[MicoZeinam]

First of all, Hi to all !

this forum helped me a lot in the past but today i'm gonna be crazy...
I'm a beginner who have to use some data from OpenFOAM 2.2.1 concerning a case running with porousInterFoam solver on OF 2.3.0

Since few weeks now they updated OF to version 2.3.0 and I can't use my folder anymore. When I launch my template with mpirun in parallel I got an error message with "transportProperties":

Reading transportProperties

--> FOAM Warning :
From function entry::getKeyword(keyType&, Istream&)
in file db/dictionary/entry/entryIO.C at line 80
Reading /home/maniez/OpenFOAM/maniez-2.3.0/run/biggerMesh_190s_5e-11_porosity05_p2/constant/transportProperties
found on line 22 the punctuation token '{'
expected either } or EOF

I have already checked the "{" problem but I think my folder is ok.
I read on forum that an update was done about how to define fluids via "phase (xx1 xx2);" in transportProperties. I'm not sure about this because my fluid is named "alpha1" in 0/ , constant/, system/. I tried to change with new name but it was not working at all so I kept alpha1.

I enclosed the job-parallel error file and my tranportProperties file. (open with NotePAD++)

Thanking in advance for your help...

greatings

Mico.

[alexeym]

Hi,

You can check transportProperties syntax in tutorial cases for interFoam.

According to your log, error happens in twoPhaseMixture constructor, which is quite simple:

Foam::twoPhaseMixture::twoPhaseMixture
(
    const fvMesh& mesh,
    const dictionary& dict
)
:
    phase1Name_(wordList(dict.lookup("phases"))[0]),
    phase2Name_(wordList(dict.lookup("phases"))[1]),
    ...
{}

Your empty phases list makes OpenFOAM unhappy (I have decided not to search for the reason why the error message is about {). Also the signal is sigSegv, guess access to the second element of empty word list causes the error.

Did you try:

phases (resin air);

resin
{
    ...
}

air
{
    ...
}

?

[MicoZeinam]

Originally Posted by alexeym

Did you try:

phases (resin air);

resin
{
    ...
}

air
{
    ...
}

?

Hi, Thanks for your answer,

Yes I tried this but I'm not sure if I did it well... (based on forums)
- I changed my tranportProperties with "resin" and "air".
- After OF was looking for 0/alpha.resin so i changed old file 0/alpha1.org by 0/alpha.resin.org
- Changed in setFieldsdict alpha1 ---> alpha.resin
- fvSchemes, alpah1 became alpha.resin

I tried with setFields to check and it was working but I got lots of errors when I launched the solver. I think i forgot to redefine something somewhere in my folder like the solver or equations (may call alpha1)

Did i miss something with the new way to name fluids ?

I can tried again with your syntax and post the error log if you want.

Sorry for my beginner questions :-)

thanks.

[alexeym]

Hi,

Everything is correct except fvSchemes, there should be just alpha. alpha.resin.* should appear in fvSolution (also settings for solution of alpha equation are moved from PIMPLE dictionary to separate sub-dictionary in solvers dictionary).

As I said: take a look at interFoam tutorials (porousInterFoam is just a derivative, and now it is even redundant as interFoam + fvOptions do the same).

[MicoZeinam]

Hi,

I did all the changes again and add "alpha.resin.*" as it's done in interFoam in fvSolution.
Concerning fvSchemes I put "alpha" in fluxreauired but after tested it it asked me to put "alpha.resin".

I tried again to launch the solver but now I have another error:

--> FOAM FATAL IO ERROR:
[2] keyword div(rhoPhi,U) is undefined in dictionary "IOstream.divSchemes"
[2]
[2] file: IOstream.divSchemes from line 0 to line 0.
[2]
[2] From function dictionary::lookupEntry(const word&, bool, bool) const
[2] in file db/dictionary/dictionary.C at line 437.

But "div(rho*Phi,U) is defined in it (fvSchemes)... It was working properly with old version and if I compare with interfoam, it's the same equation.

I really appreciate your help !

Ps: I enclosed new error log and fvSolution/Schemes.

[MicoZeinam]

Forget my last post... I saw my mistake !

div(rhoPhi, U) is not the same as old one div(rho*phi, U) ... Code is running now !! I will tell you in 1,5h if everything is fine !

Thanks you so much for your help !

I will keep your name in mind for the futur ahahah.

et merci bcp ;-)