CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM

running rhoCentralFoam in parallel: cannot find patchField entry for procBoundary

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Yann

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 3, 2016, 13:45
Default running rhoCentralFoam in parallel: cannot find patchField entry for procBoundary
  #1
New Member
 
Henry
Join Date: May 2016
Posts: 15
Rep Power: 10
hbrist7 is on a distinguished road
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 is offline   Reply With Quote

Old   June 29, 2016, 11:09
Default Solved
  #2
New Member
 
Henry
Join Date: May 2016
Posts: 15
Rep Power: 10
hbrist7 is on a distinguished road
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.
hbrist7 is offline   Reply With Quote

Old   December 7, 2020, 11:30
Default
  #3
New Member
 
Join Date: Dec 2020
Posts: 1
Rep Power: 0
Alhad is on a distinguished road
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.
Alhad is offline   Reply With Quote

Old   March 27, 2024, 02:39
Default need help for "Cannot find patchField entry for . . ."
  #4
New Member
 
Amirreza
Join Date: Mar 2020
Posts: 17
Rep Power: 6
arezayan87 is on a distinguished road
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)

Code:
[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!!
Attached Files
File Type: txt log.txt (10.3 KB, 1 views)
arezayan87 is offline   Reply With Quote

Old   March 27, 2024, 04:02
Default
  #5
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,193
Rep Power: 27
Yann will become famous soon enough
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
Yann is offline   Reply With Quote

Old   March 27, 2024, 05:59
Default
  #6
New Member
 
Amirreza
Join Date: Mar 2020
Posts: 17
Rep Power: 6
arezayan87 is on a distinguished road
Quote:
Originally Posted by Yann View Post

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?
arezayan87 is offline   Reply With Quote

Old   March 27, 2024, 07:11
Default
  #7
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,193
Rep Power: 27
Yann will become famous soon enough
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:

Code:
boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    // Your own boundary conditions setup here
}
Regards
Yann
arezayan87 likes this.
Yann is offline   Reply With Quote

Reply

Tags
parallel compressible, parallel error, patchfield, processor boundary, rhocentralfoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ANSYS Meshing] Help with element size sandri_92 ANSYS Meshing & Geometry 14 November 14, 2018 08:54
fluent divergence for no reason sufjanst FLUENT 2 March 23, 2016 17:08
Parallel Running With Problems guilha OpenFOAM Running, Solving & CFD 1 July 26, 2014 11:55
multiphase solver - parallel processing - GAMG thibault_pringuey OpenFOAM Programming & Development 2 August 27, 2013 23:03
[solidMechanics] Running contactStressFoam in Parallel Hisham OpenFOAM CC Toolkits for Fluid-Structure Interaction 2 October 16, 2012 11:34


All times are GMT -4. The time now is 18:00.