# Entropy calculation in OpenFoam

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 23, 2013, 08:37 Entropy calculation in OpenFoam #1 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 I have found a figure of entropy in this article that has made by OpenFOAM: Code: `http://www.cimec.org.ar/ojs/index.ph...view/4231/4157` I'm wondering if does OF calculates entropy?which solvers does have it?I couldn't find a useful thread about this subject in the forum. that can improve my work and the conclusions. can anyone guide me through? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 April 23, 2013, 21:08 #2 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 hi all again does anyone know an example for adding entropy equation to any of the compressible (or even other) solvers? It this work possible with a rational effort?or is too complicated? Has anyone think about this subject (seeing entropy values) so far? I thank any of thoughts __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 April 24, 2013, 12:48 #3 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 no any opinion about entropy in OpenFOAM? does have a solver calculate entropy? any hint? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 April 25, 2013, 02:09 #4 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 no one is interested? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 April 26, 2013, 22:25 #5 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 how i can't find anything useful in the forum search related to this subject? Means no one has ever thought about?!! __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 April 29, 2013, 18:56 #6 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 8,301 Blog Entries: 34 Rep Power: 84 Hi Ehsan, According to the paper you've indicated, it seems that the solver "rhoCentralFoam" was used to calculate entropy. I've searched OpenFOAM's source code with the following command: Code: `find \$FOAM_SRC -name "*.[CH]" | xargs grep -isl 'Entropy'` It will look in the "\$FOAM_SRC" folder, look for files with extension "C" or "H" and indicate which files have the text "Entropy" in them. For more on this: cellSet: command not found - post #8 The same could be done with the text editor "Kate", which can find text inside files on a particular folder. The files that were found were: Code: ```./thermophysicalModels/reactionThermo/mixtures/SpecieMixture/SpecieMixture.H ./thermophysicalModels/reactionThermo/mixtures/basicMultiComponentMixture/basicMultiComponentMixture.H ./thermophysicalModels/specie/thermo/eConst/eConstThermo.H ./thermophysicalModels/specie/thermo/hPolynomial/hPolynomialThermo.C ./thermophysicalModels/specie/thermo/hPolynomial/hPolynomialThermo.H ./thermophysicalModels/specie/thermo/thermo/thermo.H ./thermophysicalModels/specie/thermo/hConst/hConstThermo.H ./thermophysicalModels/specie/thermo/janaf/janafThermo.H ./thermophysicalModels/specie/thermo/hExponential/hExponentialThermo.H``` From what I can see, you can easily adapt the utility that calculates "Cp" to calculate "S", namely: how can see Cp values? As for not find much information on this topic: it's OpenFOAM. It's only natural that there are several undocumented or poorly documented details about OpenFOAM's features. But the great thing about OpenFOAM is that the source code is completely open for anyone to look at it and study it Best regards, Bruno CFDUser_ likes this. __________________ OpenFOAM: Frequently Asked Questions | Useful links for building and using Forum: How to ask for help | Posting code and output with [CODE] My to-do list and when I'll be able to come to the forum: http://wyldckat.github.io And please: Read this before sending private messages to me

 April 30, 2013, 06:52 #7 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 thanks so much. then entropy is calculated but not is shown.could simply change this behavior?(I have tested simple things like MUST_WRITE without success) will specificHeat.C work by changing only Cp to s or how? -------------------------- hi again I made little changes like this: Code: ```int main(int argc, char *argv[]) { timeSelector::addOptions(); # include "setRootCase.H" # include "createTime.H" instantList timeDirs = timeSelector::select0(runTime, args); # include "createMesh.H" forAll(timeDirs, timeI) { runTime.setTime(timeDirs[timeI], timeI); Info<< "Time = " << runTime.timeName() << endl; mesh.readUpdate(); Info<< "Re-reading thermophysical properties\n" << endl; autoPtr pThermo ( psiThermo::New(mesh) ); psiThermo& thermo = pThermo(); thermo.validate(args.executable(), "s"); Info<< " Calculating entropy" << endl; volScalarField s ( IOobject ( "s", runTime.timeName(), mesh, IOobject::NO_READ ), thermo.s() ); s.write(); Info<< endl; } Info<< nl << "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; Info<< "End\n" << endl; return 0; }``` but the error is: Code: ```SOURCE=entropy.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam220/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam220/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam220/src/OpenFOAM/lnInclude -I/opt/openfoam220/src/OSspecific/POSIX/lnInclude -fPIC -c \$SOURCE -o Make/linux64GccDPOpt/entropy.o entropy.C: In function ‘int main(int, char**)’: entropy.C:70:20: error: ‘class Foam::psiThermo’ has no member named ‘s’ make: *** [Make/linux64GccDPOpt/entropy.o] Error 1``` why psiThermo doesn't know s? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. Last edited by immortality; April 30, 2013 at 08:22.

