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

Problems with running a custom solver: "Unknown psiCombustionModel"

Register Blogs Community New Posts Updated Threads Search

Like Tree10Likes

Reply
Page 1 of 2 1 2
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 7, 2015, 03:47
Default Problems with running a custom solver: "Unknown psiCombustionModel"
  #1
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Hi there,

I'm quite new to CFD and OpenFOAM and have been given a thesis with uni on the simulation of Firewhirls - thankfully the work is a continuation on a previous thesis so I won't need to start from scratch - however I am having troubles running the code I have been given.

In order to create a realistic model, the previous student had to create a custom solver to allow the reference frame to rotate. I have compiled the solver using wmake, however when I go to run a case I am getting the following error with the combustion model:
Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : rotatingCDFireFoam
Date   : Aug 07 2015
Time   : 17:17:00
Host   : "alexei-OptiPlex-9010"
PID    : 4394
Case   : /home/alexei/OpenFOAM/alexei-2.2.0/run/changing_diff/whirl_0.05r_0.01in_3.0w
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

--> FOAM Warning : 
    From function dlOpen(const fileName&, const bool)
    in file POSIX.C at line 1179
    dlopen error : libcylindricalVelocityInlet.so: cannot open shared object file: No such file or directory
--> FOAM Warning : 
    From function dlLibraryTable::open(const fileName&, const bool)
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 99
    could not load "libcylindricalVelocityInlet.so"
Create mesh for time = 0


Reading g
Creating combustion model

Selecting combustion model infinitelyFastChemistry<rhoThermoCombustion,gasThermoPhysics>


--> FOAM FATAL ERROR: 
Unknown psiCombustionModel type infinitelyFastChemistry<rhoThermoCombustion,gasThermoPhysics>

Valid  combustionModels are : 

8
(
noCombustion<psiThermoCombustion>
diffusion<psiThermoCombustion,constGasThermoPhysics>
PaSR<psiChemistryCombustion>
infinitelyFastChemistry<psiThermoCombustion,gasThermoPhysics>
FSD<psiThermoCombustion,gasThermoPhysics>
infinitelyFastChemistry<psiThermoCombustion,constGasThermoPhysics>
diffusion<psiThermoCombustion,gasThermoPhysics>
FSD<psiThermoCombustion,constGasThermoPhysics>
)


    From function psiCombustionModel::New
    in file psiCombustionModel/psiCombustionModel/psiCombustionModelNew.C at line 62.

FOAM exiting
The file causing the issue is:
Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

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

#include "psiCombustionModel.H"

// * * * * * * * * * * * * * * * * Selectors * * * * * * * * * * * * * * * * //

Foam::autoPtr<Foam::combustionModels::psiCombustionModel>
Foam::combustionModels::psiCombustionModel::New
(
    const fvMesh& mesh
)
{
    const word combModelName
    (
        IOdictionary
        (
            IOobject
            (
                "combustionProperties",
                mesh.time().constant(),
                mesh,
                IOobject::MUST_READ,
                IOobject::NO_WRITE,
                false
            )
        ).lookup("combustionModel")
    );

    Info<< "Selecting combustion model " << combModelName << endl;

    dictionaryConstructorTable::iterator cstrIter =
        dictionaryConstructorTablePtr_->find(combModelName);

    if (cstrIter == dictionaryConstructorTablePtr_->end())
    {
        FatalErrorIn
        (
            "psiCombustionModel::New"
        )   << "Unknown psiCombustionModel type "
            << combModelName << endl << endl
            << "Valid  combustionModels are : " << endl
            << dictionaryConstructorTablePtr_->toc()
            << exit(FatalError);
    }

    const label tempOpen = combModelName.find('<');

    const word className = combModelName(0, tempOpen);

    return autoPtr<psiCombustionModel>(cstrIter()(className, mesh));
}


// ************************************************************************* //
Any help or tips would be greatly appreciated - if you need more information before you can provide an answer please let me know.
I am using OpenFOAM 2.2.0 on ubuntu 12.04

Cheers,
Alex
Last edited by wyldckat; August 10, 2015 at 10:03. Reason: Added [CODE][/CODE] markers
AlexKam is offline   Reply With Quote

Old   August 10, 2015, 10:07
Default
  #2
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick question: What was the OpenFOAM version that was used in the other thesis?
Because there were some substantial changes over the years and knowing the starting point would make it a lot easier to diagnose. For example: http://www.openfoam.org/version2.2.0/thermophysical.php - section "Dictionary-based Thermodynamics Selection"
AlexKam likes this.
wyldckat is offline   Reply With Quote

Old   August 11, 2015, 03:53
Default
  #3
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
He was also using version 2.2.0!

Cheers,
AlexKam is offline   Reply With Quote

Old   August 12, 2015, 17:03
Default
  #4
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer: Then there are only a few possible reasons for this error message. Some of which I can deduce right now:
  1. You have not built with success the necessary library that the other person provided with the source code, which implements this feature.
  2. Or you commented out an entry inside the "libs" list that is in the file "system/controlDict".
The error message you got, namely this one:
Code:
--> FOAM Warning : 
    From function dlOpen(const fileName&, const bool)
    in file POSIX.C at line 1179
    dlopen error : libcylindricalVelocityInlet.so: cannot open shared object file: No such file or directory
is telling you that the library "libcylindricalVelocityInlet.so" was not found, therefore this supports the 1st hypothesis, i.e. that you did not yet build with success the source code that the other person provided.
AlexKam likes this.
wyldckat is offline   Reply With Quote

Old   August 18, 2015, 10:39
Default
  #5
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Thanks for your help Bruno - I have found a folder of his where he has the Make files for the cylindricalVelocityInlet and custom combustion models - however when I try wmake in either I get an error. Would you have an idea of what is going wrong here? (this is when attempting wmake for cylindricalVelocityInlet):

