CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   cavity tutorial problem in OF 3.0.x (https://www.cfd-online.com/Forums/openfoam-solving/166625-cavity-tutorial-problem-3-0-x.html)

mohsen.boojari February 13, 2016 13:44
cavity tutorial problem in OF 3.0.x
 
hi everyone,
i tried to run the tutorial example of openFoam 3.0.x but i got this error.

Code:
--> FOAM FATAL IO ERROR:
keyword pFinal is undefined in dictionary "/home/mohen/OpenFOAM/mohen-3.0.x/run/tutorials/incompressible/icoFoam/cavity/system/fvSolution.solvers"

file: /home/mohen/OpenFOAM/mohen-3.0.x/run/tutorials/incompressible/icoFoam/cavity/system/fvSolution.solvers from line 22 to line 33.

    From function dictionary::subDict(const word& keyword) const
    in file db/dictionary/dictionary.C at line 648.

FOAM exiting
any idea whats wrong?? :confused::confused: i searched throw the fvsolution script but i didn't see any pFinal there. i also copied the cavity tutorial from other versions but nothing changed

thanks all

alexeym February 14, 2016 04:20
Hi,

cavity tutorial is meant to be run with icoFoam, yet it seems you are trying to run PISO/PIMPLE family solver. As of commit a2e25d5, icoFoam runs smoothly in cavity tutorial.

mohsen.boojari February 14, 2016 04:55
Quote:
Originally Posted by alexeym (Post 585089)
Hi,

cavity tutorial is meant to be run with icoFoam, yet it seems you are trying to run PISO/PIMPLE family solver. As of commit a2e25d5, icoFoam runs smoothly in cavity tutorial.
Hi
I followed exactly the commands in the openfoam website, i'm sure i entered icoFoam to solve.

alexeym February 14, 2016 05:32
Hi,

You are right, I should have recompiled icoFoam with newly checked out source. As a workaround for the problem, you can change this part of fvSolution:

Code:
    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance      1e-06;
        relTol          0;
    }
and make it

Code:
    "p.*"
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance      1e-06;
        relTol          0;
    }
(so PCG linear solver is used for p and pFinal). Also you can report broken tutorial case in Mantis (http://openfoam.org/mantisbt).

mohsen.boojari February 14, 2016 10:45
Quote:
Originally Posted by alexeym (Post 585094)
Hi,

You are right, I should have recompiled icoFoam with newly checked out source. As a workaround for the problem, you can change this part of fvSolution:

Code:
    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance      1e-06;
        relTol          0;
    }
and make it

Code:
    "p.*"
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance      1e-06;
        relTol          0;
    }
(so PCG linear solver is used for p and pFinal). Also you can report broken tutorial case in Mantis (http://openfoam.org/mantisbt).
Hi
thanks for your useful reply. I have another question. is there a problem with icoFoam in this version? or this error was just for the cavity tutorial?

Thanks

alexeym February 14, 2016 11:03
Hi,

I think all icoFoam tutorials became broken after commit 21cbbf7. I.e. after this source modification:

Code:
commit 21cbbf7beb561ce13a67790ce4c36a1371b17cd0
Author: Henry Weller <http://cfd.direct>
Date:  Thu Jan 28 09:03:51 2016 +0000

    pisoControl: Corrected handling of final inner (PISO) iteration control
...
+inline bool Foam::pisoControl::finalInnerIter() const
+{
+    return
+      corrPISO_ == nCorrPISO_
+    && corrNonOrtho_ == nNonOrthCorr_ + 1;
+}
fvSolution files in all icoFoam tutorials have to be modified ("p.*" instead of p, as I have written in previous post).


All times are GMT -4. The time now is 05:31.