April 30, 2013, 17:45
#8
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
Quote:
 Originally Posted by immortality why psiThermo doesn't know s?

I wrote "S", not "s"!
Quote:
 Originally Posted by wyldckat you can easily adapt the utility that calculates "Cp" to calculate "S"

Last edited by wyldckat; April 30, 2013 at 17:47. Reason: rearranged the answer and added the now 1st quote

 May 1, 2013, 03:51 #9 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 in the solver its s.I changed s to S but erroe is same: Code: ```Making dependency list for source file entropy.C SOURCE=entropy.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam220/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam220/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam220/src/OpenFOAM/lnInclude -I/opt/openfoam220/src/OSspecific/POSIX/lnInclude -fPIC -c \$SOURCE -o Make/linux64GccDPOpt/entropy.o entropy.C: In function ‘int main(int, char**)’: entropy.C:70:20: error: ‘class Foam::psiThermo’ has no member named ‘S’ make: *** [Make/linux64GccDPOpt/entropy.o] Error 1``` please have a look into it yourself ! __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 May 1, 2013, 08:21 #10 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 8,301 Blog Entries: 34 Rep Power: 84 Hi Ehsan, I didn't test it myself before... and I was assuming that if there was a "Cp", there should be an "S" as well... but apparently it doesn't exist yet! Looks like the OpenFOAM authors never needed a complete entropy field. And this isn't very simple to solve either. Here's the situation: The "S" method I saw is present in the "species" class, which means that it calculates only for a single value, not all values in a field. Problem is that the "species" information is deeply embedded into the thermodynamics mechanism that OpenFOAM uses. So the simplest solution would be to add a new method "S", which was copied-pasted-changed from the "Cp" method that is present in "heThermo": https://github.com/OpenFOAM/OpenFOAM...asic/heThermo/ edit: In other words, copy the methods named "Cp" to "S" inside the class "heThermo". The same would have to be done to the "basicThermo" class. Then rebuild "src/thermophysicalModels/basic" library. This may seem simple, but a lot more changes might be necessary for this to actually properly work. Worst thing is that this requires changing the core source code in OpenFOAM, which I don't know if you want to do this, since this would add even more complexity to your thesis, just because you need to calculate the entropy. I'm going to look a bit more into this, because I think I overlooked something... but I don't know when I might find a better answer for this. Best regards, Bruno immortality likes this. __________________ OpenFOAM: Frequently Asked Questions | Useful links for building and using Forum: How to ask for help | Posting code and output with [CODE] My to-do list and when I'll be able to come to the forum: http://wyldckat.github.io And please: Read this before sending private messages to me Last edited by wyldckat; May 1, 2013 at 08:23. Reason: see "edit:"

May 1, 2013, 15:35
#11
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
Hi Ehsan,

I think you can consider yourself very lucky today! I've managed to figure out a solution without having to hack directly into OpenFOAM's source code!
It took some C++ voodoo (mostly tricks with templates and macros), but it works!

The only downside is that you have to modify the source code every time you change "thermoType" in "constant/thermophysicalProperties".
This is exemplified in the comment section in "entropy.C" that starts with:
Code:
```/*
For reference:

makeTheLenghtyTypedefName(```
The code that will need changing is this block:
Code:
```//Define here the components of the thermodynamic class
#define myLengthyThermoClass makeTheLenghtyTypedefName( \
psiThermo, \
hePsiThermo, \
pureMixture, \
sutherlandTransport, \
sensibleEnthalpy, \
janafThermo, \
perfectGas, \
specie \
)```
The final application is named entropy. To build it, simply run:
Code:
`wmake`
Note about OpenFOAM 2.2.0: See post #17
______________________

