors : sum local = 9.63164, global = 4.62693, cumulative = -66.2753
rho max/min : 1 0.951644
GAMG: Solving for h, Initial residual = 0.166241, Final residual = 0.0139909, No Iterations 1
GAMG: Solving for epsilon, Initial residual = 0.0241813, Final residual = 0.000738986, No Iterations 2
GAMG: Solving for k, Initial residual = 0.0415477, Final residual = 0.00268973, No Iterations 2
ExecutionTime = 357.6 s ClockTime = 371 s

Time = 7

GAMG: Solving for Ux, Initial residual = 0.115854, Final residual = 0.00403452, No Iterations 2
GAMG: Solving for Uy, Initial residual = 0.0659571, Final residual = 0.00218564, No Iterations 2
GAMG: Solving for Uz, Initial residual = 0.198465, Final residual = 0.00700925, No Iterations 2
GAMG: Solving for p, Initial residual = 0.0440085, Final residual = 0.00437184, No Iterations 41
time step continuity errors : sum local = 32.504, global = 0.667329, cumulative = -65.608
rho max/min : 1 0.2635
GAMG: Solving for h, Initial residual = 0.294754, Final residual = 0.0228699, No Iterations 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/x86_64-linux-gnu/libc.so.6"
#3 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::calculate() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::correct() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#5
in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/rhoSimplecFoam"
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7
in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/rhoSimplecFoam"
Floating point exception

the screenshot is of the density field an outlet with fixed pressure.

mihaipruna June 7, 2012 17:07

fixed it, I had zerogradient for Temperature at inlet and fixed value at outlet and it didn't like that, kinda "duh!" , switched them around and now it ran past the point where it was crashing.

fcollonv June 8, 2012 03:45

Hello Mihai,

Happy for you that you fix the trouble. About the boundary conditions, when setting them, you always have to remember a basic rule:
For all fields except pressure, a value should be provided at the inlet (the code cannot know what's outside your domain ;) ). And at outlet, you should let the field go out - so usually zero gradient.
For the pressure it's the opposite due to the coupling velocity-pressure (the velocity is linked to the pressure gradient).

Regards,

mihaipruna June 8, 2012 11:01

yes, definitely!
I think that's what I had in mind, from the beginning, but I switched my patches by mistake.
To be honest, I haven't been spending much time looking at OpenFOAM input files lately, because I automated the case generation process for incompressible flows.
So when I got back to editing files, to make it work for compressible flows with SIMPLEC, I didn't realize that the outlet was listed before the inlet :)


All times are GMT -4. The time now is 17:42.