[sebastian]

Hi,

I know, this question has already been discussed (http://www.cfd-online.com/Forums/ope...roperties.html). But the answer has not been very helpful to me.

I am having exactly the same problem. Im trying to use the hPolynomialThermo for a temperaturedependent Cp.

hPsiMixtureThermo<pureMixture<sutherlandTransport< specieThermo<hPolynomialThermo<perfectGas>>>>
or
hPsiMixtureThermo<pureMixture<constantTransport<sp ecieThermo<hPolynomialThermo<perfectGas>>>>

But OpenFoam gives back

Unknown basicPsiThermo type hPsiMixtureThermo<pureMixture<sutherlandTransport< specieThermo<hPolynomialThermo<perfectGas>>>>>

Valid basicPsiThermo types are:

8
(
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<eConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
)

I can not find anything on the web about that. Which conditions must be met, or which combination must be used, in order to be able to use the hPolynomialThermo?

Another question would be, how to set the polynomial? Something like that:


mixture //keyword
air 1 28.9 //specie
1035.887 -0.255611 0.0006258047 2.627558e-07 //hPolynomialThermo, polynomial for Cp
1.458e-05 110.4; //sutherlandTransport


I woud be very appreciated to get an answer . Thanks!


Sebastian

[herbert]

Hi Sebastian,

I have had the same problem and solved it recently by changing thermophysicalModels/basic library. I have implemented it in a way that allows using polynomialTransport and polynomialThermo at the same time. I will point out what to do (sorry for formatting not being perfect):

1. Add a second constructor in psiThermo/makeBasicPsiThermo.H that can take additional arguments to be able to specify the order of the polynomial to be used
   

   #ifndef makeBasicPsiPolyThermo_H
   #define makeBasicPsiPolyThermo_H
   
   #include "basicPsiThermo.H"
   #include "addToRunTimeSelectionTable.H"
   
   // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
   
   #define makeBasicPsiPolyThermo(Cthermo,Mixture,Transport,orderTransport,Thermo,orderThermo,EqnOfState)  \
                                                                                                           \
   typedef Cthermo<Mixture<Transport<specieThermo<Thermo<EqnOfState, orderThermo> > , orderTransport> > >  \
       Cthermo##Mixture##Transport##orderTransport##Thermo##orderThermo##EqnOfState;                       \
                                                                                                           \
   defineTemplateTypeNameAndDebugWithName                                                                  \
   (                                                                                                       \
       Cthermo##Mixture##Transport##orderTransport##Thermo##orderThermo##EqnOfState,                       \
       #Cthermo                                                                                            \
           "<"#Mixture"<"#Transport#orderTransport"<specieThermo<"#Thermo#orderThermo"<"#EqnOfState">>>>>",\
       0                                                                                                   \
   );                                                                                                      \
                                                                                                           \
   addToRunTimeSelectionTable                                                                              \
   (                                                                                                       \
       basicPsiThermo,                                                                                     \
       Cthermo##Mixture##Transport##orderTransport##Thermo##orderThermo##EqnOfState,                       \
       fvMesh                                                                                              \
   )
   
   #endif

2. Declare your model combination in psiThermo/hPsiThermo/hPsiThermos.C (e.g. using 4th order polynomial for cp and 3rd order for transportProperties but here you can choose any order combination you want)
   

   makeBasicPsiPolyThermo
   (
       hPsiThermo,
       pureMixture,
       polynomialTransport,
       3,
       hPolynomialThermo,
       4,
       perfectGas
   );

3. Add an modified constructor to mixtures/basicMixture/makeBasicMixture.H, too
   

   #ifndef makeBasicPsiPolyThermo_H
   #define makeBasicPsiPolyThermo_H
   
   #include "basicMixture.H"
   
   // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
   
   
   #define makeBasicPolyMixture(Mixture,Transport,orderTransport,Thermo,orderThermo,EqnOfState)      \
                                                                                                     \
   typedef Mixture<Transport<specieThermo<Thermo<EqnOfState, orderThermo> > , orderTransport> >      \
       Mixture##Transport##orderTransport##Thermo##orderThermo##EqnOfState;                          \
                                                                                                     \
   defineTemplateTypeNameAndDebugWithName                                                            \
   (                                                                                                 \
       Mixture##Transport##orderTransport##Thermo##orderThermo##EqnOfState,                          \
       #Mixture"<"#Transport#orderTransport"<specieThermo<"#Thermo#orderThermo"<"#EqnOfState">>>>>", \
       0                                                                                             \
   );                                                                                                \
   