Code:
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude     -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -IlnInclude -I. -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o -L/home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib \
          -lOpenFOAM -ldl   -lm -o OpenFOAM.out
/usr/lib/gcc/x86_64-linux-gnu/4.6/../../../x86_64-linux-gnu/crt1.o: In function `_start':
(.text+0x20): undefined reference to `main'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::cylindricalVelocityInletFvPatchVectorField::updateCoeffs()':
cylindricalVelocityInletFvPatchVectorField.C:(.text+0xa70): undefined reference to `Foam::fvPatch::Cf() const'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::fvPatchField<Foam::Vector<double> >::type() const':
cylindricalVelocityInletFvPatchVectorField.C:(.text._ZNK4Foam12fvPatchFieldINS_6VectorIdEEE4typeEv[Foam::fvPatchField<Foam::Vector<double> >::type() const]+0x3): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::typeName'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::fixedValueFvPatchField<Foam::Vector<double> >::type() const':
cylindricalVelocityInletFvPatchVectorField.C:(.text._ZNK4Foam22fixedValueFvPatchFieldINS_6VectorIdEEE4typeEv[Foam::fixedValueFvPatchField<Foam::Vector<double> >::type() const]+0x3): undefined reference to `Foam::fixedValueFvPatchField<Foam::Vector<double> >::typeName'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::fvPatchField<Foam::Vector<double> >::adddictionaryConstructorToTable<Foam::cylindricalVelocityInletFvPatchVectorField>::~adddictionaryConstructorToTable()':
cylindricalVelocityInletFvPatchVectorField.C:(.text._ZN4Foam12fvPatchFieldINS_6VectorIdEEE31adddictionaryConstructorToTableINS_42cylindricalVelocityInletFvPatchVectorFieldEED2Ev[_ZN4Foam12fvPatchFieldINS_6VectorIdEEE31adddictionaryConstructorToTableINS_42cylindricalVelocityInletFvPatchVectorFieldEED5Ev]+0x1): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::destroydictionaryConstructorTables()'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::fvPatchField<Foam::Vector<double> >::addpatchMapperConstructorToTable<Foam::cylindricalVelocityInletFvPatchVectorField>::~addpatchMapperConstructorToTable()':
cylindricalVelocityInletFvPatchVectorField.C:(.text._ZN4Foam12fvPatchFieldINS_6VectorIdEEE32addpatchMapperConstructorToTableINS_42cylindricalVelocityInletFvPatchVectorFieldEED2Ev[_ZN4Foam12fvPatchFieldINS_6VectorIdEEE32addpatchMapperConstructorToTableINS_42cylindricalVelocityInletFvPatchVectorFieldEED5Ev]+0x1): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::destroypatchMapperConstructorTables()'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::fvPatchField<Foam::Vector<double> >::addpatchConstructorToTable<Foam::cylindricalVelocityInletFvPatchVectorField>::~addpatchConstructorToTable()':
cylindricalVelocityInletFvPatchVectorField.C:(.text._ZN4Foam12fvPatchFieldINS_6VectorIdEEE26addpatchConstructorToTableINS_42cylindricalVelocityInletFvPatchVectorFieldEED2Ev[_ZN4Foam12fvPatchFieldINS_6VectorIdEEE26addpatchConstructorToTableINS_42cylindricalVelocityInletFvPatchVectorFieldEED5Ev]+0x1): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::destroypatchConstructorTables()'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::fvPatchField<Foam::Vector<double> >::snGrad() const':
cylindricalVelocityInletFvPatchVectorField.C:(.text._ZNK4Foam12fvPatchFieldINS_6VectorIdEEE6snGradEv[Foam::fvPatchField<Foam::Vector<double> >::snGrad() const]+0x15): undefined reference to `Foam::fvPatch::deltaCoeffs() const'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::fixedValueFvPatchField<Foam::Vector<double> >::gradientInternalCoeffs() const':
cylindricalVelocityInletFvPatchVectorField.C:(.text._ZNK4Foam22fixedValueFvPatchFieldINS_6VectorIdEEE22gradientInternalCoeffsEv[Foam::fixedValueFvPatchField<Foam::Vector<double> >::gradientInternalCoeffs() const]+0xd): undefined reference to `Foam::fvPatch::deltaCoeffs() const'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `Foam::fixedValueFvPatchField<Foam::Vector<double> >::gradientBoundaryCoeffs() const':
cylindricalVelocityInletFvPatchVectorField.C:(.text._ZNK4Foam22fixedValueFvPatchFieldINS_6VectorIdEEE22gradientBoundaryCoeffsEv[Foam::fixedValueFvPatchField<Foam::Vector<double> >::gradientBoundaryCoeffs() const]+0x19): undefined reference to `Foam::fvPatch::deltaCoeffs() const'
Make/linux64GccDPOpt/cylindricalVelocityInletFvPatchVectorField.o: In function `_GLOBAL__sub_I_cylindricalVelocityInletFvPatchVectorField.C':
cylindricalVelocityInletFvPatchVectorField.C:(.text.startup+0xf7): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::constructpatchConstructorTables()'
cylindricalVelocityInletFvPatchVectorField.C:(.text.startup+0x10f): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::patchConstructorTablePtr_'
cylindricalVelocityInletFvPatchVectorField.C:(.text.startup+0x13a): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::constructpatchMapperConstructorTables()'
cylindricalVelocityInletFvPatchVectorField.C:(.text.startup+0x155): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::patchMapperConstructorTablePtr_'
cylindricalVelocityInletFvPatchVectorField.C:(.text.startup+0x180): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::constructdictionaryConstructorTables()'
cylindricalVelocityInletFvPatchVectorField.C:(.text.startup+0x19b): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::dictionaryConstructorTablePtr_'
collect2: ld returned 1 exit status
make: *** [OpenFOAM.out] Error 1
Last edited by wyldckat; August 18, 2015 at 10:53. Reason: Added [CODE][/CODE] markers
AlexKam is offline   Reply With Quote

Old   August 18, 2015, 10:54
Default
  #6
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer: Run:
Code:
wmake libso
for building this library.

Didn't the original author provide instructions on how to build the provided source code?
AlexKam likes this.
wyldckat is offline   Reply With Quote

Old   August 19, 2015, 09:03
Default
  #7
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Ahhh thank you again - unfortunately I've been given no instructions whatsoever - just 300GB of case files and old results to sift through. Apologies for another question, but I just tried "wmake libso" and now get this:
Code:
 alexei@alexei-OptiPlex-9010:~/OpenFOAM/cameron-2.2.0/applications/customcombustionModels$ wmake libso
SOURCE=diffusion/diffusions.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/basic/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/specie/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/reactionThermo/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/chemistryModel/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/turbulenceModel -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/ -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESdeltas/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/LES/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude  -IlnInclude -I. -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/diffusions.o
In file included from lnInclude/singleStepCombustion.H:119:0,
                 from diffusion/diffusion.H:39,
                 from diffusion/diffusions.C:30:
lnInclude/singleStepCombustion.C: In member function ‘virtual Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::combustionModels::singleStepCombustion<CombThermoType, ThermoType>::Sh() const’:
lnInclude/singleStepCombustion.C:140:42: error: ‘wSpecie’ was not declared in this scope
lnInclude/singleStepCombustion.C:140:73: error: ‘Y’ was not declared in this scope
lnInclude/singleStepCombustion.C: In member function ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::combustionModels::singleStepCombustion<CombThermoType, ThermoType>::Sh() const [with CombThermoType = Foam::combustionModels::psiThermoCombustion, ThermoType = Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> >]’:
lnInclude/singleStepCombustion.C:141:1: warning: control reaches end of non-void function [-Wreturn-type]
lnInclude/singleStepCombustion.C: In member function ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::combustionModels::singleStepCombustion<CombThermoType, ThermoType>::Sh() const [with CombThermoType = Foam::combustionModels::psiThermoCombustion, ThermoType = Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> >]’:
lnInclude/singleStepCombustion.C:141:1: warning: control reaches end of non-void function [-Wreturn-type]
make: *** [Make/linux64GccDPOpt/diffusions.o] Error 1
alexei@alexei-OptiPlex-9010:~/OpenFOAM/cameron-2.2.0/applications/customcombustionModels$ wmake libso
\SOURCE=diffusion/diffusions.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/basic/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/specie/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/reactionThermo/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/chemistryModel/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/turbulenceModel -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/ -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESdeltas/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/LES/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude  -IlnInclude -I. -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/diffusions.o
In file included from diffusion/diffusions.C:30:0:
diffusion/diffusion.H:39:34: fatal error: singleStepCombustion.H: No such file or directory
compilation terminated.
make: *** [Make/linux64GccDPOpt/diffusions.o] Error 1
Last edited by wyldckat; August 19, 2015 at 15:53. Reason: Added [CODE][/CODE] markers
AlexKam is offline   Reply With Quote

Old   August 19, 2015, 16:06
Default
  #8
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Hi Alex,

That is strange... did you do something between the two executions of "wmake libso"?
Because the second time you run the command it should give you the exact same error message!?

Try running:
Code:
wclean
wmake libso
Can you find any files named "Allwmake" in those source code folders from the thesis work? If you can find any, run the main script like this:
Code:
./Allwmake
If this doesn't fix the problem, please share the source code, so that it's easier to diagnose the problem. If the source code cannot be made public, send me the source code via private message, by using an online file sharing service, since private messages don't allow attachments.