Now, explain what I had to do:
1. Read the following post for an introduction into this topic: NoRepository - post #12
2. I had to create a header file that locally replaces "makeThermo.H". You can see it inside the attached file.
3. Then include both this header file and the file "psiThermos.C", which is originally used to create all of the "psiThermo" models, but with our local "makeThermo.H" file, we recreate the typedefs.
4. This way we now have access to all of the basic "psiThermo" models, as shown here: https://github.com/OpenFOAM/OpenFOAM...o/psiThermos.C
5. Now, since the naming scheme is quite cumbersome, I added a local definition that helps concatenate the typedef on the demand, namely with the following macros:
• "makeTheLenghtyTypedefName" - this macro helps concatenate the local typedef we will be using.
• "myLengthyThermoClass" - this is an alias for the local typedef we will be using.
6. So instead of creating an "autoptr<psiThermo>" as it is usually done in solvers and utilities, we now use the "myLengthyThermoClass" alias and use it directly to instantiate the "thermo" variable.
7. This way, we have access to stuff that isn't accessible from "psiThermo", more specifically we can access the "pureMixture" class, which gives us access to all of the species, janaf/thermo and gas properties that we usually don't have access to!
8. Then, since we need to calculate the entropy "S" for all of the volume cells and patch faces, I copy-paste-adapted the contents of the method "Cp()" from "src/thermophysicalModels/basic/heThermo/heThermo.C", directly into the main application source code file "entropy.C".
And that's all there is to it!

There's going to be some more people interested in this, because this gives access to the methods for the currently loaded thermodynamic sub-models!

Best regards,
Bruno
Attached Files
 entropyHePsi_2.2.tar.gz (2.5 KB, 30 views)

Last edited by wyldckat; May 2, 2013 at 10:02. Reason: added "Note about OpenFOAM 2.2.0"

 May 1, 2013, 15:41 #12 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 then s is only there and they never have used it? so there is a lot of work to do with it.could find the equation that entropy calculated from that? if it can be done is very nice.but if is so complicated never mind! ---------------------- your post received after mine! really it works?I don't believe it! its second chance i get today.except for this I figured out an issue i was engaged with for months!what a nice day! surprising.I'll test it soon. i think this thread of mine was a brilliant one and so valuable like those effective questions you had told me about before! the second one is how can see Cp values? and third prize with a small distance belongs to: how to calculate mass flow rate on patches and summation of that during the run? but no prize I have awarded yet! I'm happy that it can help others. thank you very much. (what a post with a lot of big grin icon) __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. Last edited by immortality; May 1, 2013 at 16:09.

May 1, 2013, 15:49
#13
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
Quote:
 Originally Posted by immortality then s is only there and they never have used it?
"S" probably is used internally, but doesn't seem to be used for external consumption, such as generating the complete "S" field.

Quote:
 Originally Posted by immortality could find the equation that entropy calculated from that?
I don't understand the question... do you mean:
1. Is it possible to find out how "S" is actually calculated?
2. (Or) Is is possible to find what "S" is being used for internally in OpenFOAM?

 May 1, 2013, 16:12 #14 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 I edited the before post. I think 1 is more near to my intention. what does 2 mean? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

May 1, 2013, 16:37
#15
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
Quote:
 Originally Posted by wyldckat 1. Is it possible to find out how "S" is actually calculated?[/LIST]
Let's see...
Quote:
 https://github.com/OpenFOAM/OpenFOAM...thermoI.H#L252 Code: ```template class Type> inline Foam::scalar Foam::species::thermo::S(const scalar p, const scalar T) const { return this->s(p, T)/this->W(); }```
So, it's calculated from the molar entropy, divided by the molecular weight.

The molar entropy is calculated depending on the equation of state. For example, in "janaf" it's calculated in this method:
Quote:
 https://github.com/OpenFOAM/OpenFOAM...ThermoI.H#L213 Code: ```template inline Foam::scalar Foam::janafThermo::s ( const scalar p, const scalar T ) const { const coeffArray& a = coeffs(T); return this->RR* ( (((a[4]/4.0*T + a[3]/3.0)*T + a[2]/2.0)*T + a[1])*T + a[0]*::log(T) + a[6] ); }```

As for the other question:
Quote:
 Originally Posted by wyldckat 2. (Or) Is is possible to find what "S" is being used for internally in OpenFOAM?[/LIST]
In other words: if "S" is not accessible externally, then what is it used for internally?
Answer: looks like it's mostly for calculating "Gibbs free energy - g()" and "Helmholtz free energy - a()": https://github.com/OpenFOAM/OpenFOAM...thermoI.H#L172

All of this was found thanks to the Doxygen generated documentation: http://www.openfoam.org/docs/cpp/

