CFD Online Discussion Forums - polynomial thermophysical properties II

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - polynomial thermophysical properties II (https://www.cfd-online.com/Forums/openfoam-solving/77270-polynomial-thermophysical-properties-ii.html)

Hi!

Sorry I did not find time yet to work further on it.

But as soon I will have results ill let you know!

Thanks again Stefan!

Best wishes,
Sebastian

Hello Stefan (or anyone who knows about Open Foam ;))!

The Code is still not working..
The only thing I changed compared to your case is, that I use sutherland transport and no polynomial transport. Still gives me back the following error message:

Quote:

Reading thermophysical properties

ill defined primitiveEntry starting at keyword 'mixture' on line 23 and ending at line 34

file: /home32/sebastian/OpenFOAM/sebastian-1.6/run_rhoSimpleThermo/constant/thermophysicalProperties at line 34.

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

FOAM exiting

Would you mind to have a look on my changes in the code. :-)

Change in hPsiThermos.C:

Quote:

#include "hPolynomialThermo.H"

makeBasicPsiPolyThermo
(
hPsiThermo,
pureMixture,
sutherlandTransport,
hPolynomialThermo,
4,
perfectGas
);

Change in makeBasicPsiThermo.H:

Quote:

#ifndef makeBasicPsiPolyThermo_H
#define makeBasicPsiPolyThermo_H

#define makeBasicPsiPolyThermo(Cthermo,Mixture,Transport,T hermo,orderThermo,EqnOfState) \
\
typedef Cthermo<Mixture<Transport<specieThermo<Thermo<EqnO fState,orderThermo> > > > > \
Cthermo##Mixture##Transport##Thermo##orderThermo## EqnOfState; \
\
defineTemplateTypeNameAndDebugWithName \
( \
Cthermo##Mixture##Transport##Thermo##orderThermo## EqnOfState, \
#Cthermo \
"<"#Mixture"<"#Transport"<specieThermo<"#Thermo#or derThermo"<"#EqnOfState">>>>>", \
0 \
); \
\
addToRunTimeSelectionTable \
( \
basicPsiThermo, \
Cthermo##Mixture##Transport##Thermo##orderThermo## EqnOfState, \
fvMesh \
)

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

Change in basicMixtures.C

Quote:

#include "hPolynomialThermo.H"

makeBasicPolyMixture
(
pureMixture,
sutherlandTransport,
hPolynomialThermo,
4,
perfectGas
);

Change in makeBasicMixture.H

Quote:

#ifndef makeBasicPsiPolyThermo_H
#define makeBasicPsiPolyThermo_H

#define makeBasicPolyMixture(Mixture,Transport,Thermo,orde rThermo,EqnOfState) \
\
typedef Mixture<Transport<specieThermo<Thermo<EqnOfState,o rderThermo> > > > \
Mixture##Transport##Thermo##orderThermo##EqnOfStat e; \
\
defineTemplateTypeNameAndDebugWithName \
(Mixture##Transport##Thermo##orderThermo##EqnOfSta te, \
#Mixture"<"#Transport"<specieThermo<"#Thermo#order Thermo"<"#EqnOfState">>>>", 0)

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

And thats my thermophysicalProperties file

Quote:

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

//mixture air 1 28.9 1000 0 1 1;

mixture //keyword
air 1 28.9 //specie bzw specieCoeffs
//1007 0 //hConstThermo bzw thermoCoeffs
0.0 //standard formation enthalpy [J/kg]
0.0 //standard formation entropy [J/kg]
cpPolynomial(1035.887 -0.255611 0.0006258047 -2.627558e-07)//hPolynomialThermo bzw. thermoCoeffs
1.458e-05 110.4; //sutherlandTransport bzw. transportCoeffs
//1.8e-05 0.7; //constTransport

Sorry for the formatting. Really hope you can help me.
Everything compiles well. Maybe hPolynomialThermo does not work in combination with sutherland??

Thanks a lot in advance!

