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

Missing pointProcAddressing

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

Like Tree3Likes
  • 1 Post By quarkz
  • 1 Post By quarkz
  • 1 Post By Amosx

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 23, 2021, 04:58
Unhappy Missing pointProcAddressing
  #1
New Member
 
Join Date: Mar 2021
Posts: 11
Rep Power: 5
Rebeca is on a distinguished road
Hi everyone!

I'm trying to run the rhoSimpleFoam/gasMixing/injectorPipe tutotial's case with little lucky.

After solving the case, I haven't been able to see the results. If I use the command "reconstructPar", the next error appears:

Code:
--> FOAM FATAL ERROR: (openfoam-2012)
cannot find file "/media/sf_OpenFoam/run/tutorials/compressible/rhoSimpleFoam/gasMixing/injectorPipe/processor0/constant/polyMesh/pointProcAddressing"

    From virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 547.

FOAM exiting
And If I try with "reconstructParMesh", it seems to do nothing:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2012                                  |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 79e353b8-20201222 OPENFOAM=2012
Arch   : "LSB;label=32;scalar=64"
Exec   : reconstructParMesh -mergeTol 1e-06
Date   : Apr 23 2021
Time   : 09:16:22
Host   : rebeca-VirtualBox
PID    : 16906
I/O    : uncollated
Case   : /media/sf_OpenFoam/run/tutorials/compressible/rhoSimpleFoam/gasMixing/injectorPipe
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
This is an experimental tool which tries to merge individual processor
meshes back into one master mesh. Use it if the original master mesh has
been deleted or if the processor meshes have been modified (topology change).
This tool will write the resulting mesh to a new time step and construct
xxxxProcAddressing files in the processor meshes so reconstructPar can be
used to regenerate the fields on the master mesh.

Not well tested & use at your own risk!

Merge tolerance : 1e-06
Write tolerance : 1e-06
Doing geometric matching on correct procBoundaries only.
This assumes a correct decomposition.
Found 8 processor directories

Reading database "injectorPipe/processor0"
sigWriteNow : Enabling writing upon signal 12
Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
Reading database "injectorPipe/processor1"
sigWriteNow : Enabling writing upon signal 12
Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
Reading database "injectorPipe/processor2"
sigWriteNow : Enabling writing upon signal 12
Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
Reading database "injectorPipe/processor3"
sigWriteNow : Enabling writing upon signal 12
Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
Reading database "injectorPipe/processor4"
sigWriteNow : Enabling writing upon signal 12
Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
Reading database "injectorPipe/processor5"
sigWriteNow : Enabling writing upon signal 12
Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
Reading database "injectorPipe/processor6"
sigWriteNow : Enabling writing upon signal 12
Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
Reading database "injectorPipe/processor7"
sigWriteNow : Enabling writing upon signal 12
Overriding OptimisationSwitches according to controlDict
    writeNowSignal  12;

sigWriteNow : Enabling writing upon signal 12
Time = 100

No mesh.

Time = 200

No mesh.

Time = 300

No mesh.

Time = 400

No mesh.

Time = 500

No mesh.

Time = 600

No mesh.

Time = 700

No mesh.

Time = 800

No mesh.

Time = 900

No mesh.

Time = 1000

No mesh.

Time = 1100

No mesh.

Time = 1200

No mesh.


End
I have been trying to solve this problems for days and I don't know what else to do.

I hope you can help me!

Thanks in advance,
Rebeca
Rebeca is offline   Reply With Quote

Old   December 25, 2021, 20:03
Default
  #2
New Member
 
Aps
Join Date: Oct 2013
Posts: 3
Rep Power: 13
apoorv121 is on a distinguished road
Hello Rebeca,

It seems like you have a processor*/constant/polyMesh folder structure. reconstructParMesh works when there is only polyMesh folder under each processor* folder. Once all the mesh is reconstructed then you can use the reconstructPar to get all the variable data in single file/time slot.

Also sometimes paraview crashes when loading this type of data. You can use foamToVTK to convert this data since each time folder might have a different mesh due to DyM refinement or topology changes.