 May 2, 2013, 09:42 #16 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 hi it displayes this error when compiling: Code: ```ehsan@Ehsan-com:~/Desktop/entropyHePsi\$ wmake Making dependency list for source file entropy.C could not open file cyclicAMILduInterfaceField.H for source file entropy.C could not open file cyclicAMILduInterface.H for source file entropy.C could not open file cyclicAMIPolyPatch.H for source file entropy.C SOURCE=entropy.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam220/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam220/src/thermophysicalModels/specie/lnInclude -I/opt/openfoam220/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam220/src/OpenFOAM/lnInclude -I/opt/openfoam220/src/OSspecific/POSIX/lnInclude -fPIC -c \$SOURCE -o Make/linux64GccDPOpt/entropy.o In file included from /opt/openfoam220/src/finiteVolume/lnInclude/jumpCyclicAMIFvPatchField.H:47:0, from /opt/openfoam220/src/finiteVolume/lnInclude/fixedJumpAMIFvPatchField.H:71, from /opt/openfoam220/src/finiteVolume/lnInclude/fixedJumpAMIFvPatchFields.H:29, from /opt/openfoam220/src/thermophysicalModels/basic/lnInclude/heThermo.C:32, from /opt/openfoam220/src/thermophysicalModels/basic/lnInclude/heThermo.H:320, from /opt/openfoam220/src/thermophysicalModels/basic/lnInclude/hePsiThermo.H:39, from /opt/openfoam220/src/thermophysicalModels/basic/lnInclude/psiThermos.C:41, from entropy.C:32: /opt/openfoam220/src/finiteVolume/lnInclude/cyclicAMIFvPatchField.H:62:40: fatal error: cyclicAMILduInterfaceField.H: No such file or directory compilation terminated. make: *** [Make/linux64GccDPOpt/entropy.o] Error 1``` __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 May 2, 2013, 10:01 #17 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 8,301 Blog Entries: 34 Rep Power: 84 OpenFOAM 2.2.0 has some broken stuff that has been already been fixed in 2.2.x.... Anyway, the quick fix is as follows: Edit the file "Make/options" and replace: Code: ```EXE_INC = \ -I\$(LIB_SRC)/thermophysicalModels/basic/lnInclude \ -I\$(LIB_SRC)/thermophysicalModels/specie/lnInclude \ -I\$(LIB_SRC)/finiteVolume/lnInclude``` For this: Code: ```EXE_INC = \ -I\$(LIB_SRC)/thermophysicalModels/basic/lnInclude \ -I\$(LIB_SRC)/thermophysicalModels/specie/lnInclude \ -I\$(LIB_SRC)/meshTools/lnInclude \ -I\$(LIB_SRC)/finiteVolume/lnInclude``` Then run: Code: ```wclean wmake``` __________________ OpenFOAM: Frequently Asked Questions | Useful links for building and using Forum: How to ask for help | Posting code and output with [CODE] My to-do list and when I'll be able to come to the forum: http://wyldckat.github.io And please: Read this before sending private messages to me

 May 2, 2013, 10:37 #18 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 thank you.it works except one of the cases.the error in this case is this: Code: ```ehsan@Ehsan-com:~/Desktop/WR_pimple_p\$ entropy /*---------------------------------------------------------------------------*\ | ========= | | | \\ / 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-b363e8d14789 Exec : entropy Date : May 02 2013 Time : 18:59:03 Host : "Ehsan-com" PID : 7363 Case : /home/ehsan/Desktop/WR_pimple_p 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 Time = 0 Re-reading thermophysical properties --> FOAM Warning : From function polyBoundaryMesh::groupPatchIDs() const in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 474 Patch empty specifies a group empty which is also a patch name. This might give problems later on. --> FOAM Warning : From function groovyBCFvPatchField::groovyBCFvPatchField(const fvPatch& p,const DimensionedField& iF,const dictionary& dict) in file groovyBCFvPatchField.C at line 131 No value defined for T on right therefore using 20{0} --> FOAM Warning : From function groovyBCFvPatchField::groovyBCFvPatchField(const fvPatch& p,const DimensionedField& iF,const dictionary& dict) in file groovyBCFvPatchField.C at line 131 No value defined for T on left therefore using 20{0} #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 Foam::hePsiThermo >, Foam::sensibleEnthalpy> > > >::calculate() in "/home/ehsan/OpenFOAM/ehsan-2.2.0/platforms/linux64GccDPOpt/bin/entropy" #4 in "/home/ehsan/OpenFOAM/ehsan-2.2.0/platforms/linux64GccDPOpt/bin/entropy" #5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #6 in "/home/ehsan/OpenFOAM/ehsan-2.2.0/platforms/linux64GccDPOpt/bin/entropy" Floating point exception``` is it related to S? S dimensions is in SI,correct? is there any real gas model in OF rather than perfectGas? __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 May 2, 2013, 10:41 #19 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 8,301 Blog Entries: 34 Rep Power: 84 The problem is that the T field is not properly defined for the time instance "0". It's assuming values of 0 K (zero Kelvin!) for the "left" and "right" patches, which therefore leads to some massive problems! Try: Code: `entropy -time '1e-30:'` __________________ OpenFOAM: Frequently Asked Questions | Useful links for building and using Forum: How to ask for help | Posting code and output with [CODE] My to-do list and when I'll be able to come to the forum: http://wyldckat.github.io And please: Read this before sending private messages to me

