Species not found when using reduced H2 mechanism with reactingFoam
 

I was trying to simulate the usual Sandia D's flame from tutorial but using H2 instead CH4. With GRI3.0 mech all worked out just fine. As solver I chose following the tutorial reactingFoam. Now I was aiming at simulating it with a reduced mechanism: https://chemistry.cerfacs.fr/en/chem...ins-mechanism/.

Unfortunately, this does not work anymore. I've been trying to converse the original mech from .cti to .yaml and then to Chemkin. Finally, a last conversion from ck to foam is carried out. After this last step, some minor changes (e.g. spacing, THERMO to THERMO ALL) have to be applied so OF does not complain.

In any case, I still get the following error log:

...
Selecting combustion model EDC
Selecting chemistry solver
{
solver ode;
method chemistryModel;
}

odeChemistryModel: Number of species = 10
Selecting chemistry reduction method DAC


--> FOAM FATAL ERROR:
CH4 not found in table. Valid entries:
10
(
OH
KOH
N2
K
O2
H2
HO2
O
H2O
H
)


From function const T& Foam::HashTable<T, Key, Hash>::operator[](const Key&) const [with T = int; Key = Foam::word; Hash = Foam::string::hash]
in file /home/ubuntu/OpenFOAM/OpenFOAM-10/src/OpenFOAM/lnInclude/HashTableI.H at line 126.

FOAM exiting ...



I've grepped through all the directories in order to spot and delete eventual places where the missing species is, but the error keeps on appearing.

Any help is more than appreciated :(


Ps. I am using OF 10 from OF foundation

Any updates on this topic? I'm having the same exact problem. There are other threads discussing this issue and none have gotten resolved.


If someone has already encountered this problem, could you give an hint on how you came up with a solution? Any help would be much appreciated.


Best Regards,

Thomas.

Hi There!



Found the solution for this problem. I had to edit the "chemistryPropertiesFlame.cfg" file to exclude CH4 from the initiating species. Using "$ grep -r CH4 *" wasn't getting any apearences inside the case folder, as this file is in "$FOAM_ETC/caseDicts/solvers/chemistry/TDAC/" directory. I don't know about the .com version, but with the foundation version i had to copy the "chemistryPropertiesFlame.cfg" file to the constant folder and "#include chemistryPropertiesFlame.cfg" in the chemistryProperties file. I'm using OpenFOAM v10 form the foundation version.


Greetings,


Thomas.

Thank you very much Thomas!! That solved also my issue.

Cheers!