   #endif

4. Declare your model combination again in mixture/basicMixture/basicMixtures.C
   

   makeBasicPolyMixture
   (
       pureMixture,
       polynomialTransport,
       3,
       hPolynomialThermo,
       4,
       perfectGas
   );

In your constant/thermophysicalProperties you have to call this by using

thermoType  hPsiThermo<pureMixture<polynomialTransport3<specieThermo<hPolynomialThermo4<perfectGas>>>>>;

mixture  air 
         1 //nMoles (??)
         28.32708688 //molecular weight [kg/kmol]
         0.0 //standard formation enthalpy [J/kg]
         0.0 //standard formation enthropy [J/kg]
         cpPolynomial (9.86931771e02 1.73030395e-01 6.64980490e-05 1.25487e-09)//heat capacity [J/kgK]
         muPolynomial (4.70335908e-06 4.67918313e-08 -1.09914897e-11) //dynamic viscosity [kg/ms]
         kappaPolynomial (4.64248147e-03 7.28706102e-05 -6.13777213e-09); //heat conductivity [W/mK]

I hope there are not too much mistakes caused by copy/paste .

Kind regards,
Stefan

[herbert]

Hi everyone,

if anyone uses this piece of code, could you please report how it works and if there arise any problems? I have already tested it but you can never be sure.

Regards,
Stefan

[Chrisi1984]

Hi Herbert,

I would like to test your thermophysical model.

Is there any new compilation necessary?

Should I make a backup of may original files or should I do not change the original files and create instead of new files?

Thanks in advance!

Best regards
Chrisi

[herbert]

Hi Chrisi,

I'd recommend to copy the $FOAM_SRC/thermophysicalModels/basic/ to your $WM_PROJECT_USER_DIR/lib, make the changes I pointed out in my previous post and compile it to $FOAM_USER_LIBBIN. So the original files are not replaced.

To use it with your solver, you should have to edit the Make/options and recompile the solver.

Have a lot of fun
Stefan

[Chrisi1984]

Hi,

I did exactly what you said.

But how can I complie it to $FOAM_USER_LIBBIN?

Can you give me a detailed discription how to compile everything correctly?

Regards Chrisi

[sebastian]

Hi Stefan!

Wow, thanks a lot for that detailed instruction!

I have implemented it into the Code. It compiled without an error. But when I am solving it, it gives me back an error again:


Reading thermophysical properties



ill defined primitiveEntry starting at keyword 'mixture' on line 22 and ending at line 30

file: /home/sebastian/OpenFOAM/sebastian-1.6/run_rhoSimpleThermo/constant/thermophysicalProperties at line 30.

From function primitiveEntry::readEntry(const dictionary&, Istream&)
in file db/dictionary/primitiveEntry/primitiveEntryIO.C at line 210.

FOAM exiting


Here, thats my thermo File:


thermoType hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hPolynomialThermo4<perfectGas>>>>>;


mixture //keyword
air 1 28.9 //specie / specieCoeffs
//1007 0 //hConstThermo / thermoCoeffs
cpPolynomial(1035.887 -0.255611 0.0006258047 -2.627558e-07) //hPolynomialThermo / thermoCoeffs
1.458e-05 110.4; //sutherlandTransport / transportCoeffs



Best wishes,
Sebastian

[herbert]

Originally Posted by Chrisi1984

But how can I complie it to $FOAM_USER_LIBBIN?

Just replace

LIB=$(FOAM_LIBBIN)/libbasicThermophysicalModels

by e.g.

LIB=$(FOAM_USER_LIBBIN)/libuserBasicThermophysicalModels

in basic/Make/files and compile with wmake libso.

Later in your solvers Make/options replace -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude by -I$(WM_PROJECT_USER_DIR)/lib/"path to your lnInclude" and for EXE_LIBS replace -lbasicThermophysicalModels by $(FOAM_USER_LIBBIN)/libuserBasicThermophysicalModels.so

Hope it helps,
Stefan

[herbert]

Dear Sebastian,

please try what happens, if you put two additional scalars before cpPolynomial. I'm not quite sure, but I think there should be standard enthalpy and entropy of formation be added.

Good luck,
Stefan

[Chrisi1984]

Hi Stefan,

Thank you so much for your help!

