[hbrist7]

Hi,

I'm fairly new to OpenFOAM and am trying to run the rhoCentralFoam solver in parallel (with 8 processors). I keep getting the following error:

"--> FOAM FATAL IO ERROR:
Cannot find patchField entry for procBoundary0to3

file: home/mpiuser/OpenFOAM/mpiuser-3.0.1/run/henry/rhoCentralTest/processor0/0/p.boundaryField from line 25 to line 58.

From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh&, const dictionary&)

in file /home/openfoam/OpenFOAM/OpenFOAM-3.0.1/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209

FOAM parallel run exiting"

I have tried creating placeholder procBoundary entries in the 0/p, 0/T and 0/U files inside the boundaryField dictionary in each of those files:

boundaryField
{
inlet
{
type fixedValue;
value uniform (100 0 0);
}
... there are other patch entries here
procBoundary0to1 // this is what I tried to add (for each processor to processor connection)
{
type processor;
}
}

The error I get when I do this, however, is even more complicated and unintelligible. I feel like I am missing something simple. Is there a file or dictionary entry missing somewhere that is required for a rhoCentralFoam parallel run?

Thanks,

Henry

[hbrist7]

Sometimes we miss stupid things: this is solved with a simple

"#include $WM_PROJECT_DIR/etc/caseDicts/setConstraintTypes"

statement in each of the 0/* files.

[Alhad]

The patch that you entered is the correct fix.
Except that you put in 'procBoundary0to1' instead of 'procBoundary0to3'.


Just add the following to your p file:


procBoundary0to3
{
type processor;
value uniform 0;
}




If the error occurs for u or k the text against the 'value' string will need to be different.

[arezayan87]

Hi everyone

I'm inexperienced to Parallel run in OF. I follow these commands:

1- blockMesh
2- surfaceFeatureExtract
3- decomposePar (with scotch method)
4- foamJob -pararllel -screen snappyHexMesh -overwrite
5- reconstructParMesh
6- foamJob -pararllel simpleFoam

in this stage I keep getting this error: ( this is part of the error and I've attached the complete log.txt file)

[0] --> FOAM FATAL IO ERROR: (openfoam-2312)
[0] Cannot find patchField entry for buildings
[0] 
[0] file: processor0/0/p/boundaryField at line 27 to 83.
[0] 
[0]     From void Foam::GeometricBoundaryField<Type, PatchField, GeoMesh>::readField(const Foam::DimensionedField<TypeR, GeoMesh>&, const Foam::dictionary&) [with Type = double; PatchField = Foam::fvPatchField; GeoMesh = Foam::volMesh]
[0]     in file ./src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 330.

the "buildings" boundary is that one, which is generated with snppyHexMesh.
I dont know how to get rode pf this error!!

[Yann]

Hello,

Check these posts and see if it helps to find the issue.

"Cannot find patchField entry for allBoundary" - when setting two inlets in interFoam
Cannot find patchField entry for motorBike

Regards,
Yann

[arezayan87]

Originally Posted by Yann

Hello,

Check these posts and see if it helps to find the issue.

"Cannot find patchField entry for allBoundary" - when setting two inlets in interFoam
Cannot find patchField entry for motorBike

Regards,
Yann

Thanks Dear Yann

I saw the posts and they were useful, the question is why this is happening? it's not reasonable to change 0 folder foe each processor before parallel running. what's your idea?

[Yann]

It is happening because decomposePar decomposes only the patches existing in the mesh.

When meshing in parallel, you decompose the initial mesh created with blockMesh, so the patches related to the geometry do not exist yet (as it will be created by snappy) and decomposePar removes it from the 0 directory.

You can avoid it using decomposePar with the -copyZero option, it will just copy the 0 directory into the processors directories without altering the files.
If you do so, you will need to have this line defined in all the files files in 0 directory:

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    // Your own boundary conditions setup here
}

Regards
Yann