[hannes]

Hello to everyone,

I encounter a problem when I try to use the the cyclicGgi in MRFSimpleFoam in a parallel run (using the latest OF-1.5-dev from SVN).
As I have found out, the new GGI-Implementation requires the two cyclic patches to be in two different zones whereas the MRF solver requires them to be in the rotor zone. So, I have defined the two cyclic face zones in the constant/MRFZones dict to be rotating as well (symmm and symmp are the cyclic patch face zones, the corresponding cellZones are empty):

3
(
rotor
{
patches (PROP);
origin origin [0 1 0 0 0 0 0] (0 0 0);
axis axis [0 0 0 0 0 0 0] (0 0 1);
omega omega [0 0 -1 0 0 0 0] 58.6431;
}
symmm
{
patches ();
origin origin [0 1 0 0 0 0 0] (0 0 0);
axis axis [0 0 0 0 0 0 0] (0 0 1);
omega omega [0 0 -1 0 0 0 0] 58.6431;
}
symmp
{
patches ();
origin origin [0 1 0 0 0 0 0] (0 0 0);
axis axis [0 0 0 0 0 0 0] (0 0 1);
omega omega [0 0 -1 0 0 0 0] 58.6431;
}
)

This seems to work in serial, but when I try to run the case in parallel, the following error occurs:

Starting time loop
Time = 1
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0591515, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0426731, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0704887, No Iterations 2
[1]
[1]
[1] given label greater than the number of geometric faces
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/kroegeh/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/kroegeh/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam:olyBoundaryMesh::whichPatch(int) const in "/home/kroegeh/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so"
#3 Foam::MRFZone::relativeFlux(Foam::GeometricField<d ouble, Foam::fvsPatchField, Foam::surfaceMesh>&) const in "/home/kroegeh/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libfiniteVolume.so"
#4 Foam::MRFZones::relativeFlux(Foam::GeometricField< double, Foam::fvsPatchField, Foam::surfaceMesh>&) const in "/home/kroegeh/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libfiniteVolume.so"
#5 main in "/home/kroegeh/OpenFOAM/kroegeh-1.5-dev/applications/bin/linux64GccDPOpt/MRFSimpleFoam"
#6 __libc_start_main in "/lib/libc.so.6"
#7 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/kroegeh/OpenFOAM/kroegeh-1.5-dev/applications/bin/linux64GccDPOpt/MRFSimpleFoam"

It seems that the MRFZones-Code tries to access some faces that are not present. Is there a nice and elegant way to fix that?

Best regards, Hannes

[hannes]

For those who are interested: I have fixed it by inserting the marked statement below in MRFZones.C (in function "relativeFlux"):

forAll(faces, i)
{
label facei = faces;
if (facei < mesh_.nInternalFaces())
{
phi[facei] -= (Omega ^ (Cf[facei] - origin)) & Sf[facei];
}
[i] else if (facei < mesh_.nFaces())
{
label patchi = mesh_.boundaryMesh().whichPatch(facei);
label patchFacei = mesh_.boundaryMesh()[patchi].whichFace(facei);
phi.boundaryField()[patchi][patchFacei] -=
(Omega ^ (Cf.boundaryField()[patchi][patchFacei] - origin))
& Sf.boundaryField()[patchi][patchFacei];
}
}

[bastil]

Hannes,

take into account using the MRF from 1.5.x combined with ggi from 1.5-dev. The latest MRF can use cellZones without Facezones so you can form a cellzone for your mrf and a faceZone for the ggi.

Regards.

[raavis]

Hanes

I am trying to setup a MRF simulaton with ggi. Will it be possible for you to send me your system dictionaries, constant/dictionaries, boundary file and 0/files?

Thanks

[hjasak]

Fixed - thank you for the bug fix. Apologies - there may be a few more problems like this because the mesh is now a bit more complex.

Hrv

[timo_IHS]

Hello everybody,

I also want to run MRFSimpleFoam with cyclicGgi (latest OF-1.5-dev version).
Running this job in parallel doesn't work, a single run works.
Is there a mistake in my setup or is it a generell problem to run MRF with cyclicGgi in parallel?

Thanks in advance
Timo

[bastil]

Parallel run should work. Without knowing you setup I would suspect it is more likely to have an error in this than a problem with Paralleisation. How doues your setup look like? How did you decompose your case?

Regards.

[timo_IHS]

The steps of my setup are:

I. the "makeMesh" file for the setup
####for MRF:
cellSet ###choose all cells of rotor
setsToZones -noFlipMap
cp system/faceSetDict_rotorFaces system/faceSetDict
faceSet ###choose all faces of set rotor
cp system/faceSetDict_delInlet system/faceSetDict
faceSet ###delete faces of patch inlet
cp system/faceSetDict_delOutlet system/faceSetDict
faceSet ###delete faces of patch outlet
####for cyclicGgi:
cp system/faceSetDict_per1 system/faceSetDict
faceSet ###create face-zone per1_zone
cp system/faceSetDict_per2 system/faceSetDict
faceSet ###create face-zone per2_zone
setsToZones -noFlipMap


II: my constant/MRFzones:
1
(
rotor
{
patches (hub per1 per2 shroud blade);
origin origin [0 1 0 0 0 0 0] (0 0 0);
axis axis [0 0 0 0 0 0 0] (0 0 1);
omega omega [0 0 -1 0 0 0 0] 100.81;
}
)


III: my system/decomposeParDict:
numberOfSubdomains 2;

method metis;

globalFaceZones ( per1_zone per2_zone );
metisCoeffs
{
processorWeights
(
1 1
);
}
...


Btw: I checked one setup possibility, I want to tell (single run):
if I delete the periodic faces of my set rotor (I), the results at the ggi are nonsens (velocity and pressure profile)

If you need some more info, let me know!