But I have got a probleme compiling the new model. This is my error message. It is in german but I think I need not translate it for you .

root@chrisilinux:/media/DATA/Daten/Chrisi_Dokumente/Studium/Masterarbeit/lib/src/thermophysicalModels/basic# wmake libso
Making dependency list for source file mixtures/basicMixture/basicMixture.C
Making dependency list for source file mixtures/basicMixture/basicMixtures.C
Making dependency list for source file basicThermo/basicThermo.C
Making dependency list for source file psiThermo/basicPsiThermo/basicPsiThermo.C
Making dependency list for source file psiThermo/basicPsiThermo/newBasicPsiThermo.C
Making dependency list for source file psiThermo/hPsiThermo/hPsiThermos.C
Making dependency list for source file psiThermo/ePsiThermo/ePsiThermos.C
Making dependency list for source file rhoThermo/basicRhoThermo/basicRhoThermo.C
Making dependency list for source file rhoThermo/basicRhoThermo/newBasicRhoThermo.C
Making dependency list for source file rhoThermo/hRhoThermo/hRhoThermos.C
Making dependency list for source file derivedFvPatchFields/fixedEnthalpy/fixedEnthalpyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/gradientEnthalpy/gradientEnthalpyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/mixedEnthalpy/mixedEnthalpyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/fixedInternalEnergy/fixedInternalEnergyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/gradientInternalEnergy/gradientInternalEnergyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/mixedInternalEnergy/mixedInternalEnergyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/wallHeatTransfer/wallHeatTransferFvPatchScalarField.C
SOURCE=mixtures/basicMixture/basicMixture.C ; g++ -m32 -Dlinux -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/root/OpenFOAM/OpenFOAM-1.6.x/src/finiteVolume/lnInclude -I/root/OpenFOAM/OpenFOAM-1.6.x/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/root/OpenFOAM/OpenFOAM-1.6.x/src/OpenFOAM/lnInclude -I/root/OpenFOAM/OpenFOAM-1.6.x/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linuxGccDPOpt/basicMixture.o
SOURCE=mixtures/basicMixture/basicMixtures.C ; g++ -m32 -Dlinux -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/root/OpenFOAM/OpenFOAM-1.6.x/src/finiteVolume/lnInclude -I/root/OpenFOAM/OpenFOAM-1.6.x/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/root/OpenFOAM/OpenFOAM-1.6.x/src/OpenFOAM/lnInclude -I/root/OpenFOAM/OpenFOAM-1.6.x/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linuxGccDPOpt/basicMixtures.o
mixtures/basicMixture/basicMixtures.C:97: Fehler: »polynomialTransport« wurde in diesem Gültigkeitsbereich nicht definiert
mixtures/basicMixture/basicMixtures.C:97: Fehler: »hPolynomialThermo« wurde in diesem Gültigkeitsbereich nicht definiert
mixtures/basicMixture/basicMixtures.C:97: Fehler: falsche Anzahl der Templateargumente (2, sollte 1 sein)
/root/OpenFOAM/OpenFOAM-1.6.x/src/thermophysicalModels/specie/lnInclude/specieThermo.H:49: Fehler: für »template<class thermo> class Foam::specieThermo« bereitgestellt
mixtures/basicMixture/basicMixtures.C:97: Fehler: Templateargument 1 ist ungültig
mixtures/basicMixture/basicMixtures.C:97: Fehler: expected unqualified-id before »,« token
mixtures/basicMixture/basicMixtures.C:97: Fehler: expected unqualified-id before numeric constant
mixtures/basicMixture/basicMixtures.C:97: Fehler: »pureMixturepolynomialTransport3hPolynomialThermo4 perfectGas« has not been declared
mixtures/basicMixture/basicMixtures.C:97: Fehler: »pureMixturepolynomialTransport3hPolynomialThermo4 perfectGas« has not been declared
mixtures/basicMixture/basicMixtures.C:97: Warnung: Variable »Foam::debug« wird nicht verwendet
make: *** [Make/linuxGccDPOpt/basicMixtures.o] Fehler 1

Have you got an idea where the error comes from?

