[.bastian]

Hi Yuusha, hi folks,


i kinda don't get it compiled using your instructions given on your github page.

Allwmake /home/sebastian/OpenFOAM/FOAMExtensions/tabulatedThermophysicalProperties/src
wmakeLnInclude: linking include files to OpenFOAM/lnInclude
wmake thermophysicalModels/specie
wmakeLnIncludeAll: running wmakeLnInclude on dependent libraries:
    wmakeLnInclude error: base directory /home/sebastian/OpenFOAM/sebastian-6/src/OpenFOAM/ does not exist
g++ -std=c++11 -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -Wno-attributes -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam6/src/thermophysicalModels/specie/lnInclude -I/home/sebastian/OpenFOAM/sebastian-6/src/OpenFOAM/lnInclude -IlnInclude -I. -I/opt/openfoam6/src/OpenFOAM/lnInclude -I/opt/openfoam6/src/OSspecific/POSIX/lnInclude   -fPIC -c reaction/reactions/makeTabularReactions.C -o Make/linux64GccDPInt32Opt/reaction/reactions/makeTabularReactions.o
In file included from lnInclude/tabularThermoPhysicsTypes.H:42,
                 from lnInclude/tabularReactionTypes.H:36,
                 from reaction/reactions/makeTabularReactions.C:27:
lnInclude/tabularEOS.H:41:10: fatal error: extrapolation2DTable.H: file or folder not found
 #include "extrapolation2DTable.H"
              ^~~~~~~~~~~~~~~~~~~~~~~~
compilation terminated.
make: *** [/opt/openfoam6/wmake/rules/General/transform:26: Make/linux64GccDPInt32Opt/reaction/reactions/makeTabularReactions.o] error 1

Can anyone give me a hint what I'm doing wrong?

EDIT: Got it. I've messed up the correct path in the bashrc.

[iiigoriii]

Dear Yuusha,
thank you for your work. Could you please also add example with tabular reaction?
Thanks, BR, ii

[Yuusha]

Hi iiigoriii,


Unfortunately I havent'got a case with reactionThermo. I have tested it a long time ago with a two gas mixture without reaction and it works well. However I do not use it anymore.
Maybe you can try to modify the current tutorial by adding a second specie and look at OpenFOAM reacting test cases to add the needed files.
I have added a issue in GitHub to remind me to add a reacting tutorial case.

[vince_cfd]

Hallo everyone,
has anyone tested this under OFv7 yet? I can't make it work in OFv7, but I'm not sure if I'm doing it wrong, or if it's a compatibility problem.

Using the ./Allwmake command seems to do a lot, but also returns an error at the end:

/home/cfd/OpenFOAM_ESI/OpenFOAM-v1906/wmake/rules/General/transform:34: recipe for target 'Make/linux64GccDPInt32Opt/tabularThermo/tabularThermos.o' failed
 make: *** [Make/linux64GccDPInt32Opt/tabularThermo/tabularThermos.o] Error 1

When trying to run the tutorial testcase it returns >>>could not load "libTabularThermophysicalModels.so"<<< and some other library files.
Any ideas?


EDIT: Just found the OF7 version: simply click on the Branch drop-down menu and select the correct version. Installing it now.

[CarlosRom90]

Hello everyone,


I have tried to compute in parallel the tutorial case from https://github.com/Yuusha0/tabulated...icalProperties.


Surprisingly, it didn't work with the decomposeParDict delivered in tutorial case system folder, where the authors proposed to use the "scotch" methods.


I even tried with simple decomposition but it also failed.


Any ideas?


Thanks in advance.



PS: The decomposeParDict file in below:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

numberOfSubdomains 8;

method scotch;


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

[.bastian]

Originally Posted by CarlosRom90

[...]
Surprisingly, it didn't work with the decomposeParDict delivered in tutorial case system folder, where the authors proposed to use the "scotch" methods.

I even tried with simple decomposition but it also failed.

Any ideas?

[...]

Ciao Carlos,

this should do the trick:

1. Comment or remove the following lines in your control dict, that this:

libs
(
    "libuserspecie.so"
    "libTabularThermophysicalModels.so"
    "libtabularReactionThermophysicalModels.so"
);

becomes:

// libs
// (
//     "libuserspecie.so"
//     "libTabularThermophysicalModels.so"
//     "libtabularReactionThermophysicalModels.so"
// );

2. Run decomposePar

3. Undo step 1 and run your simulation.

Certainly not the most elegant solution, baer it works - At least for me

[Yuusha]

Hi,

The official release for OpenFOAM-7 is available on GitHub : https://github.com/Yuusha0/tabulated...icalProperties.

