[sqek]

Hello
Have you run topoSet since changing the actions in topoSetDict?
The names of the sets shouldn't cause an error, as long as they're the same in actions in topoSetDict as they are in singleProcessorFaceSets in decomposeParDict.
I'd suggest using the original names, as openFOAM sometimes automatically generates cellSets called region0, region1 etc, which would then get confused with the faceSets you're making
So put the original names in both topoSetDict and singleProcessorFaceSets,
then run topoSet (and look through the output - it should tell you the size of each set it makes, check that the number of faces in each is something reasonable)
If it's making too much output to easily read, run topoSet &>log.topoSet, then look at the log.topoSet file
then try decomposePar again

[qutadah.r]

So, thanks alot for the advices and hints! It finally works @sqek


here is how my files look like, for purposes of documentation for anyone who runs through this problem again


1- in topoSetDict i added:

actions
(
{
name INT_BLADE_1;
type faceSet;
action new;
source patchToFace;
sourceInfo
{
name "INT_BLADE_1-SIDE-1";
}
}

{
name INT_BLADE_1;
type faceSet;
action add;
source patchToFace;
sourceInfo
{
name "INT_BLADE_1-SIDE-2";
}
}
.
.
.

and so on for all my patches to gather them in sets like above....




2- in decomposeParDict i added:

constraints
{
singleProcessorFaceSets
{
        type singleProcessorFaceSets;
        singleProcessorFaceSets (
                (INT_BLADE_1 -1)
                (INT_BLADE_2 -1)
                (INT_BLADE_3 -1)
                (INT_BLADE_4 -1)
                (INT_BLADE_5 -1)
                (INT_BLADE_6 -1)
                (INT_IMP_VOL -1)
                (INT_SP_IMP -1)
                );
        enabled true;
    }
}

and then i ran topoSet and then decomposePar like said.


Thanks alot for your help!