Regards Chrisi

[herbert]

Dear Chrisi,

I'm sorry, I've forgotten to mention a detail. You have to include additional files into the header of hPsiThermos.C and basicMixtures.C to define polynomialTransport and hPolynomialThermo, respectivley. Just add

#include "hPolynomialThermo.H"
#include "polynomialTransport.H"

Hope it works now,
Stefan

[Chrisi1984]

Hi Stefan,

Thank you again. Without your help I would have never been able to compile it.

I succeded compiling the new model but first I got this error:

/cfd/externe-ma/Alt/lib/src/thermophysicalModels/basic >wmake libso
Making dependency list for source file mixtures/basicMixture/basicMixture.C
Making dependency list for source file mixtures/basicMixture/basicMixtures.C
Making dependency list for source file basicThermo/basicThermo.C
Making dependency list for source file psiThermo/basicPsiThermo/basicPsiThermo.C
Making dependency list for source file psiThermo/basicPsiThermo/newBasicPsiThermo.C
Making dependency list for source file psiThermo/hPsiThermo/hPsiThermos.C
Making dependency list for source file psiThermo/ePsiThermo/ePsiThermos.C
Making dependency list for source file rhoThermo/basicRhoThermo/basicRhoThermo.C
Making dependency list for source file rhoThermo/basicRhoThermo/newBasicRhoThermo.C
Making dependency list for source file rhoThermo/hRhoThermo/hRhoThermos.C
Making dependency list for source file derivedFvPatchFields/fixedEnthalpy/fixedEnthalpyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/gradientEnthalpy/gradientEnthalpyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/mixedEnthalpy/mixedEnthalpyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/fixedInternalEnergy/fixedInternalEnergyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/gradientInternalEnergy/gradientInternalEnergyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/mixedInternalEnergy/mixedInternalEnergyFvPatchScalarField.C
Making dependency list for source file derivedFvPatchFields/wallHeatTransfer/wallHeatTransferFvPatchScalarField.C
SOURCE=mixtures/basicMixture/basicMixture.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/basicMixture.o
SOURCE=mixtures/basicMixture/basicMixtures.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/basicMixtures.o
SOURCE=basicThermo/basicThermo.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/basicThermo.o
SOURCE=psiThermo/basicPsiThermo/basicPsiThermo.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/basicPsiThermo.o
SOURCE=psiThermo/basicPsiThermo/newBasicPsiThermo.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/newBasicPsiThermo.o
SOURCE=psiThermo/hPsiThermo/hPsiThermos.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/hPsiThermos.o
In file included from psiThermo/hPsiThermo/hPsiThermos.C:27:
lnInclude/makeBasicPsiThermo.H:86:2: error: #endif without #if
make: *** [Make/linux64GccDPOpt/hPsiThermos.o] Error 1

Then I removed the endif it complained about, at then it run.

I hope this will not cause a problem later?




But know I try to recompile my solver like you told me. What did you mean with "path to your lnInclude"? Should this be the absolut path? Must it be in "" or not?

At the moment I am getting this error message:

/cfd/externe-ma/Alt/applications/solvers/compressible/rhoPorousSimpleFoam_poly >wmake
Making dependency list for source file rhoPorousSimpleFoam_poly.C
could not open file basicPsiThermo.H for source file rhoPorousSimpleFoam_poly.C
could not open file basicThermo.H for source file rhoPorousSimpleFoam_poly.C
SOURCE=rhoPorousSimpleFoam_poly.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/home/user/e18980/OpenFOAM/e18980-1.6/lib/"/cfd/externe-ma/Alt/lib/src/thermophysicalModels/basic/lnInclude" -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/cfdTools -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/meshTools/lnInclude -IlnInclude -I. -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/rhoPorousSimpleFoam_poly.o
rhoPorousSimpleFoam_poly.C:35:28: error: basicPsiThermo.H: No such file or directory
In file included from /cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:48,
from rhoPorousSimpleFoam_poly.C:36:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:52:25: error: basicThermo.H: No such file or directory
In file included from /cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:48,
from rhoPorousSimpleFoam_poly.C:36:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:85: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:85: error: expected ‘;’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:130: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:131: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:142: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:143: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:172: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:172: error: expected ‘;’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:178: error: expected `;' before ‘const’
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In static member function ‘static Foam::autoPtr<Foam::compressible::turbulenceModel> Foam::compressible::turbulenceModel::addturbulence ModelConstructorToTable<turbulenceModelType>::Newt urbulenceModel(const Foam::volScalarField&, const Foam::volVectorField&, const Foam::surfaceScalarField&, int)’:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: ‘thermoPhysicalModel’ was not declared in this scope
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In member function ‘const Foam::volScalarField& Foam::compressible::turbulenceModel::mu() const’:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:180: error: ‘thermophysicalModel_’ was not declared in this scope
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In member function ‘const Foam::volScalarField& Foam::compressible::turbulenceModel::alpha() const’:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:186: error: ‘thermophysicalModel_’ was not declared in this scope
In file included from rhoPorousSimpleFoam_poly.C:36:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H: At global scope:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:163: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:164: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:175: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:176: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H: In static member function ‘static Foam::autoPtr<Foam::compressible::RASModel> Foam::compressible::RASModel::adddictionaryConstru ctorToTable<RASModelType>::New(const Foam::volScalarField&, const Foam::volVectorField&, const Foam::surfaceScalarField&, int)’:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: ‘thermoPhysicalModel’ was not declared in this scope
In file included from rhoPorousSimpleFoam_poly.C:46:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:3: error: ‘basicPsiThermo’ was not declared in this scope
createFields.H:3: error: template argument 1 is invalid
createFields.H:4: error: invalid type in declaration before ‘(’ token
createFields.H:5: error: ‘basicPsiThermo’ is not a class or namespace
createFields.H:7: error: ‘thermo’ was not declared in this scope
createFields.H:7: error: ‘pThermo’ cannot be used as a function
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readSIMPLEControls.H:6: warning: unused variable ‘momentumPredictor’
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readSIMPLEControls.H:9: warning: unused variable ‘fluxGradp’
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readSIMPLEControls.H:12: warning: unused variable ‘transonic’
make: *** [Make/linux64GccDPOpt/rhoPorousSimpleFoam_poly.o] Error 1

[herbert]

Hi Chrisi,

I'm really sorry, but there was still something missing in my first post. I have updated the code for makeBasicPsiThermo.H.

The "path to your lnInclude" should be replaced by the absolute patch to basic/lnInclude. If you followed my suggestion it should look like

-I$(WM_PROJECT_USER_DIR)/lib/thermophysicalModels/basic/lnInclude

Hope it will work now
Stefan

[Chrisi1984]

Hi,

Sorry its me again.

At first thank you again.

The model compiles perfect now.

I can still not compile my solvers with the new model.

This is my error:

/cfd/externe-ma/Alt/applications/solvers/compressible/rhoPorousSimpleFoam_1 >wclean
/cfd/externe-ma/Alt/applications/solvers/compressible/rhoPorousSimpleFoam_1 >wmake
Making dependency list for source file rhoPorousSimpleFoam_1.C
could not open file basicPsiThermo.H for source file rhoPorousSimpleFoam_1.C
could not open file basicThermo.H for source file rhoPorousSimpleFoam_1.C
SOURCE=rhoPorousSimpleFoam_1.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/home/user/e18980/OpenFOAM/e18980-1.6/lib/thermophysicalModels/basic/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/cfdTools -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/meshTools/lnInclude -IlnInclude -I. -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/rhoPorousSimpleFoam_1.o
rhoPorousSimpleFoam_1.C:35:28: error: basicPsiThermo.H: No such file or directory
In file included from /cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:48,
from rhoPorousSimpleFoam_1.C:36:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:52:25: error: basicThermo.H: No such file or directory
In file included from /cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:48,
from rhoPorousSimpleFoam_1.C:36:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:85: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:85: error: expected ‘;’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:130: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:131: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:142: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:143: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:172: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:172: error: expected ‘;’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:178: error: expected `;' before ‘const’
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In static member function ‘static Foam::autoPtr<Foam::compressible::turbulenceModel> Foam::compressible::turbulenceModel::addturbulence ModelConstructorToTable<turbulenceModelType>::Newt urbulenceModel(const Foam::volScalarField&, const Foam::volVectorField&, const Foam::surfaceScalarField&, int)’:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:107: error: ‘thermoPhysicalModel’ was not declared in this scope
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In member function ‘const Foam::volScalarField& Foam::compressible::turbulenceModel::mu() const’:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:180: error: ‘thermophysicalModel_’ was not declared in this scope
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In member function ‘const Foam::volScalarField& Foam::compressible::turbulenceModel::alpha() const’:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:186: error: ‘thermophysicalModel_’ was not declared in this scope
In file included from rhoPorousSimpleFoam_1.C:36:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H: At global scope:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:163: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:164: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:175: error: expected ‘,’ or ‘...’ before ‘&’ token
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:176: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H: In static member function ‘static Foam::autoPtr<Foam::compressible::RASModel> Foam::compressible::RASModel::adddictionaryConstru ctorToTable<RASModelType>::New(const Foam::volScalarField&, const Foam::volVectorField&, const Foam::surfaceScalarField&, int)’:
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:139: error: ‘thermoPhysicalModel’ was not declared in this scope
In file included from rhoPorousSimpleFoam_1.C:46:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:3: error: ‘basicPsiThermo’ was not declared in this scope
createFields.H:3: error: template argument 1 is invalid
createFields.H:4: error: invalid type in declaration before ‘(’ token
createFields.H:5: error: ‘basicPsiThermo’ is not a class or namespace
createFields.H:7: error: ‘thermo’ was not declared in this scope
createFields.H:7: error: ‘pThermo’ cannot be used as a function
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readSIMPLEControls.H:6: warning: unused variable ‘momentumPredictor’
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readSIMPLEControls.H:9: warning: unused variable ‘fluxGradp’
/cfd/CFD/PROGRAMME/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readSIMPLEControls.H:12: warning: unused variable ‘transonic’
make: *** [Make/linux64GccDPOpt/rhoPorousSimpleFoam_1.o] Error 1