Best regards,
Bruno

PS: Please use follow the instructions for Posting code and output with [CODE]
 (i.e. when writing the output in one of your posts )
__________________
wyldckat is offline   Reply With Quote

Old   August 19, 2015, 23:30
Default
  #9
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Hi Bruno,

I didn't do anything between the executions of "wmake libso" - there is no Allwmake in the source code unfortunately, but I’ve tried it again with 'wclean' and get the following:

Code:
 alexei@alexei-OptiPlex-9010:~/OpenFOAM/cameron-2.2.0/applications/customcombustionModels$ wclean
alexei@alexei-OptiPlex-9010:~/OpenFOAM/cameron-2.2.0/applications/customcombustionModels$ wmake libso
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file combustionModel/combustionModel.C
Making dependency list for source file psiCombustionModel/psiCombustionModel/psiCombustionModel.C
Making dependency list for source file psiCombustionModel/psiCombustionModel/psiCombustionModelNew.C
Making dependency list for source file psiCombustionModel/psiThermoCombustion/psiThermoCombustion.C
Making dependency list for source file diffusion/diffusions.C
SOURCE=combustionModel/combustionModel.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/basic/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/specie/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/reactionThermo/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/chemistryModel/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/turbulenceModel -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/ -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESdeltas/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/LES/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude  -IlnInclude -I. -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/combustionModel.o
SOURCE=psiCombustionModel/psiCombustionModel/psiCombustionModel.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/basic/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/specie/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/reactionThermo/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/chemistryModel/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/turbulenceModel -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/ -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESdeltas/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/LES/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude  -IlnInclude -I. -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/psiCombustionModel.o
SOURCE=psiCombustionModel/psiCombustionModel/psiCombustionModelNew.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/basic/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/specie/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/reactionThermo/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/chemistryModel/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/turbulenceModel -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/ -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESdeltas/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/LES/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude  -IlnInclude -I. -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/psiCombustionModelNew.o
SOURCE=psiCombustionModel/psiThermoCombustion/psiThermoCombustion.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/basic/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/specie/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/reactionThermo/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/chemistryModel/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/turbulenceModel -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/ -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESdeltas/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/LES/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude  -IlnInclude -I. -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/psiThermoCombustion.o
SOURCE=diffusion/diffusions.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/basic/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/specie/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/reactionThermo/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/chemistryModel/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/turbulenceModel -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/ -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESdeltas/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/turbulenceModels/compressible/LES/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/finiteVolume/lnInclude  -IlnInclude -I. -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude -I/home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/diffusions.o
In file included from lnInclude/singleStepCombustion.H:119:0,
                 from diffusion/diffusion.H:39,
                 from diffusion/diffusions.C:30:
lnInclude/singleStepCombustion.C: In member function ‘virtual Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::combustionModels::singleStepCombustion<CombThermoType, ThermoType>::Sh() const’:
lnInclude/singleStepCombustion.C:140:42: error: ‘wSpecie’ was not declared in this scope
lnInclude/singleStepCombustion.C:140:73: error: ‘Y’ was not declared in this scope
lnInclude/singleStepCombustion.C: In member function ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::combustionModels::singleStepCombustion<CombThermoType, ThermoType>::Sh() const [with CombThermoType = Foam::combustionModels::psiThermoCombustion, ThermoType = Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> >]’:
lnInclude/singleStepCombustion.C:141:1: warning: control reaches end of non-void function [-Wreturn-type]
lnInclude/singleStepCombustion.C: In member function ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::combustionModels::singleStepCombustion<CombThermoType, ThermoType>::Sh() const [with CombThermoType = Foam::combustionModels::psiThermoCombustion, ThermoType = Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> >]’:
lnInclude/singleStepCombustion.C:141:1: warning: control reaches end of non-void function [-Wreturn-type]
make: *** [Make/linux64GccDPOpt/diffusions.o] Error 1
I've made a dropbox of the directories and code for you to have a look where everything is set out exactly as is on my system - https://www.dropbox.com/sh/omwdatlmw...bkMga6uza?dl=0

customcombustionModels is where the issues are - I've had a look and the singleStepCombustion and infinitelyFastChemistry files don't seem to be mentioned within the Make files? If this is the problem I'm not entirely sure how to fix it

if you need anything else please let me know
Thank you so much for your help/time

https://www.dropbox.com/sh/0tldmchii...OttANOlma?dl=0
Last edited by wyldckat; August 20, 2015 at 13:18. Reason: merged posts that were a few minutes apart
AlexKam is offline   Reply With Quote

Old   August 20, 2015, 13:43
Default
  #10
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Hi Alex,

Well, this was interesting... I had to do some probabilistic reverse engineering to the way of thinking of the author of the thesis you inherited... this to say that I had to guess (based on the information and files you provided) that this version of the source code you have is at a point where the author was apparently experimenting the implementation of a diffusion model... but had to stop for whatever reason and didn't revert the source code to the previous point where it was previously working.

The solution is as follows:
  • Edit the file "customcombustionModels/Make/options" and use this content:
    Code:
    EXE_INC = \
    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/reactionThermo/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/chemistryModel/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/compressible/turbulenceModel \
    -I$(LIB_SRC)/turbulenceModels/ \
    -I$(LIB_SRC)/turbulenceModels/LES/LESdeltas/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/LES/LESfilters/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/compressible/LES/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/combustionModels/lnInclude

LIB_LIBS = \
    -lfiniteVolume \
    -lincompressibleLESModels \
    -lchemistryModel
    The only difference is the addition of the "combustionModels" line, so that it can properly inherit code from OpenFOAM's own library.
  • Edit the file "customcombustionModels/Make/" and use this content:
    Code:
    combustionModel/combustionModel.C

psiCombustionModel/psiCombustionModel/psiCombustionModel.C
psiCombustionModel/psiCombustionModel/psiCombustionModelNew.C
psiCombustionModel/psiThermoCombustion/psiThermoCombustion.C

/* diffusion/diffusions.C */
infinitelyFastChemistry/infinitelyFastChemistrys.C


LIB = $(FOAM_USER_LIBBIN)/libcustomcombustionModels
    The difference is that I commented out the code for the diffusions and added the one for "infinitelyFastChemistry".
Then run:
Code:
wclean
wmake libso
And it should now build properly.


Best regards,
Bruno
AlexKam likes this.
__________________
wyldckat is offline   Reply With Quote

Old   August 22, 2015, 01:23
Default
  #11
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Thank you so much Bruno, it built successfully!
AlexKam is offline   Reply With Quote

Old   August 23, 2015, 02:11
Default
  #12
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Bruno,

Apologies for all the questions - I've had another issue with this custom solver that you may understand

Now that the libraries have been built I've run a case using the stock fireFoam solver with no problem - however trying to use the custom solver gave me the following error:

Code:
alexei@alexei-OptiPlex-9010:~/OpenFOAM/alexei-2.2.0/changing_diff/whirl_0.05r_0.01in_3.0w$ rotatingCDFireFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0
Exec   : rotatingCDFireFoam
Date   : Aug 23 2015
Time   : 15:32:20
Host   : "alexei-OptiPlex-9010"
PID    : 4317
Case   : /home/alexei/OpenFOAM/alexei-2.2.0/changing_diff/whirl_0.05r_0.01in_3.0w
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
Creating combustion model

Selecting combustion model infinitelyFastChemistry<psiThermoCombustion,gasThermoPhysics>
Selecting thermodynamics package 
{
    type            heRhoThermo;
    mixture         singleStepReactingMixture;
    transport       sutherland;
    thermo          janaf;
    energy          sensibleEnthalpy;
    equationOfState perfectGas;
    specie          specie;
}



--> FOAM FATAL ERROR: 
Unknown psiReactionThermo type 
thermoType
{
    type            heRhoThermo;
    mixture         singleStepReactingMixture;
    transport       sutherland;
    thermo          janaf;
    energy          sensibleEnthalpy;
    equationOfState perfectGas;
    specie          specie;
}


