|
[Sponsors] |
Symbol look up error while compiling new library |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Aju Abraham
Join Date: Jul 2019
Posts: 4
Rep Power: 7 ![]() |
Dear Foamers,
I need an urgent help in resolving an issue in implementing something in my Master Thesis. My requirement is to make the following thermophysical model combination work for the sprayFoam solver thermoType { type hePsiThermo; mixture reactingMixture; transport polynomial; thermo hPolynomial; energy sensibleEnthalpy; equationOfState perfectGas; specie specie; } I get the following error as expected as the combination is not defined in the thermypysical model: /*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 6 \\/ M anipulation | \*---------------------------------------------------------------------------*/ Build : 6-e29811f5dff8 Exec : mysprayFoam Date : Jul 23 2019 Time : 15:40:35 Host : "aju-HP-Pavilion-g6-Notebook-PC" PID : 5302 I/O : uncollated Case : /home/aju/OpenFOAM/aju-6/run/sprayFoam/trial nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 PIMPLE: No convergence criteria found PIMPLE: Operating solver in PISO mode Reading g Reading thermophysical properties Selecting thermodynamics package { type hePsiThermo; mixture reactingMixture; transport polynomial; thermo hPolynomial; energy sensibleEnthalpy; equationOfState perfectGas; specie specie; } --> FOAM FATAL ERROR: Unknown psiReactionThermo type thermoType { type hePsiThermo; mixture reactingMixture; transport polynomial; thermo hPolynomial; energy sensibleEnthalpy; equationOfState perfectGas; specie specie; } Valid psiReactionThermo types are: 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 const hConst perfectGas specie sensibleInternalEnergy hePsiThermo multiComponentMixture sutherland janaf perfectGas specie sensibleEnthalpy hePsiThermo multiComponentMixture sutherland janaf perfectGas specie sensibleInternalEnergy hePsiThermo pureMixture const hConst perfectGas specie sensibleEnthalpy hePsiThermo pureMixture const hConst perfectGas specie sensibleInternalEnergy hePsiThermo pureMixture sutherland janaf perfectGas specie sensibleEnthalpy hePsiThermo pureMixture sutherland janaf perfectGas specie sensibleInternalEnergy hePsiThermo reactingMixture const hConst perfectGas specie sensibleEnthalpy hePsiThermo reactingMixture const hConst perfectGas specie sensibleInternalEnergy hePsiThermo reactingMixture sutherland janaf perfectGas specie sensibleEnthalpy hePsiThermo reactingMixture sutherland janaf perfectGas specie sensibleInternalEnergy hePsiThermo singleStepReactingMixture sutherland janaf perfectGas specie sensibleEnthalpy hePsiThermo singleStepReactingMixture sutherland janaf perfectGas specie sensibleInternalEnergy hePsiThermo veryInhomogeneousMixture const hConst perfectGas specie sensibleEnthalpy hePsiThermo veryInhomogeneousMixture sutherland hConst perfectGas specie sensibleEnthalpy hePsiThermo veryInhomogeneousMixture sutherland janaf perfectGas specie sensibleEnthalpy From function static typename Table::iterator Foam::basicThermo::lookupThermo(const Foam::dictionary&, Table*, int, const char**, const Foam::word&) [with Thermo = Foam: ![]() ![]() ![]() in file /home/ubuntu/OpenFOAM/OpenFOAM-6/src/thermophysicalModels/basic/lnInclude/basicThermoTemplates.C at line 46. FOAM exiting I compiled a new library libreactionThermophysicalModels.so adding the new model. The compile works successfully but when the solver sprayFoam is run, I get the following error: mysprayFoam: symbol lookup error: /home/aju/OpenFOAM/aju-6/platforms/linux64GccDPInt32Opt/lib/libreactionThermophysicalModels.so: undefined symbol: _ZN4Foam15chemistryReaderINS_19polynomialTransport INS_7species6thermoINS_17hPolynomialThermoINS_10pe rfectGasINS_6specieEEELi8EEENS_16sensibleEnthalpyE EELi8EEEE30dictionaryConstructorTablePtr_E What could possibly be wrong? I am quite new with the solver and compiler stuffs in openfoam |
|
![]() |
![]() |
![]() |
![]() |
#2 |
New Member
Christian
Join Date: Jun 2019
Posts: 14
Rep Power: 7 ![]() |
Can you please give some details about how you created your thermophysical model?