Sorry for the long delay. Apart from the switch to OpenFOAM-7 this new release brings some fixes.

First, a new numbering system is used for release. I think it is easier to understand. The first number is the OpenFOAM version (in that case 7), the second number is the tabulated properties version for this OpenFOAM (so 7.1 for the first with OpenFOAM-7) and the last number will be used for bug fixes (actually it is 7.1.0).

Second, the bug with sensibleEnthalpy model is now (normally) fixed. Feel free to test it if you have cases using this model.

Third, the tutorial has been improved. It is a more physical case and it supports sensibleEnthalpy thermopysical model.

And last but not least, old version (OpenFOAM-6 one) is now preserved in a Old_OF6 version on GitHub. So it will be easier if you want to download it or suggest bug fixes.

[CarlosRom90]

Hi everyone,


First, thanks .bastian your tip worked in my case


Second, Yuusha, I was wondering if the tabulated thermo would work for cases with conjugate heat transfers (chtMultiRegionFoam).



Thank you!

[Yuusha]

Hi CarlosRom90,


There is no problem for using the tabulated thermo for the fluid part in chtMultiRegionFoam. Unfortunately, you cannot use it for the solid part.

[CarlosRom90]

Thank you for your answer Yuusha.


I'm trying to use chtMultiRegionFoam solver with tabulatedThermo (fluid part).


To test both together I used the heatTransfer/chtMultiRegionFoam/heatedDuct tutorial as test case.



So, I added the required libraries inside controlDict:


libs
(
"libuserspecie.so"
"libTabularThermophysicalModels.so"
"libtabularReactionThermophysicalModels.so"
);


and when I run the simulation to check the available thermophysical models I get only the following with tabularThermo:


" heRhoThermo-reactingMixture-tabular-hTabular-tabularEOS -specie-sensibleInternalEnergy "

I am interested in:


heRhoThermo-pureMixture-tabular-hTabular-tabularEOS -specie-sensibleInternalEnergy


heRhoThermo-pureMixture-tabular-hTabular-tabularEOS -specie-sensibleEnthalpy




I think it should not be too complicated, but I tried to modified the src/ folder inside the tabulatedThermophysicalProperties-master and I didn't success...



Could you maybe give me an advice?


Thank you in advance!

Originally Posted by Yuusha

Hi CarlosRom90,


There is no problem for using the tabulated thermo for the fluid part in chtMultiRegionFoam. Unfortunately, you cannot use it for the solid part.

[Yuusha]

Originally Posted by CarlosRom90

and when I run the simulation to check the available thermophysical models I get only the following with tabularThermo:


" heRhoThermo-reactingMixture-tabular-hTabular-tabularEOS -specie-sensibleInternalEnergy "

I am interested in:


heRhoThermo-pureMixture-tabular-hTabular-tabularEOS -specie-sensibleInternalEnergy


heRhoThermo-pureMixture-tabular-hTabular-tabularEOS -specie-sensibleEnthalpy




I think it should not be too complicated, but I tried to modified the src/ folder inside the tabulatedThermophysicalProperties-master and I didn't success...



Could you maybe give me an advice?


Thank you in advance!

Ok. I don't know why but OpenFOAM uses reaction thermo for chtMultiRegionFoam.


You have to edit the tabularReactionsThermos.C file in the src/thermophysicalModels/reactionThermo/tabularReactionThermo/ directory. Copy the structure written line 56 paste in the same file whith the desired properties. Maybe it is :
makeReactionThermos
(
rhoThermo,
rhoReactionThermo,
heRhoThermo,
pureMixture,
tabularTransport,
sensibleInternalEnergy,
hTabularThermo,
tabularEOS,
specie
);

and

makeReactionThermos
(
rhoThermo,
rhoReactionThermo,
heRhoThermo,
pureMixture,
tabularTransport,
sensibleEnthalpy,
hTabularThermo,
tabularEOS,
specie
);


Recompile the src folder and it should work.

[pranay347]

Originally Posted by Yuusha

Ok. I don't know why but OpenFOAM uses reaction thermo for chtMultiRegionFoam.