Best wishes,
Sebastian

Hi Sebastian,

due to the error message you get it seems that the model is known. Therefore the problem is inside the definition of your coeffs. I think there should be a space between "cpPolynomial" and its defintion.

Code:

cpPolynomial (1035.887 -0.255611 0.0006258047 -2.627558e-07)

Please give a try.

Regards,
Stefan

Hi Stefan,

indeed!! Now it works! :)

Thanks a lot!!!!

Sorry, another question about your code, Stefan:

in the makeBasicMixture.H, you included

#ifndef makeBasicPsiPolyThermo_H
#define makeBasicPsiPolyThermo_H

shouldn't that be

#ifndef makeBasicPsiPolyMixture_H
#define makeBasicPsiPolyMixture_H

Maybe I am wrong. I tried both, and in every case it compiles and the code runs..

Regards,
Sebastian

Yes you are right. It should be

Code:

#ifndef makeBasicPolyMixture_H

#define makeBasicPolyMixture_H

However .... ;)

hpolynomial for hRhoThermo

Hallo!

Thank you for your posts. It was very helpfully for me.

Is it possible to implement the temperaturdependency for the buoyantPimpleFoam because it is using the hRhoThermo instead of the hPsiThermo which is used in the description.

I tried it in the same way as described above but it does not solve the pressure equation in my case.

I hope you can help me!

Thx

br

Franz

Dear Stefan, Sebastian and Chrisi,

First of all thank you so much for this post, the user guide was of very little help with this issue. I followed every step that herbert had posted and was able to compile both the libuserThermophysicalModels.so and got my solver to compile with the new library.

However when I run my case, here the error that I get.

atareen@ubuntu:~/OpenFOAM/atareen-1.7.1/run/venturiTransport$ ammarSonicFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.x |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.7.x-4bbf33160caf
Exec : ammarSonicFoam
Date : Feb 10 2011
Time : 14:31:35
Host : ubuntu
PID : 8072
Case : /home/atareen/OpenFOAM/atareen-1.7.1/run/venturiTransport
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading thermophysical properties

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

--> FOAM FATAL ERROR:
Not implemented

From function basicThermo::e()
in file basicThermo/basicThermo.C at line 354.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::basicThermo::e() in "/home/atareen/OpenFOAM/atareen-1.7.1/lib/linuxGccDPOpt/libuserBasicThermophysicalModels.so"
#3
in "/home/atareen/OpenFOAM/atareen-1.7.1/applications/bin/linuxGccDPOpt/ammarSonicFoam"
#4 __libc_start_main in "/lib/libc.so.6"
#5
in "/home/atareen/OpenFOAM/atareen-1.7.1/applications/bin/linuxGccDPOpt/ammarSonicFoam"
Aborted

I don't know how to fix this error? can somebody please help me?

Warm regards,
Ammar.

Hi Ammar,

For sonicFoam it should be ePsiThermo instead of hPsiThermo in thermophysicalProperties. hPsiThermo<pureMiyture...

Regards,
Huong

Quote:

Originally Posted by fattychickenrun (Post 297479)

Hi Ammar,

For sonicFoam it should be ePsiThermo instead of hPsiThermo in thermophysicalProperties. hPsiThermo<pureMiyture...

Regards,
Huong

Dear Huong,

Thank you. I noticed that too. I should've updated this thread. Thanks for replying.

Sincerely,
Ammar.

All the heat transfer solvers in OpenFOAM besides the Bousinessq ones are defined for gases . Is there a solver for fluids too ? What i want to do is vary cp and mu according to a polynomial and use buoyantPimpleFoam for fluids . How do i go about doing this ?

http://www.openfoam.com/features/standard-solvers.php

buoyantPimpleFoam is a solver for fluids.

Have you followed the instructions posted earlier in this thread to make polynomial forms of cp and mu? I think the process is the same, you'll just have to modify the .C and .H files in buoyantPimpleFoam and some files in the thermoPhysicalModels folder located in /opt/openfoam-ver/src.

Try the instructions, once you're a little comfortable with modifying files and using wmake, you'll be creating your own solvers in no time. Post again if it doesn't work.

