[biscarri]

Hi,

I run a model in parallel with simpleFOAM, that worked OK with OF previous version, and now when running with OF3.0.0 gives and MPI_ABORT error.
Please find enclosed log file.
Thanks for any help, advice.

Lluis

[biscarri]

In the parallel run the MPI_ABORT error is produced after simpleFoam completes the first time iteration.

I have tried to run the case in serial and simpleFoam completes the first time step but does not continue iterating (contrlDict file specifies to run 2000 time steps) and does not create postPrcessing folder with results.

Then the problem seems to have no relation with running the case in parallel.

Any suggestion?

Thank U

[floquation]

No one will be able to help you if you only post the STDOUT stream. The useful information is usually contained in the STDERR stream.

When you redirect your solver output to a file, please also redirect the error to it:

solverName >log 2>&1

Although, I do notice that your solver seems to only care about achieving a residual of 0.1 for k. What convergence criterion did you specify? Then I see that kmin is negative. Something is probably going wrong right there.

[biscarri]

Thank you very much for yur respnse, Kevin.

Please find enclosed the file log.simpleFoam resulting from

simpleFoam > log.simpleFoam 2>&1

I don't understand in this case the meaning of "FOAM FATAL ERROR: Could not find rho", after solving the first time step. I don't figure out what 'rho' has to do with simpleFoam, since I understand that NS equations are divided by 'rho' in OF.

I attach also file fvSolution with the convergence criteria for the diferent solvers. In this run simpleFoam is specified to complete 2000 timesteps.

[Joshua14]

The reason your simulation crashed is that rho does not seem to be defined for your function object forces.

--> FOAM FATAL ERROR:
Could not find rho

From function void Foam::functionObjects::forces::initialise()
in file forces/forces.C at line 196.

FOAM exiting

Joshua

[biscarri]

Thanks for the comment, Joshua.

The folder constant contains the file transportProperties, where rho and nu are defined.

The forceCoeffs file in the system folder contains the definition of rhoName and rhoInf for postprocessing purposes..

Please find those files attached.

[Joshua14]

What does your controlDict look like?

[biscarri]

here it is controlDict file...

[Joshua14]

Everything looks like it is defined right. I am not sure why it is erroring out then. It is hung up on the postProcessing step tho. Hence the forces.C file.

[alexeym]

Hi all,

@biscarri

If you look into $FOAM_SRC/functionObjects/forces/forces/forces.C read method:

        ...
        // Optional entries U and p
        pName_ = dict.lookupOrDefault<word>("p", "p");
        UName_ = dict.lookupOrDefault<word>("U", "U");
        rhoName_ = dict.lookupOrDefault<word>("rho", "rho");
        ...

So this

...
pName               p; 
UName               U; 
rhoName             rhoInf; 
...

should be

p p;
U U;
rho rhoInf;

You can even remove p and U entries.

Also you can look at the header comment in $FOAM_SRC/functionObjects/forces/forces/forces.H, where parameters names are put into table.

[biscarri]

Thank you very much Alexey, now simpleFOAM is processing forces properly.