Valid psiReactionThermo types are:

type         mixture                    transport   thermo  equationOfState  specie  energy            

hePsiThermo  homogeneousMixture         const       hConst  perfectGas       specie  sensibleEnthalpy  
hePsiThermo  homogeneousMixture         sutherland  hConst  perfectGas       specie  sensibleEnthalpy  
hePsiThermo  homogeneousMixture         sutherland  janaf   perfectGas       specie  sensibleEnthalpy  
hePsiThermo  inhomogeneousMixture       const       hConst  perfectGas       specie  sensibleEnthalpy  
hePsiThermo  inhomogeneousMixture       sutherland  hConst  perfectGas       specie  sensibleEnthalpy  
hePsiThermo  inhomogeneousMixture       sutherland  janaf   perfectGas       specie  sensibleEnthalpy  
hePsiThermo  multiComponentMixture      const       hConst  perfectGas       specie  sensibleEnthalpy  
hePsiThermo  multiComponentMixture      sutherland  janaf   perfectGas       specie  sensibleEnthalpy  
hePsiThermo  reactingMixture            const       hConst  perfectGas       specie  sensibleEnthalpy  
hePsiThermo  reactingMixture            sutherland  janaf   perfectGas       specie  sensibleEnthalpy  
hePsiThermo  singleStepReactingMixture  sutherland  janaf   perfectGas       specie  sensibleEnthalpy  
hePsiThermo  veryInhomogeneousMixture   const       hConst  perfectGas       specie  sensibleEnthalpy  
hePsiThermo  veryInhomogeneousMixture   sutherland  hConst  perfectGas       specie  sensibleEnthalpy  
hePsiThermo  veryInhomogeneousMixture   sutherland  janaf   perfectGas       specie  sensibleEnthalpy  


    From function psiReactionThermo::New
    in file /home/alexei/OpenFOAM/OpenFOAM-2.2.0/src/thermophysicalModels/basic/lnInclude/basicThermoTemplates.C at line 73.

FOAM exiting
So I changed the thermoType from 'heRhoThermo' to 'hePsiThermo' and now get the following:

Code:
 alexei@alexei-OptiPlex-9010:~/OpenFOAM/alexei-2.2.0/changing_diff/whirl_0.05r_0.01in_3.0w$ rotatingCDFireFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0
Exec   : rotatingCDFireFoam
Date   : Aug 23 2015
Time   : 15:34:59
Host   : "alexei-OptiPlex-9010"
PID    : 4323
Case   : /home/alexei/OpenFOAM/alexei-2.2.0/changing_diff/whirl_0.05r_0.01in_3.0w
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
Creating combustion model

Selecting combustion model infinitelyFastChemistry<psiThermoCombustion,gasThermoPhysics>
Selecting thermodynamics package 
{
    type            hePsiThermo;
    mixture         singleStepReactingMixture;
    transport       sutherland;
    thermo          janaf;
    energy          sensibleEnthalpy;
    equationOfState perfectGas;
    specie          specie;
}

Selecting chemistryReader foamChemistryReader
Fuel heat of combustion :5.00312e+07
stoichiometric air-fuel ratio :17.0854
stoichiometric oxygen-fuel ratio :3.98918
Maximum products mass concentrations:
    H2O: 0.124183
    CO2: 0.151685
    N2: 0.724132
Combustion mode: explicit
Reading thermophysical properties

Creating component thermo properties:
    multi-component carrier - 5 species
    no liquid components
    no solid components
Creating field rho

Reading coriolis Omega


Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type LESModel
Selecting LES turbulence model homogeneousDynOneEqEddy
Selecting LES delta type cubeRootVol
homogeneousDynOneEqEddyCoeffs
{
    cubeRootVolCoeffs
    {
        deltaCoeff      1;
    }
    filter          simple;
    ce              1.048;
    Prt             1;
}

Creating field alphaEff

Creating field dpdt

Creating field kinetic energy K

Calculating field g.h

Creating finite volume options
No finite volume options present


Constructing reacting cloud
Constructing particle injection models
Selecting injection model none

Constructing surface film model
Selecting surfaceFilmModel none
    Selecting region model functions
    none
Creating pyrolysis model
Selecting pyrolysisModel none
Selecting radiationModel none
Courant Number mean: 1.99734e-07 max: 0.000333333

PIMPLE: Operating solver in PISO mode


Starting time loop

Courant Number mean: 1.95817e-07 max: 0.000326797
deltaT = 0.00138889
Time = 0.00138889

DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 2.24715e-12, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 2.25169e-12, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 3.58386e-10, No Iterations 2
DILUPBiCG:  Solving for O2, Initial residual = 0.999997, Final residual = 4.23966e-05, No Iterations 1
DILUPBiCG:  Solving for H2O, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for CH4, Initial residual = 1, Final residual = 4.25376e-05, No Iterations 1
DILUPBiCG:  Solving for CO2, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for h, Initial residual = 0.999998, Final residual = 7.89022e-09, No Iterations 2
min/max(T) = 292.995, 293


--> FOAM FATAL IO ERROR: 
keyword p is undefined in dictionary "/home/alexei/OpenFOAM/alexei-2.2.0/changing_diff/whirl_0.05r_0.01in_3.0w/system/fvSolution.solvers"

file: /home/alexei/OpenFOAM/alexei-2.2.0/changing_diff/whirl_0.05r_0.01in_3.0w/system/fvSolution.solvers from line 22 to line 82.

    From function dictionary::subDict(const word& keyword) const
    in file db/dictionary/dictionary.C at line 608.

FOAM exiting
I have updated dropbox with the case as well as the solver I am trying to use if you need to have a look:
https://www.dropbox.com/sh/0tldmchii...OttANOlma?dl=0

Kind Regards,
Alexei
AlexKam is offline   Reply With Quote

Old   August 23, 2015, 12:13
Default
  #13
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer:
The case does not have a mesh, therefore I can't test things myself.
Either way, my guess is that you also need to add the other library to the "libs" list in "system/controlDict":
Code:
libs  (
   "libcylindricalVelocityInlet.so"
   "libcustomcombustionModels.so"
);
AlexKam likes this.
wyldckat is offline   Reply With Quote

Old   August 26, 2015, 20:52
Default
  #14
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Bruno,

Thanks for your advice, I tried doing that and hit run on the code and it has been running for the past 3 days (over 60hrs). This morning I woke up and saw the following error - I've only posted some of it because it was quite long:

Code:
7fa415096000-7fa415099000  rw-p 004a9000 08:01 41960084                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so
7fa415099000-7fa41509a000 rw-p 00000000 00:00 0 
7fa41509a000-7fa4150bc000  r-xp 00000000 08:01 41960078                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libthermophysicalFunctions.so
7fa4150bc000-7fa4152bc000  ---p 00022000 08:01 41960078                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libthermophysicalFunctions.so
7fa4152bc000-7fa4152bd000  r--p 00022000 08:01 41960078                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libthermophysicalFunctions.so
7fa4152bd000-7fa4152be000  rw-p 00023000 08:01 41960078                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libthermophysicalFunctions.so
7fa4152be000-7fa4152c2000  r-xp 00000000 08:01 41960082                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsolidMixtureProperties.so
7fa4152c2000-7fa4154c1000  ---p 00004000 08:01 41960082                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsolidMixtureProperties.so
7fa4154c1000-7fa4154c2000  r--p 00003000 08:01 41960082                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsolidMixtureProperties.so
7fa4154c2000-7fa4154c3000  rw-p 00004000 08:01 41960082                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsolidMixtureProperties.so
7fa4154c3000-7fa4154d3000  r-xp 00000000 08:01 41960081                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsolidProperties.so
7fa4154d3000-7fa4156d3000  ---p 00010000 08:01 41960081                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsolidProperties.so
7fa4156d3000-7fa4156d4000  r--p 00010000 08:01 41960081                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsolidProperties.so
7fa4156d4000-7fa4156d5000  rw-p 00011000 08:01 41960081                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsolidProperties.so
7fa4156d5000-7fa415890000  r-xp 00000000 08:01 41960083                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so
7fa415890000-7fa415a8f000  ---p 001bb000 08:01 41960083                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so
7fa415a8f000-7fa415a9c000  r--p 001ba000 08:01 41960083                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so
7fa415a9c000-7fa415a9e000  rw-p 001c7000 08:01 41960083                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so
7fa415a9e000-7fa415c3d000  r-xp 00000000 08:01 41960076                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libspecie.so
7fa415c3d000-7fa415e3d000  ---p 0019f000 08:01 41960076                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libspecie.so
7fa415e3d000-7fa415e46000  r--p 0019f000 08:01 41960076                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libspecie.so
7fa415e46000-7fa415e47000  rw-p 001a8000 08:01 41960076                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libspecie.so
7fa415e47000-7fa415e48000 rw-p 00000000 00:00 0 
7fa415e48000-7fa415f99000  r-xp 00000000 08:01 41960102                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libcompressibleLESModels.so
7fa415f99000-7fa416198000  ---p 00151000 08:01 41960102                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libcompressibleLESModels.so
7fa416198000-7fa41619f000  r--p 00150000 08:01 41960102                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libcompressibleLESModels.so
7fa41619f000-7fa4161a2000  rw-p 00157000 08:01 41960102                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libcompressibleLESModels.so
7fa4161a2000-7fa4163f2000  r-xp 00000000 08:01 41960101                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so
7fa4163f2000-7fa4165f1000  ---p 00250000 08:01 41960101                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so
7fa4165f1000-7fa4165fa000  r--p 0024f000 08:01 41960101                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so
7fa4165fa000-7fa4165fd000  rw-p 00258000 08:01 41960101                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so
7fa4165fd000-7fa4165fe000 rw-p 00000000 00:00 0 
7fa4165fe000-7fa416916000  r-xp 00000000 08:01 41959587                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsampling.so
7fa416916000-7fa416b16000  ---p 00318000 08:01 41959587                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsampling.so
7fa416b16000-7fa416b21000  r--p 00318000 08:01 41959587                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsampling.so
7fa416b21000-7fa416b26000  rw-p 00323000 08:01 41959587                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libsampling.so
7fa416b26000-7fa416b27000 rw-p 00000000 00:00 0 
7fa416b27000-7fa416e25000  r-xp 00000000 08:01 41957627                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libmeshTools.so
7fa416e25000-7fa417024000  ---p 002fe000 08:01 41957627                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libmeshTools.so
7fa417024000-7fa417032000  r--p 002fd000 08:01 41957627                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libmeshTools.so
7fa417032000-7fa417036000  rw-p 0030b000 08:01 41957627                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libmeshTools.so
7fa417036000-7fa417042000 rw-p 00000000 00:00 0 
7fa417042000-7fa417161000  r-xp 00000000 08:01 41960123                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfvOptions.so
7fa417161000-7fa417360000  ---p 0011f000 08:01 41960123                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfvOptions.so
7fa417360000-7fa417367000  r--p 0011e000 08:01 41960123                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfvOptions.so
7fa417367000-7fa417369000  rw-p 00125000 08:01 41960123                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfvOptions.so
7fa417369000-7fa41736a000 rw-p 00000000 00:00 0 
7fa41736a000-7fa418464000  r-xp 00000000 08:01 41959073                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so
7fa418464000-7fa418664000  ---p 010fa000 08:01 41959073                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so
7fa418664000-7fa4186bf000  r--p 010fa000 08:01 41959073                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so
7fa4186bf000-7fa4186c9000  rw-p 01155000 08:01 41959073                    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so
7fa4186c9000-7fa4186d0000 rw-p 00000000 00:00 0 
7fa4186d0000-7fa4186f2000 r-xp 00000000 08:01 25956145                   /lib/x86_64-linux-gnu/ld-2.15.so
7fa4188b9000-7fa4188d3000 rw-p 00000000 00:00 0 
7fa4188e5000-7fa4188f2000 rw-p 00000000 00:00 0 
7fa4188f2000-7fa4188f3000 r--p 00022000 08:01 25956145                   /lib/x86_64-linux-gnu/ld-2.15.so
7fa4188f3000-7fa4188f5000 rw-p 00023000 08:01 25956145                   /lib/x86_64-linux-gnu/ld-2.15.so
7fffbd7c9000-7fffbd7eb000 rw-p 00000000 00:00 0                          [stack]
7fffbd7fe000-7fffbd800000 r-xp 00000000 00:00 0                          [vdso]
ffffffffff600000-ffffffffff601000 r-xp 00000000 00:00 0                  [vsyscall]
Aborted (core dumped)
alexei@alexei-OptiPlex-9010:~/OpenFOAM/alexei-2.2.0/changing_diff/whirl_0.05r_0.01in_3.0w$ paraFoam
created temporary 'whirl_0.05r_0.01in_3.0w.OpenFOAM'
--> FOAM Warning : 
    From function dlOpen(const fileName&, const bool)
    in file POSIX.C at line 1179
     dlopen error :  /home/alexei/OpenFOAM/alexei-2.2.0/platforms/linux64GccDPOpt/lib/libcustomcombustionModels.so:  undefined symbol:  _ZNK4Foam16combustionModels19rhoThermoCombustion3rhoEv
--> FOAM Warning : 
    From function dlLibraryTable::open(const fileName&, const bool)
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 99
    could not load "libcustomcombustionModels.so"
Kind Regards,

(i also uploaded those mesh files if you were interested)
AlexKam is offline   Reply With Quote

Old   August 26, 2015, 21:51
Default
  #15
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Sorry for all the questions again - but does it make sense to you that I still get an error such as this even though I've successfully compiled the library with your help earlier?

Code:
alexei@alexei-OptiPlex-9010:~/OpenFOAM/alexei-2.2.0/fixedDiff/small/whirl_0.05r_0.01in_1.125w_7e-4Diff$ rotatingCDFireFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0
Exec   : rotatingCDFireFoam
Date   : Aug 27 2015
Time   : 11:48:44
Host   : "alexei-OptiPlex-9010"
PID    : 9995
Case   : /home/alexei/OpenFOAM/alexei-2.2.0/fixedDiff/small/whirl_0.05r_0.01in_1.125w_7e-4Diff
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
Creating combustion model

Selecting combustion model infinitelyFastChemistry<rhoThermoCombustion,gasThermoPhysics>


--> FOAM FATAL ERROR: 
Unknown psiCombustionModel type infinitelyFastChemistry<rhoThermoCombustion,gasThermoPhysics>

Valid  combustionModels are : 

8
(
noCombustion<psiThermoCombustion>
diffusion<psiThermoCombustion,constGasThermoPhysics>
PaSR<psiChemistryCombustion>
infinitelyFastChemistry<psiThermoCombustion,gasThermoPhysics>
FSD<psiThermoCombustion,gasThermoPhysics>
infinitelyFastChemistry<psiThermoCombustion,constGasThermoPhysics>
diffusion<psiThermoCombustion,gasThermoPhysics>
FSD<psiThermoCombustion,constGasThermoPhysics>
)


    From function psiCombustionModel::New
    in file psiCombustionModel/psiCombustionModel/psiCombustionModelNew.C at line 62.

FOAM exiting
I also tried adding in the customCombustion library to the controlDict file and it seems to get slightly further before coming up with the same error
AlexKam is offline   Reply With Quote

Old   August 30, 2015, 17:07
Default
  #16
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Hi Alex,

The error log for the crash is incomplete. The real reason should be disclaimed before the long list of memory addresses you posted. Try running with the following command:
Code:
rotatingCDFireFoam > log.rotatingCDFireFoam 2>&1
The "2>&1" is for redirecting error output to the standard one. The file "log.rotatingCDFireFoam" will have the complete list of error messages.

The issue with paraFoam is because the library that ParaView loads for opening OpenFOAM cases will only load the minimum libraries it needs. If you have your own libraries in "libs", the custom libraries will depend on other libraries that aren't loaded by default. The easiest workaround is to comment the "libs" entry. Or use the following command for listing the libraries that your solver depends on:
Code:
ldd $(which rotatingCDFireFoam)
then adding the combustion libraries to the "libs" list.