Perhabs I mad a mistake in /make/options in the solver folder. This is my options file:

EXE_INC = \
-I$(WM_PROJECT_USER_DIR)/lib/thermophysicalModels/basic/lnInclude \
-I$(LIB_SRC)/turbulenceModels \
-I$(LIB_SRC)/turbulenceModels/compressible/RAS/RASModel \
-I$(LIB_SRC)/finiteVolume/cfdTools \
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
$(FOAM_USER_LIBBIN)/libuserBasicThermophysicalModels.so \
-lspecie \
-lcompressibleRASModels \
-lfiniteVolume \
-lmeshTools

For the thermophysical models a made exactly the procedure like you described with your new additionals.

Can you see a mistake in my options-file?

Regards Chrisi

[herbert]

Hi Chrisi,

it seems that the error lies here:

-I$(WM_PROJECT_USER_DIR)/lib/thermophysicalModels/basic/lnInclude \

because the compiler reports that it couldn't find the source files of thermophysicalModels (error report "could not open ..."). It's hard for me to tell you what exactly you have to type there, but you need to give in the path of your new source files there, so the compiler can read them. For explanation: -I$(WM_PROJECT_USER_DIR) points to your personal folder (e.g. chrisi-1.6/) and starting from there please give in the path to your new source files (or better to their links in basic/lnInclude).

Regards,
Stefan

[Chrisi1984]

Hi Herbert,

thanks.

Now I compiled my solver succesfully. But I get the same error like Sebastian when I try to run the solver. I took exactly your thermophysical properties.

Any ideas?

Best regards

Chrisi

[Chrisi1984]

Hi Herbert,

thanks.

Now I compiled my solver succesfully. But I get the same error like Sebastian when I try to run the solver.

Create mesh for time = 0

Reading thermophysical properties

Selecting thermodynamics package hPsiThermo<pureMixture<polynomialTransport3<specie Thermo<hPolynomialThermo4<perfectGas>>>>>


Unknown basicPsiThermo type hPsiThermo<pureMixture<polynomialTransport3<specie Thermo<hPolynomialThermo4<perfectGas>>>>>

Valid basicPsiThermo types are:

8
(
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<eConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
)



From function basicPsiThermo::New(const fvMesh&)
in file psiThermo/basicPsiThermo/newBasicPsiThermo.C at line 64.

FOAM exiting

I took exactly your thermophysical properties.

Any ideas?

Best regards



Chrisi

[herbert]

Dear Chrisi,

now I'm totally confused! That means the new model-combinations are not defined and the changes are completely ignored. I have to think about, but I don't think I missed something such elementary in my description! Please have a look on each single step again.

Regards,
Stefan

[Chrisi1984]

Hi,

I am sorry I made a mistake!!!

Now the solver with the new model is running!!

Thank you so much!

I will keep you up to date about the results!

Best regards

Chrisi

[Chrisi1984]

Hi,

like promised I want to give an update.

Everything seems to work very well with your new themphysical models.

Thank you once again!!

Best regards
Chrisi