Ammar.

Hi Ammar ,
Thanks for the response

All the solvers define enthalpy as
volScalarField& h = thermo.h() ;

thermo is defined in thermophysical properties as :
Valid basicRhoThermo types are:

6
(
hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<constTransport<specieTherm o<hConstThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<hConstThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<janafThermo<perfectGas>>>>>
)

OR

11
(
ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<eConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<constTransport<specieTherm o<hConstThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<sutherlandTransport<specie Thermo<hConstThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<sutherlandTransport<specie Thermo<janafThermo<perfectGas>>>>>
)

What is the term perfectGas doing in a solver for general fluids ? That was the reason i thought that buoyantPimpleFoam is not for fluids .

Kindly correct me if I am wrong

I think the layers modifications on top of perfectGas will define your fluid.
Although you have a good point, this could be a poor way of labeling things or may be I missed something too. However I know that for a liquid you will have to replace <perfectGas> by <icoPolynomial>. So you do in fact wanna keep perfect gas in there: that just means that the intermolecluar forces of your fluid are negligible. I think can you separately define chemical interactions between particles of fluid in you have such interactions.

Please look at the following if you haven't already, will help you find definitions:

http://www.openfoam.com/docs/user/thermophysical.php

Also, I am only working with mixtures of gases and thermoPhysical properties for liquids might be defined differently. If you're working with gases, than this should be fine. If you want to implement liquids than may be look at some of the liquid tutorials e.g. sonicLiquidFoam?

Sorry if this doesn't help much.

Ammar.

polynomial thermophysical properties

Hi All,

I have followed the procedure mentioned in the thread but could not succeed in compiling the code. i am bit new to OpenFoam and not sure where i made mistake.

Can somebody has a consolidated procedure to help me with implementing Polynomial thermo physical properties

error during polynomial thermophysical properties

Hi All,

When i modified the code based on the thread mentioned. i am receiving the following error.
Please help me what was the mistake in my code. i am bit new to OpenFoam.

wmakeLnInclude: linking include files to ./lnInclude
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/basicPsiThermoNew.C
Making dependency list for source file psiThermo/hPsiThermo/hPsiThermos.C
Making dependency list for source file psiThermo/hsPsiThermo/hsPsiThermos.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/basicRhoThermoNew.C
Making dependency list for source file rhoThermo/hRhoThermo/hRhoThermos.C
Making dependency list for source file rhoThermo/hsRhoThermo/hsRhoThermos.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 -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam200/src/finiteVolume/lnInclude -I/opt/openfoam200/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/opt/openfoam200/src/OpenFOAM/lnInclude -I/opt/openfoam200/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/basicMixture.o
SOURCE=mixtures/basicMixture/basicMixtures.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam200/src/finiteVolume/lnInclude -I/opt/openfoam200/src/thermophysicalModels/specie/lnInclude -IlnInclude -I. -I/opt/openfoam200/src/OpenFOAM/lnInclude -I/opt/openfoam200/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/basicMixtures.o
In file included from mixtures/basicMixture/basicMixtures.C:32:
mixtures/basicMixture/makeBasicMixture.H:82:1: warning: "makeBasicPolyMixture" redefined
mixtures/basicMixture/makeBasicMixture.H:48:1: warning: this is the location of the previous definition
mixtures/basicMixture/basicMixtures.C:117:1: error: macro "makeBasicPolyMixture" requires 5 arguments, but only 2 given
mixtures/basicMixture/basicMixtures.C:123:1: error: macro "makeBasicPolyMixture" requires 5 arguments, but only 2 given
mixtures/basicMixture/basicMixtures.C:117: error: expected constructor, destructor, or type conversion before ‘;’ token
mixtures/basicMixture/basicMixtures.C:123: error: expected constructor, destructor, or type conversion before ‘;’ token
make: *** [Make/linux64GccDPOpt/basicMixtures.o] Error 1

Please anyone who are successful in implementing the polynomial properties can help me
Regards
Krishna

Dear Krishna,

look at the last few lines of your error:

mixtures/basicMixture/basicMixtures.C:117:1: error: macro "makeBasicPolyMixture" requires 5 arguments, but only 2 given
mixtures/basicMixture/basicMixtures.C:123:1: error: macro "makeBasicPolyMixture" requires 5 arguments, but only 2 given

You could've missed adding the right number of coefficients for your polynomial: e.g. A very basic mistake you could've made is that you could've defined your thermophysicalProperties file to take a fifth order polynomial instead of two. But this is just a guess.