Going back to the first crash: without the complete error log, it's hard to deduce why it crashed.
My fear is that the case files they provided you are either incorrect, or you're working with the last development snapshot. In other words: given the issue I diagnosed for a previous post, the source code was left in a point where new developments were being tested but were not completed. It's possible the thesis author provided two types of folders:
  1. the one used for getting the documented results for the thesis;
  2. and another folder for the latest code and case development.
Best regards,
Bruno
AlexKam likes this.
__________________
wyldckat is offline   Reply With Quote

Old   September 7, 2015, 09:21
Default
  #17
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Bruno thanks again,

I believe you're right in that the folders i've been given were still under development - unfortunately the lecturer he was working under was not following the coding side of the project and only helping analyse results so he hasn't been much help.

I've tried running another solver of a smaller case as an example for you and get the following error:
Code:
*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0
Exec   : constantdensityfireFoam
Date   : Sep 07 2015
Time   : 22:00:43
Host   : "alexei-OptiPlex-9010"
PID    : 6399
Case   : /home/alexei/OpenFOAM/alexei-2.2.0/changing_diff/nowhirl_0.05r_0.01in
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

Duplicate entry infinitelyFastChemistry<psiThermoCombustion,gasThermoPhysics> in runtime selection table psiCombustionModel
#0    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x25) [0x7f5aace18cd5]
#1    /home/alexei/OpenFOAM/alexei-2.2.0/platforms/linux64GccDPOpt/lib/libcustomcombustionModels.so(+0x1af66) [0x7f5aa6a74f66]
#2    /lib64/ld-linux-x86-64.so.2(+0xf306) [0x7f5ab2d8a306]
#3    /lib64/ld-linux-x86-64.so.2(+0xf3df) [0x7f5ab2d8a3df]
#4    /lib64/ld-linux-x86-64.so.2(+0x13ada) [0x7f5ab2d8eada]
#5    /lib64/ld-linux-x86-64.so.2(+0xf176) [0x7f5ab2d8a176]
#6    /lib64/ld-linux-x86-64.so.2(+0x1331a) [0x7f5ab2d8e31a]
#7    /lib/x86_64-linux-gnu/libdl.so.2(+0xf26) [0x7f5aac6b6f26]
#8    /lib64/ld-linux-x86-64.so.2(+0xf176) [0x7f5ab2d8a176]
#9    /lib/x86_64-linux-gnu/libdl.so.2(+0x152f) [0x7f5aac6b752f]
#10    /lib/x86_64-linux-gnu/libdl.so.2(dlopen+0x31) [0x7f5aac6b6fc1]
#11    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam6dlOpenERKNS_8fileNameEb+0x45) [0x7f5aace11d25]
#12    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam14dlLibraryTable4openERKNS_8fileNameEb+0x63) [0x7f5aacb7e7d3]
#13    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam14dlLibraryTable4openERKNS_10dictionaryERKNS_4wordE+0x9d) [0x7f5aacb7fa9d]
#14    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam4TimeC1ERKNS_4wordERKNS_7argListES3_S3_+0x63a) [0x7f5aacb9caea]
#15    constantdensityfireFoam() [0x42a058]
#16    /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f5aabb0578d]
#17    constantdensityfireFoam() [0x432181]
Duplicate entry infinitelyFastChemistry<psiThermoCombustion,constGasThermoPhysics> in runtime selection table psiCombustionModel
#0    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x25) [0x7f5aace18cd5]
#1    /home/alexei/OpenFOAM/alexei-2.2.0/platforms/linux64GccDPOpt/lib/libcustomcombustionModels.so(+0x1b062) [0x7f5aa6a75062]
#2    /lib64/ld-linux-x86-64.so.2(+0xf306) [0x7f5ab2d8a306]
#3    /lib64/ld-linux-x86-64.so.2(+0xf3df) [0x7f5ab2d8a3df]
#4    /lib64/ld-linux-x86-64.so.2(+0x13ada) [0x7f5ab2d8eada]
#5    /lib64/ld-linux-x86-64.so.2(+0xf176) [0x7f5ab2d8a176]
#6    /lib64/ld-linux-x86-64.so.2(+0x1331a) [0x7f5ab2d8e31a]
#7    /lib/x86_64-linux-gnu/libdl.so.2(+0xf26) [0x7f5aac6b6f26]
#8    /lib64/ld-linux-x86-64.so.2(+0xf176) [0x7f5ab2d8a176]
#9    /lib/x86_64-linux-gnu/libdl.so.2(+0x152f) [0x7f5aac6b752f]
#10    /lib/x86_64-linux-gnu/libdl.so.2(dlopen+0x31) [0x7f5aac6b6fc1]
#11    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam6dlOpenERKNS_8fileNameEb+0x45) [0x7f5aace11d25]
#12    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam14dlLibraryTable4openERKNS_8fileNameEb+0x63) [0x7f5aacb7e7d3]
#13    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam14dlLibraryTable4openERKNS_10dictionaryERKNS_4wordE+0x9d) [0x7f5aacb7fa9d]
#14    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam4TimeC1ERKNS_4wordERKNS_7argListES3_S3_+0x63a) [0x7f5aacb9caea]
#15    constantdensityfireFoam() [0x42a058]
#16    /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f5aabb0578d]
#17    constantdensityfireFoam() [0x432181]
Duplicate entry infinitelyFastChemistry<rhoThermoCombustion,gasThermoPhysics> in runtime selection table rhoCombustionModel
#0    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x25) [0x7f5aace18cd5]
#1    /home/alexei/OpenFOAM/alexei-2.2.0/platforms/linux64GccDPOpt/lib/libcustomcombustionModels.so(+0x1b00e) [0x7f5aa6a7500e]
#2    /lib64/ld-linux-x86-64.so.2(+0xf306) [0x7f5ab2d8a306]
#3    /lib64/ld-linux-x86-64.so.2(+0xf3df) [0x7f5ab2d8a3df]
#4    /lib64/ld-linux-x86-64.so.2(+0x13ada) [0x7f5ab2d8eada]
#5    /lib64/ld-linux-x86-64.so.2(+0xf176) [0x7f5ab2d8a176]
#6    /lib64/ld-linux-x86-64.so.2(+0x1331a) [0x7f5ab2d8e31a]
#7    /lib/x86_64-linux-gnu/libdl.so.2(+0xf26) [0x7f5aac6b6f26]
#8    /lib64/ld-linux-x86-64.so.2(+0xf176) [0x7f5ab2d8a176]
#9    /lib/x86_64-linux-gnu/libdl.so.2(+0x152f) [0x7f5aac6b752f]
#10    /lib/x86_64-linux-gnu/libdl.so.2(dlopen+0x31) [0x7f5aac6b6fc1]
#11    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam6dlOpenERKNS_8fileNameEb+0x45) [0x7f5aace11d25]
#12    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam14dlLibraryTable4openERKNS_8fileNameEb+0x63) [0x7f5aacb7e7d3]
#13    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam14dlLibraryTable4openERKNS_10dictionaryERKNS_4wordE+0x9d) [0x7f5aacb7fa9d]
#14    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam4TimeC1ERKNS_4wordERKNS_7argListES3_S3_+0x63a) [0x7f5aacb9caea]
#15    constantdensityfireFoam() [0x42a058]
#16    /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f5aabb0578d]
#17    constantdensityfireFoam() [0x432181]
Duplicate entry infinitelyFastChemistry<rhoThermoCombustion,constGasThermoPhysics> in runtime selection table rhoCombustionModel
#0    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x25) [0x7f5aace18cd5]
#1    /home/alexei/OpenFOAM/alexei-2.2.0/platforms/linux64GccDPOpt/lib/libcustomcombustionModels.so(+0x1afba) [0x7f5aa6a74fba]
#2    /lib64/ld-linux-x86-64.so.2(+0xf306) [0x7f5ab2d8a306]
#3    /lib64/ld-linux-x86-64.so.2(+0xf3df) [0x7f5ab2d8a3df]
#4    /lib64/ld-linux-x86-64.so.2(+0x13ada) [0x7f5ab2d8eada]
#5    /lib64/ld-linux-x86-64.so.2(+0xf176) [0x7f5ab2d8a176]
#6    /lib64/ld-linux-x86-64.so.2(+0x1331a) [0x7f5ab2d8e31a]
#7    /lib/x86_64-linux-gnu/libdl.so.2(+0xf26) [0x7f5aac6b6f26]
#8    /lib64/ld-linux-x86-64.so.2(+0xf176) [0x7f5ab2d8a176]
#9    /lib/x86_64-linux-gnu/libdl.so.2(+0x152f) [0x7f5aac6b752f]
#10    /lib/x86_64-linux-gnu/libdl.so.2(dlopen+0x31) [0x7f5aac6b6fc1]
#11    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam6dlOpenERKNS_8fileNameEb+0x45) [0x7f5aace11d25]
#12    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam14dlLibraryTable4openERKNS_8fileNameEb+0x63) [0x7f5aacb7e7d3]
#13    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam14dlLibraryTable4openERKNS_10dictionaryERKNS_4wordE+0x9d) [0x7f5aacb7fa9d]
#14    /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam4TimeC1ERKNS_4wordERKNS_7argListES3_S3_+0x63a) [0x7f5aacb9caea]
#15    constantdensityfireFoam() [0x42a058]
#16    /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f5aabb0578d]
#17    constantdensityfireFoam() [0x432181]
Create mesh for time = 0