You have to edit the tabularReactionsThermos.C file in the src/thermophysicalModels/reactionThermo/tabularReactionThermo/ directory. Copy the structure written line 56 paste in the same file whith the desired properties. Maybe it is :
makeReactionThermos
(
rhoThermo,
rhoReactionThermo,
heRhoThermo,
pureMixture,
tabularTransport,
sensibleInternalEnergy,
hTabularThermo,
tabularEOS,
specie
);

and

makeReactionThermos
(
rhoThermo,
rhoReactionThermo,
heRhoThermo,
pureMixture,
tabularTransport,
sensibleEnthalpy,
hTabularThermo,
tabularEOS,
specie
);


Recompile the src folder and it should work.

hi

i am too trying to make a new thermophysicalModel for my case i just need to make new combination of

thermoType
{
type heRhoThermo;
mixture pureMixture;
transport sutherland;
thermo hPolynomial;
equationOfState perfectGas;
specie specie;
energy sensibleEnthalpy
}
so i added this class in thermophysicalModel/basic/rhoreaction/rhothermos.c file and compiled without changing the file and option files in make folder, it compiled but not using in the simulation as its giving same error of "unknown reaction thermo" and listing valid thermo types.
so do i need to change the files and option files ? if so what are the changes? and any other changes?

Thank you
Pranay

[Yuusha]

Hi,


A new version (v7.2.0) is available on GitHub : https://github.com/Yuusha0/tabulated...icalProperties.

It fixes a bug with tables for multi-species simulations. It adds a 'pseudo tutorial' for multi-species with tabulated properties. The tutorial does not properly work. It crashes after some iterations. But you can use it to set-up more quickly your multi-species calculations.

Last, it adds a new perfectGas switch option for equation of state property (default is false). With this option Cp - Cv is calculated for a perfect gas. It can help you with unstable calculation when the standard model does not work.

[joaran]

Originally Posted by .bastian

Hi Yuusha, hi folks,


i kinda don't get it compiled using your instructions given on your github page.

Allwmake /home/sebastian/OpenFOAM/FOAMExtensions/tabulatedThermophysicalProperties/src
wmakeLnInclude: linking include files to OpenFOAM/lnInclude
wmake thermophysicalModels/specie
wmakeLnIncludeAll: running wmakeLnInclude on dependent libraries:
    wmakeLnInclude error: base directory /home/sebastian/OpenFOAM/sebastian-6/src/OpenFOAM/ does not exist
g++ -std=c++11 -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -Wno-attributes -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam6/src/thermophysicalModels/specie/lnInclude -I/home/sebastian/OpenFOAM/sebastian-6/src/OpenFOAM/lnInclude -IlnInclude -I. -I/opt/openfoam6/src/OpenFOAM/lnInclude -I/opt/openfoam6/src/OSspecific/POSIX/lnInclude   -fPIC -c reaction/reactions/makeTabularReactions.C -o Make/linux64GccDPInt32Opt/reaction/reactions/makeTabularReactions.o
In file included from lnInclude/tabularThermoPhysicsTypes.H:42,
                 from lnInclude/tabularReactionTypes.H:36,
                 from reaction/reactions/makeTabularReactions.C:27:
lnInclude/tabularEOS.H:41:10: fatal error: extrapolation2DTable.H: file or folder not found
 #include "extrapolation2DTable.H"
              ^~~~~~~~~~~~~~~~~~~~~~~~
compilation terminated.
make: *** [/opt/openfoam6/wmake/rules/General/transform:26: Make/linux64GccDPInt32Opt/reaction/reactions/makeTabularReactions.o] error 1

Can anyone give me a hint what I'm doing wrong?

EDIT: Got it. I've messed up the correct path in the bashrc.

Hi all! First of all, thanks for sharing such a valuable tool.

I'm having the same output as Bastian when hitting "./Allwmake". I followed the instructions of the "README" in github. The sourcing part look fine to me:

[usuario@localhost src]$ echo $TAB_PROPERTIES
/home/usuario/OpenFOAM/usuario-7
[usuario@localhost src]$ emacs ../etc/bashrc&

Could anyone please guide me on how to solve this issue?
I'm using OF 7, and the last available version of the tabulated library.

Thank you!

I also could just solve this issue by placing the contents of the folder "tabulatedThermophysicalProperties" in $WM_PROJECT_USER_DIR

[vortexnix]

Originally Posted by joaran

Hi all! First of all, thanks for sharing such a valuable tool.

I'm having the same output as Bastian when hitting "./Allwmake". I followed the instructions of the "README" in github. The sourcing part look fine to me:

[usuario@localhost src]$ echo $TAB_PROPERTIES
/home/usuario/OpenFOAM/usuario-7
[usuario@localhost src]$ emacs ../etc/bashrc&

Could anyone please guide me on how to solve this issue?
I'm using OF 7, and the last available version of the tabulated library.

Thank you!

I also could just solve this issue by placing the contents of the folder "tabulatedThermophysicalProperties" in $WM_PROJECT_USER_DIR

Or if you update bashrc such that
echo $TAB_PROPERTIES
gives
/home/usuario/OpenFOAM/usuario-7/tabulatedThermophysicalProperties