So check the files you've made the changes in ( I think there are only 3 or 4 files in which you make these changes) and make sure that the number of arguments are consistent everywhere.

Post again with the changes if you're still having trouble.

Best,
Ammar.

error: polynomial thermophysical properties

Dear Ammar,
Please find below the details of my basicMixtures.C
makeBasicPolyMixture
(
pureMixture,
sutherlandTransport,
hPolynomialThermo,
4,
perfectGas
);
and makeBasicMixture.H file consists of following code.
At the bottom i have added the required definition for polynomial thermophysical properties.

Please help me where i went wrong

Regards
Krishna

#ifndef makeBasicMixture_H
#define makeBasicMixture_H

#include "basicMixture.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#define makeBasicMixture(Mixture,Transport,Thermo,EqnOfSta te) \
\
typedef Mixture<Transport<specieThermo<Thermo<EqnOfState> > > > \
Mixture##Transport##Thermo##EqnOfState; \
\
defineTemplateTypeNameAndDebugWithName \
(Mixture##Transport##Thermo##EqnOfState, \
#Mixture"<"#Transport"<specieThermo<"#Thermo"<"#Eq nOfState">>>>", 0)

#define makeBasicPolyMixture(Mixture,Order) \
\
typedef polynomialTransport \
< \
specieThermo \
< \
hPolynomialThermo \
< \
icoPolynomial<Order>, \
Order \
> \
>, \
Order \
> icoPoly##Order##ThermoPhysics; \
\
typedef Mixture<icoPoly##Order##ThermoPhysics> \
Mixture##icoPoly##Order##ThermoPhysics; \
\
defineTemplateTypeNameAndDebugWithName \
(Mixture##icoPoly##Order##ThermoPhysics, \
#Mixture"<icoPoly"#Order"ThermoPhysics>", 0)

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

#ifndef makeBasicPsiPolyMixture_H
#define makeBasicPsiPolyMixture_H

#include "basicMixture.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#define makeBasicPolyMixture(Mixture,Transport,Thermo,orde rThermo,EqnOfState) \
\
typedef Mixture<Transport<specieThermo<Thermo<EqnOfState,o rderThermo> > > > \
Mixture##Transport##Thermo##orderThermo##EqnOfStat e; \
\
defineTemplateTypeNameAndDebugWithName \
( \
Mixture##Transport##Thermo##orderThermo##EqnOfStat e, \
#Mixture"<"#TransportmakeBasic"<specieThermo<"#The rmo#orderThermo"<"#EqnOfState">>>>", \
0 \
);

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

error: polynomial thermophysical properties

Dear Ammar,

I was able to solve the problem and there is some syntax error in the last line and specified 3 coefficients for polynomial.

Now i have another problem while compiling the applications/solvers/compressible/rhoSimpleFoam/rhoPorousMRFSimpleFoam.
In Make directory i modified the options file as shown below

can you please help me where i went wrong.