Make sure that you add your new thermoType Code:
thermoType { type hePsiThermo; mixture reactingMixture; transport polynomial; thermo hPolynomial; energy sensibleEnthalpy; equationOfState perfectGas; specie specie; } |
|
![]() |
![]() |
![]() |
![]() |
#3 | |
New Member
Aju Abraham
Join Date: Jul 2019
Posts: 4
Rep Power: 7 ![]() |
Quote:
Hi, Thanks a lot for your reply. But there is no file named hePsiThermos.C in that folder. Only PsiThermos.C is available, which contains only those types of pureMixture and not reactingMixture. I started the implementation new again, to avoid any more confusion,as follows:
Code:
makeReactionThermos ( psiThermo, psiReactionThermo, hePsiThermo, veryInhomogeneousMixture, polynomialTransport, sensibleEnthalpy, hPolynomialThermo, perfectGas, specie );
Code:
EXE_INC = \ -I$(LIB_SRC)/transportModels/compressible/lnInclude \ -I$(WM_PROJECT_USER_DIR)/src/myThermophysicalModels/myBasic/lnInclude \ -I$(WM_PROJECT_USER_DIR)/src/myThermophysicalModels/mySpecie/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/solidSpecie/lnInclude \ -I$(LIB_SRC)/finiteVolume/lnInclude LIB_LIBS = \ -L$(FOAM_USER_LIBBIN) \ -lcompressibleTransportModels \ -lfluidThermophysicalModels \ -lspecie \ -lsolidSpecie \ -lfiniteVolume
Code:
EXE_INC = \ -I. \ -I$(FOAM_SOLVERS)/lagrangian/reactingParcelFoam \ -I$(LIB_SRC)/finiteVolume/lnInclude \ -I$(LIB_SRC)/meshTools/lnInclude \ -I$(LIB_SRC)/sampling/lnInclude \ -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \ -I$(LIB_SRC)/TurbulenceModels/compressible/lnInclude \ -I$(LIB_SRC)/lagrangian/basic/lnInclude \ -I$(LIB_SRC)/lagrangian/intermediate/lnInclude \ -I$(LIB_SRC)/lagrangian/spray/lnInclude \ -I$(LIB_SRC)/lagrangian/distributionModels/lnInclude \ -I$(WM_PROJECT_USER_DIR)/src/myThermophysicalModels/mySpecie/lnInclude \ -I$(LIB_SRC)/transportModels/compressible/lnInclude \ -I$(WM_PROJECT_USER_DIR)/src/myThermophysicalModels/myBasic/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/thermophysicalProperties/lnInclude \ -I$(WM_PROJECT_USER_DIR)/src/myThermophysicalModels/myreactionThermo/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/SLGThermo/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/chemistryModel/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/radiation/lnInclude \ -I$(LIB_SRC)/ODE/lnInclude \ -I$(LIB_SRC)/regionModels/regionModel/lnInclude \ -I$(LIB_SRC)/regionModels/surfaceFilmModels/lnInclude \ -I$(LIB_SRC)/combustionModels/lnInclude EXE_LIBS = \ -L$(FOAM_USER_LIBBIN) \ -lturbulenceModels \ -lcompressibleTurbulenceModels \ -llagrangian \ -llagrangianIntermediate \ -llagrangianTurbulence \ -llagrangianSpray \ -lspecie \ -lcompressibleTransportModels \ -lfluidThermophysicalModels \ -lthermophysicalProperties \ -lreactionThermophysicalModels \ -lSLGThermo \ -lchemistryModel \ -lradiationModels \ -lODE \ -lregionModels \ -lsurfaceFilmModels \ -lcombustionModels \ -lfiniteVolume \ -lfvOptions \
Code:
mysprayFoam: symbol lookup error: /home/aju/OpenFOAM/aju-6/platforms/linux64GccDPInt32Opt/lib/libreactionThermophysicalModels.so: undefined symbol: _ZN4Foam15chemistryReaderINS_19polynomialTransportINS_7species6thermoINS_17hPolynomialThermoINS_10perfectGasINS_6specieEEELi8EEENS_16sensibleEnthalpyEEELi8EEEE30dictionaryConstructorTablePtr_E NB: I use Openfoam version 6 Last edited by ajucgnr; July 27, 2019 at 08:00. Reason: Improve code readability |
||
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Christian
Join Date: Jun 2019
Posts: 14
Rep Power: 7 ![]() |
Did you include "polynomialTransport.H" and "hPolynomialThermo.H" in"psiReactionThermos.C"?
|
|
![]() |
![]() |
![]() |
![]() |
#5 | |
New Member
Aju Abraham
Join Date: Jul 2019
Posts: 4
Rep Power: 7 ![]() |
Quote:
Hi, Yes I did include those already.I actually resolved my issue ![]() The problem was that any new additons of thermophysical model has to be updated in all the corresponding files too. So basically, apart from the above files, I had to update all the below files too:
Code:
typedef polynomialTransport < species::thermo < hPolynomialThermo < perfectGas<specie> >, sensibleEnthalpy >, 8 > gasPoly8HThermoPhysics;
Code:
makeChemistryReaderType(foamChemistryReader, gasPoly8HThermoPhysics);
Code:
makeChemistryModelType ( TDACChemistryModel, psiReactionThermo, gasPoly8HThermoPhysics ); makeChemistryModelType ( StandardChemistryModel, psiReactionThermo, gasPoly8HThermoPhysics );
Code:
makeChemistrySolverTypes(psiReactionThermo, gasPoly8HThermoPhysics);
Code:
makeChemistryReductionMethods(psiReactionThermo, gasPoly8HThermoPhysics);
Code:
makeChemistryTabulationMethods(psiReactionThermo, gasPoly8HThermoPhysics); |
||
![]() |
![]() |
![]() |
Tags |
compiling new library, psireactionthermo, sprayfoam |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Caffa 3D code | Waliur Rahman | Main CFD Forum | 0 | May 29, 2018 00:53 |
using METIS functions in fortran | dokeun | Main CFD Forum | 7 | January 29, 2013 04:06 |
OpenFOAM install on Ubuntu Natty 11.04 | bkubicek | OpenFOAM | 13 | May 26, 2011 05:48 |
POSDAT problem | piotka | STAR-CD | 4 | June 12, 2009 08:43 |
Errors running allwmake in OpenFOAM141dev with WM_COMPILE_OPTION%3ddebug | unoder | OpenFOAM Installation | 11 | January 30, 2008 20:30 |