Reading g
Creating combustion model

Selecting combustion model diffusion<rhoThermoCombustion,gasThermoPhysics>


--> FOAM FATAL ERROR: 
Unknown psiCombustionModel type diffusion<rhoThermoCombustion,gasThermoPhysics>

Valid  combustionModels are : 

8
(
noCombustion<psiThermoCombustion>
diffusion<psiThermoCombustion,constGasThermoPhysics>
PaSR<psiChemistryCombustion>
infinitelyFastChemistry<psiThermoCombustion,gasThermoPhysics>
FSD<psiThermoCombustion,gasThermoPhysics>
infinitelyFastChemistry<psiThermoCombustion,constGasThermoPhysics>
diffusion<psiThermoCombustion,gasThermoPhysics>
FSD<psiThermoCombustion,constGasThermoPhysics>
)


    From function psiCombustionModel::New
    in file psiCombustionModel/psiCombustionModel/psiCombustionModelNew.C at line 62.

FOAM exiting
the case I've run (nowhirl_0.05r_0.01in) , as well as the solver (constantdensityfireFoam) are in this dropbox:https://www.dropbox.com/sh/0tldmchii...OttANOlma?dl=0

The case is attempting to simulate a non-whirling fire under constant density conditions if this helps.


Kind regards,
Alexei
AlexKam is offline   Reply With Quote

Old   September 7, 2015, 18:30
Default
  #18
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Hi Alexei,

I won't be able to look into the case before the weekend, but from your description and the output error message, it feels like you didn't mention some important detail: did you compile/build any other library?
I ask this because the two error messages are implying that something is amiss with one or two libraries:
  1. The first error is pointing out that there are two objects of the same name loaded into memory, which means that more than one library has an object of the same name.
  2. The second error is pointing out that the selected thermodynamic model does not exist. Perhaps the wrong library was compiled?
Best regards,
Bruno
AlexKam likes this.
__________________
wyldckat is offline   Reply With Quote

Old   September 19, 2015, 22:17
Default
  #19
New Member
 
A. Kamitsis
Join Date: Aug 2015
Posts: 15
Rep Power: 10
AlexKam is on a distinguished road
Hi Bruno,

I've decided to just re-write the re-build the custom solver's and they seem to be working much better now, however I've tried running a case in parallel and received the following output (it was going ok for a little while before this), would you be able to offer any advice on this?

I've run:
Code:
 mpirun -np 8 dynamicDensity -parallel
and received this output

Code:
Courant Number mean: 7.06846e-07 max: 0.551005
deltaT = 1.29191e-22
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1029
    Increased the timePrecision from 152 to 153 to distinguish between timeNames at time 0.204108
Time = 0.2041082395427052109670995605483767576515674591064453125

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 9.05426e-11, Final residual = 9.05426e-11, No Iterations 0
DILUPBiCG:  Solving for Uy, Initial residual = 9.05425e-11, Final residual = 9.05425e-11, No Iterations 0
DILUPBiCG:  Solving for Uz, Initial residual = 9.05423e-11, Final residual = 9.05423e-11, No Iterations 0
DILUPBiCG:  Solving for O2, Initial residual = 5.91346e-08, Final residual = 5.91346e-08, No Iterations 0
DILUPBiCG:  Solving for H2O, Initial residual = 6.47461e-08, Final residual = 6.47461e-08, No Iterations 0
DILUPBiCG:  Solving for CH4, Initial residual = 9.28681e-08, Final residual = 9.28681e-08, No Iterations 0
DILUPBiCG:  Solving for CO2, Initial residual = 6.47461e-08, Final residual = 6.47461e-08, No Iterations 0
DILUPBiCG:  Solving for h, Initial residual = 8.66642e-09, Final residual = 8.66642e-09, No Iterations 0
min/max(T) = 200, 5000
GAMG:  Solving for p_rgh, Initial residual = 1.65213e-12, Final residual = 1.65213e-12, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 2.9777e-15, global = 2.49275e-18, cumulative = -0.000943226
GAMG:  Solving for p_rgh, Initial residual = 1.85273e-12, Final residual = 1.85273e-12, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 3.34043e-15, global = 2.50425e-18, cumulative = -0.000943226
DILUPBiCG:  Solving for k, Initial residual = 3.01901e-06, Final residual = 1.54484e-18, No Iterations 1
bounding k, min: 1e-15 max: 1.03582e+07 average: 282.151
ExecutionTime = 542.76 s  ClockTime = 557 s

Courant Number mean: 7.06846e-07 max: 0.551005
deltaT = 1.17232e-22
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1029
    Increased the timePrecision from 153 to 154 to distinguish between timeNames at time 0.204108
Time = 0.2041082395427052109670995605483767576515674591064453125

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 9.05426e-11, Final residual = 9.05426e-11, No Iterations 0
DILUPBiCG:  Solving for Uy, Initial residual = 9.05426e-11, Final residual = 9.05426e-11, No Iterations 0
DILUPBiCG:  Solving for Uz, Initial residual = 9.05424e-11, Final residual = 9.05424e-11, No Iterations 0
DILUPBiCG:  Solving for O2, Initial residual = 5.91346e-08, Final residual = 5.91346e-08, No Iterations 0
DILUPBiCG:  Solving for H2O, Initial residual = 6.47461e-08, Final residual = 6.47461e-08, No Iterations 0
DILUPBiCG:  Solving for CH4, Initial residual = 9.28681e-08, Final residual = 9.28681e-08, No Iterations 0
DILUPBiCG:  Solving for CO2, Initial residual = 6.47461e-08, Final residual = 6.47461e-08, No Iterations 0
DILUPBiCG:  Solving for h, Initial residual = 1.0519e-08, Final residual = 3.68864e-21, No Iterations 1
min/max(T) = 200, 5000
GAMG:  Solving for p_rgh, Initial residual = 3.07879e-06, Final residual = 3.24144e-15, No Iterations 1
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 5.95489e-15, global = -5.85787e-15, cumulative = -0.000943226
GAMG:  Solving for p_rgh, Initial residual = 3.46474e-12, Final residual = 3.46474e-12, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 4.59862e-16, global = 6.04504e-19, cumulative = -0.000943226
DILUPBiCG:  Solving for k, Initial residual = 3.35215e-06, Final residual = 1.71052e-18, No Iterations 1
bounding k, min: 1e-15 max: 1.03582e+07 average: 282.163
ExecutionTime = 543.29 s  ClockTime = 558 s

