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

rhoSimpleFoam error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 5, 2012, 18:39
Default rhoSimpleFoam error
  #1
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 7
mihaipruna is on a distinguished road
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:rintStack(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
__________________
Mihai Pruna's Bio

Last edited by mihaipruna; June 5, 2012 at 19:21.
mihaipruna is offline   Reply With Quote

Old   June 6, 2012, 02:07
Default
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
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).
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods

Last edited by alberto; June 6, 2012 at 02:12. Reason: Added clarification
alberto is offline   Reply With Quote

Old   June 6, 2012, 10:06
Default
  #3
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
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
__________________
Frederic Collonval
Technische Universität München
Thermodynamics Dpt.
fcollonv is offline   Reply With Quote

Old   June 6, 2012, 12:10
Default
  #4
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 7
mihaipruna is on a distinguished road
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:rintStack(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:ureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam:erfectGas> > > > >::calculate() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam:ureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam:erfectGas> > > > >::correct() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"



The crash coincides with a drop in rho min from 0.36 to 0.1
__________________
Mihai Pruna's Bio

Last edited by mihaipruna; June 6, 2012 at 15:11.
mihaipruna is offline   Reply With Quote

Old   June 6, 2012, 16:01
Default
  #5
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 7
mihaipruna is on a distinguished road
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:rintStack(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:ureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam:erfectGas> > > > >::calculate() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam:ureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam:erfectGas> > > > >::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.
Attached Images
File Type: jpg sducoutletrho.jpg (96.0 KB, 9 views)
__________________
Mihai Pruna's Bio
mihaipruna is offline   Reply With Quote

Old   June 7, 2012, 17:07
Default
  #6
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 7
mihaipruna is on a distinguished road
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.
__________________
Mihai Pruna's Bio
mihaipruna is offline   Reply With Quote

Old   June 8, 2012, 03:45
Default
  #7
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
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,
__________________
Frederic Collonval
Technische Universität München
Thermodynamics Dpt.
fcollonv is offline   Reply With Quote

Old   June 8, 2012, 11:01
Default
  #8
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 7
mihaipruna is on a distinguished road
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
__________________
Mihai Pruna's Bio
mihaipruna 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
GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM 300 October 29, 2014 19:00
c++ libraries and solver compiling vaina74 OpenFOAM Installation 13 February 3, 2012 18:43
OpenFOAM on MinGW crosscompiler hosted on Linux allenzhao OpenFOAM Installation 127 January 30, 2009 20:08
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51
user defined function cfduser CFX 0 April 29, 2006 10:58


All times are GMT -4. The time now is 10:13.