 September 8, 2013, 09:18 #20 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,186 Rep Power: 16 Hi Bruno I changed the dictionary for one of my cases as this: Code: ```#define myLengthyThermoClass makeTheLenghtyTypedefName( \ psiThermo, \ hePsiThermo, \ pureMixture, \ constTransport, \ sensibleEnthalpy, \ hConstThermo, \ perfectGas, \ specie \ )``` but this is the error: Code: ```Create time Create mesh for time = 0.01586 Time = 0.01586 Re-reading thermophysical properties [3] [3] [3] --> FOAM FATAL ERROR: [3] Not implemented [3] [3] From function scalar hConstThermo::s(const scalar p, const scalar T) const [3] in file /opt/openfoam220/src/thermophysicalModels/specie/lnInclude/hConstThermoI.H at line 150. [3] FOAM parallel run aborting [3] [3] #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [3] #1 Foam::error::abort()[1] Calculating S [0] [0] [0] --> FOAM FATAL ERROR: [0] Not implemented [0] [0] From function scalar hConstThermo::s(const scalar p, const scalar T) const [0] in file /opt/openfoam220/src/thermophysicalModels/specie/lnInclude/hConstThermoI.H at line 150. [0] FOAM parallel run aborting [0] in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [3] #2 [2] [2] [2] --> FOAM FATAL ERROR: [2] Not implemented [2] [2] From function scalar hConstThermo::s(const scalar p, const scalar T) const [2] in file /opt/openfoam220/src/thermophysicalModels/specie/lnInclude/hConstThermoI.H at line 150. [2] FOAM parallel run aborting [2] [1] [1] --> FOAM FATAL ERROR: [1] Not implemented [1] [1] From function scalar hConstThermo::s(const scalar p, const scalar T) const [1] in file /opt/openfoam220/src/thermophysicalModels/specie/lnInclude/hConstThermoI.H at line 150. [1] FOAM parallel run aborting [1] [2] #0 Foam::error::printStack(Foam::Ostream&)[0] #0 Foam::error::printStack(Foam::Ostream&)[1] #0 Foam::error::printStack(Foam::Ostream&) [3] in "/home/ehsan/OpenFOAM/ehsan-2.2.0/platforms/linux64GccDPOpt/bin/entropyConst" [3] #3 __libc_start_main in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [2] #1 Foam::error::abort() in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [0] #1 Foam::error::abort() in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [1] #1 Foam::error::abort() in "/lib/x86_64-linux-gnu/libc.so.6" [3] #4 in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [2] #2 in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [1] #2 -------------------------------------------------------------------------- MPI_ABORT was invoked on rank 3 in communicator MPI_COMM_WORLD with errorcode 1. NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes. You may or may not see output from other processes, depending on exactly when Open MPI kills them. -------------------------------------------------------------------------- [3] in "/home/ehsan/OpenFOAM/ehsan-2.2.0/platforms/linux64GccDPOpt/bin/entropyConst" in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [0] #2 [2] in "/home/ehsan/OpenFOAM/ehsan-2.2.0/platforms/linux64GccDPOpt/bin/entropyConst" [2] #3 __libc_start_main[1] in "/home/ehsan/OpenFOAM/ehsan-2.2.0/platforms/linux64GccDPOpt/bin/entropyConst" [1] #3 __libc_start_main-------------------------------------------------------------------------- mpirun has exited due to process rank 3 with PID 6760 on node Ehsan-com exiting without calling "finalize". This may have caused other processes in the application to be terminated by signals sent by mpirun (as reported here). --------------------------------------------------------------------------``` __________________ Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36 wyldckat OpenFOAM Bugs 18 October 21, 2010 05:51 hansel OpenFOAM Installation 62 March 19, 2010 15:43 Valle OpenFOAM Running, Solving & CFD 4 August 19, 2009 05:53 Cormac Main CFD Forum 4 August 13, 2000 23:26

All times are GMT -4. The time now is 17:11.

 Contact Us - CFD Online - Top