Courant Number mean: 8.53153e-07 max: 0.665054
deltaT = 8.81371e-23
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1029
    Increased the timePrecision from 154 to 155 to distinguish between timeNames at time 0.204108
Time = 0.2041082395427052109670995605483767576515674591064453125

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 7.50155e-11, Final residual = 7.50155e-11, No Iterations 0
DILUPBiCG:  Solving for Uy, Initial residual = 7.50155e-11, Final residual = 7.50155e-11, No Iterations 0
DILUPBiCG:  Solving for Uz, Initial residual = 7.50153e-11, Final residual = 7.50153e-11, No Iterations 0
DILUPBiCG:  Solving for O2, Initial residual = 5.91346e-08, Final residual = 5.91346e-08, No Iterations 0
DILUPBiCG:  Solving for H2O, Initial residual = 6.47461e-08, Final residual = 6.47461e-08, No Iterations 0
DILUPBiCG:  Solving for CH4, Initial residual = 9.28681e-08, Final residual = 9.28681e-08, No Iterations 0
DILUPBiCG:  Solving for CO2, Initial residual = 6.47461e-08, Final residual = 6.47461e-08, No Iterations 0
DILUPBiCG:  Solving for h, Initial residual = 1.29364e-09, Final residual = 1.29364e-09, No Iterations 0
min/max(T) = 200, 5000
GAMG:  Solving for p_rgh, Initial residual = 6.24552e-12, Final residual = 6.24552e-12, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.12917e-14, global = -8.80768e-15, cumulative = -0.000943226
GAMG:  Solving for p_rgh, Initial residual = 6.41168e-12, Final residual = 6.41168e-12, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.15923e-14, global = -8.80767e-15, cumulative = -0.000943226
DILUPBiCG:  Solving for k, Initial residual = 3.08592e-06, Final residual = 1.30013e-18, No Iterations 1
bounding k, min: 1e-15 max: 1.03582e+07 average: 282.175
ExecutionTime = 543.82 s  ClockTime = 558 s

Courant Number mean: 7.06846e-07 max: 0.551005
deltaT = 7.99785e-23
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1029
    Increased the timePrecision from 155 to 156 to distinguish between timeNames at time 0.204108
Time = 0.2041082395427052109670995605483767576515674591064453125

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 7.50155e-11, Final residual = 7.50155e-11, No Iterations 0
DILUPBiCG:  Solving for Uy, Initial residual = 7.50155e-11, Final residual = 7.50155e-11, No Iterations 0
DILUPBiCG:  Solving for Uz, Initial residual = 7.50153e-11, Final residual = 7.50153e-11, No Iterations 0
DILUPBiCG:  Solving for O2, Initial residual = 5.91346e-08, Final residual = 5.91346e-08, No Iterations 0
DILUPBiCG:  Solving for H2O, Initial residual = 6.47461e-08, Final residual = 6.47461e-08, No Iterations 0
DILUPBiCG:  Solving for CH4, Initial residual = 9.28681e-08, Final residual = 9.28681e-08, No Iterations 0
DILUPBiCG:  Solving for CO2, Initial residual = 6.47461e-08, Final residual = 6.47461e-08, No Iterations 0
DILUPBiCG:  Solving for h, Initial residual = 1.56629e-09, Final residual = 1.56629e-09, No Iterations 0
min/max(T) = 200, 5000
GAMG:  Solving for p_rgh, Initial residual = 1.37483e-12, Final residual = 1.37483e-12, No Iterations 0
[1] #0  Foam::error::printStack(Foam::Ostream&) in "/home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #1  Foam::sigFpe::sigHandler(int) in "/home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #2   in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #4  void Foam::divide<Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/alexei/OpenFOAM/alexei-2.2.0/platforms/linux64GccDPOpt/bin/dynamicDensity"
[1] #5  
[1]  in "/home/alexei/OpenFOAM/alexei-2.2.0/platforms/linux64GccDPOpt/bin/dynamicDensity"
[1] #6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #7  
[1]  in "/home/alexei/OpenFOAM/alexei-2.2.0/platforms/linux64GccDPOpt/bin/dynamicDensity"
[alexei-OptiPlex-9010:05924] *** Process received signal ***
[alexei-OptiPlex-9010:05924] Signal: Floating point exception (8)
[alexei-OptiPlex-9010:05924] Signal code:  (-6)
[alexei-OptiPlex-9010:05924] Failing at address: 0x3e800001724
[alexei-OptiPlex-9010:05924] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x36570) [0x7ff8b48dc570]
[alexei-OptiPlex-9010:05924] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7ff8b48dc4f5]
[alexei-OptiPlex-9010:05924] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x36570) [0x7ff8b48dc570]
[alexei-OptiPlex-9010:05924] [ 3] /home/alexei/OpenFOAM/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKNS_5UListIdEES6_+0xe6) [0x7ff8b5b0bfe6]
[alexei-OptiPlex-9010:05924] [ 4] dynamicDensity(_ZN4Foam6divideINS_13fvsPatchFieldENS_11surfaceMeshEEEvRNS_14GeometricFieldIdT_T0_EERKS6_S9_+0x3e) [0x45316e]
[alexei-OptiPlex-9010:05924] [ 5] dynamicDensity() [0x428b26]
[alexei-OptiPlex-9010:05924] [ 6] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7ff8b48c778d]
[alexei-OptiPlex-9010:05924] [ 7] dynamicDensity() [0x42cfad]
[alexei-OptiPlex-9010:05924] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 1 with PID 5924 on node alexei-OptiPlex-9010 exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------
Kind Regards,
Alexei
AlexKam is offline   Reply With Quote

Old   September 20, 2015, 06:36
Default
  #20
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Hi Alexei,

Quote:
Originally Posted by AlexKam View Post
Code:
Courant Number mean: 7.06846e-07 max: 0.551005
deltaT = 1.29191e-22
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1029
    Increased the timePrecision from 152 to 153 to distinguish between timeNames at time 0.204108
Time = 0.2041082395427052109670995605483767576515674591064453125

...

bounding k, min: 1e-15 max: 1.03582e+07 average: 282.151
These two sections hint that things aren't going well, long before the crash:
  • The first issue is due to the deltaT having to be made so small in order to be able to have the Courant Number around and below the 0.5 limit.
  • The second issue is related to the flow being highly unstable, which leads to high turbulence values.
This is either due to a bad mesh or there is some chemical reaction that is giving an explosion as or more intense than the sun Or rho varying too much or too little...


My advice: baby steps. Don't try to isolate 100 problems all at once, create small test cases and isolate one problem at a time.


Best regards,
Bruno
AlexKam likes this.
__________________
wyldckat is offline   Reply With Quote

Reply
Page 1 of 2 1 2

« Previous Thread | Next Thread »

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
[ANSYS Meshing] Help with element size sandri_92 ANSYS Meshing & Geometry 14 November 14, 2018 07:54
Segmentation fault running waveDyMFoam solver (mod. interDyMFoam solver - waves2Foam) Ed R OpenFOAM Running, Solving & CFD 5 July 2, 2013 11:36
Problems running customized solver for diffusion mmkr825 OpenFOAM Running, Solving & CFD 1 August 30, 2012 14:01
problem in running a modified solver adambarfi OpenFOAM 5 August 10, 2012 15:52
CFX 5.5 Roued CFX 1 October 2, 2001 16:49


All times are GMT -4. The time now is 18:23.

Contact Us - CFD Online - Privacy Statement - Top