Hope it works for you.
apoorv121 is offline   Reply With Quote

Old   March 27, 2023, 01:29
Default
  #3
Senior Member
 
TWB
Join Date: Mar 2009
Posts: 414
Rep Power: 19
quarkz is on a distinguished road
For me, I have got this error:

Create time



Reconstructing fields
region=region0



--> FOAM FATAL ERROR: (openfoam-2206)
cannot find file "/home//tsl/scratch/agile_flight/OpenFOAM/model_black_UAV_2.5e-5_5.59M_6dof_moi1_SST/processor0/2e-05/polyMesh/pointProcAddressing"

From virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::rea dStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 540.

FOAM exiting

Hence, I wrote a "of_copy_ProcAddressing_loop.sh" script:

Code:
#!/bin/bash
for ((i = 0; i < $1; i++ )); do
    echo "$i"
    cp processor$i/constant/polyMesh/*ProcAddressing processor$i/$2/polyMesh/
done
Usage:

of_copy_ProcAddressing_loop.sh a b

where:

a = no of processors
b = time saved

e.g.

of_copy_ProcAddressing_loop.sh a b 512 0.1

Hope it helps.
Adamwambert likes this.
quarkz is offline   Reply With Quote

Old   January 8, 2024, 16:28
Default
  #4
New Member
 
ZsoltDraga
Join Date: Jan 2011
Location: Albertirsa, Hungary
Posts: 10
Rep Power: 15
dragazsolt is on a distinguished road
Hi quarkz,



Iam have a same issue in case of AMI and Openfoam2306 and 2212.

I tried your scipt it does not work for me properly.

syntax :

sh of_copyProcAddressing_loop.sh 128 0.05

Error is bad for loop variables?

Do you have ideas to fix reconstructPar error?



Thanks,

Zsolt
dragazsolt is offline   Reply With Quote

Old   January 10, 2024, 09:53
Default
  #5
Senior Member
 
TWB
Join Date: Mar 2009
Posts: 414
Rep Power: 19
quarkz is on a distinguished road
Hi dragazsolt, there's no need for sh in front, just run it like:

./of_copy.sh 512 0.1 if the file is in the same dir.

hope it works.
deepakvil likes this.
quarkz is offline   Reply With Quote

Old   February 2, 2024, 02:30
Unhappy does anyone have solution for this problem
  #6
New Member
 
Amos
Join Date: Nov 2022
Posts: 2
Rep Power: 0
Amosx is on a distinguished road
hello everyone I'm facing the same problem, i managed to run the tutorial but i cannot view the results.
Amosx is offline   Reply With Quote

Old   February 2, 2024, 02:45
Default found how to view the results
  #7
New Member
 
Amos
Join Date: Nov 2022
Posts: 2
Rep Power: 0
Amosx is on a distinguished road
1. create a .foam file using touch command ex. touch case.foam
2.open case.foam using paraview
3.in paraview properties - case type change it to decomposed case.


thank you
Adamwambert likes this.
Amosx is offline   Reply With Quote

Old   July 29, 2024, 15:32
Default
  #8
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 539
Rep Power: 20
JBeilke is on a distinguished road
you have to run:


Code:
reconstructParMesh
reconstructPar
JBeilke is offline   Reply With Quote

Reply

Tags
error, injectorpipe, openfoam, pointprocaddressing

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
[OpenFOAM.org] RHEL 7.8 Issues installing ParaView - Third Party install not creating OpenMPI browny OpenFOAM Installation 2 April 24, 2021 06:18
[ANSYS Meshing] missing internal faces and uncovered faces after redifining parts containing surface. grv ANSYS Meshing & Geometry 2 December 9, 2016 05:38
what is syntax error : missing ')' before ';' aleisia Fluent UDF and Scheme Programming 8 March 10, 2015 16:42
[OpenFOAM] Xlib: extension "GLX" missing on display goldbeard ParaView 5 March 24, 2013 14:12
errors when installing openfoam2.1 on ubuntu12.o4 hewei OpenFOAM Installation 5 May 29, 2012 08:43


All times are GMT -4. The time now is 08:18.