Regards
Krishna

file: options
EXE_INC = \
-I.. \
-I$(WM_PROJECT_USER_DIR)/lib/thermophysicalModels/basic/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/thermalPorousZone/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 = \
$(FOAM_USER_LIBBIN)/libuserBasicThermophysicalModels.so\
-lthermalPorousZone \
-EXE_INC = \
-I.. \
-I$(WM_PROJECT_USER_DIR)/lib/thermophysicalModels/basic/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/thermalPorousZone/lnInclude \
-I$(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

Error:

root@santhosh-desktop:/opt/openfoam200/applications/solvers/compressible/rhoSimpleFoam/rhoPorousMRFSimpleFoam# wmake
SOURCE=rhoPorousMRFSimpleFoam.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I.. -I/home/santhosh/OpenFOAM/root-2.0.0/lib/thermophysicalModels/basic/lnInclude -I/opt/openfoam200/src/thermophysicalModels/thermalPorousZone/lnInclude -I/opt/openfoam200/src/turbulenceModels -I/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel -I/opt/openfoam200/src/finiteVolume/cfdTools -I/opt/openfoam200/src/finiteVolume/lnInclude -I/opt/openfoam200/src/meshTools/lnInclude -IlnInclude -I. -I/opt/openfoam200/src/OpenFOAM/lnInclude -I/opt/openfoam200/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/rhoPorousMRFSimpleFoam.o
rhoPorousMRFSimpleFoam.C:35:28: error: basicPsiThermo.H: No such file or directory
In file included from /opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:46,
from rhoPorousMRFSimpleFoam.C:36:
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:51:25: error: basicThermo.H: No such file or directory
In file included from /opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:46,
from rhoPorousMRFSimpleFoam.C:36:
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:86: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:86: error: expected ‘;’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:132: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:132: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:145: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:145: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:176: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:176: error: expected ‘;’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:182: error: expected ‘;’ before ‘const’
/opt/openfoam200/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)’:
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: ‘thermoPhysicalModel’ was not declared in this scope
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: ‘turbulenceModelName’ was not declared in this scope
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In static member function ‘static Foam::autoPtr<Foam::compressible::turbulenceModel> Foam::compressible::turbulenceModel::addRemovablet urbulenceModelConstructorToTable<turbulenceModelTy pe>::NewturbulenceModel(const Foam::volScalarField&, const Foam::volVectorField&, const Foam::surfaceScalarField&, int)’:
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: ‘thermoPhysicalModel’ was not declared in this scope
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:108: error: ‘turbulenceModelName’ was not declared in this scope
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In member function ‘const Foam::volScalarField& Foam::compressible::turbulenceModel::mu() const’:
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:184: error: ‘thermophysicalModel_’ was not declared in this scope
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H: In member function ‘const Foam::volScalarField& Foam::compressible::turbulenceModel::alpha() const’:
/opt/openfoam200/src/turbulenceModels/compressible/turbulenceModel/turbulenceModel.H:190: error: ‘thermophysicalModel_’ was not declared in this scope
In file included from rhoPorousMRFSimpleFoam.C:36:
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H: At global scope:
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:153: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:153: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:166: error: ISO C++ forbids declaration of ‘basicThermo’ with no type
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:166: error: expected ‘,’ or ‘...’ before ‘&’ token
/opt/openfoam200/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)’:
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: ‘thermoPhysicalModel’ was not declared in this scope
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: ‘turbulenceModelName’ was not declared in this scope
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H: In static member function ‘static Foam::autoPtr<Foam::compressible::RASModel> Foam::compressible::RASModel::addRemovabledictiona ryConstructorToTable<RASModelType>::New(const Foam::volScalarField&, const Foam::volVectorField&, const Foam::surfaceScalarField&, int)’:
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: ‘thermoPhysicalModel’ was not declared in this scope
/opt/openfoam200/src/turbulenceModels/compressible/RAS/RASModel/RASModel.H:128: error: ‘turbulenceModelName’ was not declared in this scope
In file included from rhoPorousMRFSimpleFoam.C:48:
../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
make: *** [Make/linux64GccDPOpt/rhoPorousMRFSimpleFoam.o] Error 1

error: polynomial thermophysical properties

Dear Ammar,

My options file is as shown below

EXE_INC = \
-I.. \
-I$(WM_PROJECT_USER_DIR)/lib/thermophysicalModels/basic/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/thermalPorousZone/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\
-lthermalPorousZone \
-lspecie \
-lcompressibleTurbulenceModel \
-lcompressibleRASModels \
-lfiniteVolume \
-lmeshTools

Regards
Krishna