[cyln]

Hello,

I am working with transient simulations (large in size). While I am reconstructing data using reconstructPar, simultaneously I would like the decomposed data to be deleted.


Is this possible in OpenFOAM?


Cheers

[ed_bar]

I'm unsure if there is an utility available for that, however you could write a bash script to do it. If you are really short on space and need to remove each time step at every reconstruction, then you would probably need to write a loop with (this is not correct bash, but gives the idea).

for timeName in processor0/ ignoring directory uniform do

reconstructPar -time $timeName
rm -rf processor*/$timeName
done

Otherwise reconstruct the fields and then delete the processor directories afterwards.

reconstructPar ; rm -rf process*

[cyln]

Thanks Ed. I am already deleting the corresponding files in processor directories after reconstruction while the simulation is still running (I am not deleting the processor directories since the simulation has to continue). I do it using the second way you described.

For now, I will keep using the second way since I do not have a good command of C++. But if anyone has another suggestion, please let me know.


Cheers

[Bodo1993]

Hi,
I am wondering if you figured out a better way.
I want this because I have a limitation on the number of files that I can write on the allocated space in clusters.
I would appreciate any assistance.
Thanks!

[JBeilke]

Here is my Perl6/Raku code to delete all but the last time directories from the processor dirs.

#!/usr/bin/env perl6

use v6;

shell 'reconstructPar -newTimes';    
    
my @processor_dirs = dir( test => /:i ^ 'processor' \d+ / ).grep({ $_.IO.d }).sort;
my @time_dirs;

for @processor_dirs -> $processor_dir {

    chdir $processor_dir;

    once {
        @time_dirs = dir( test => /^ \d+ \.* / ).sort({ $^a <=> $^b });
        @time_dirs.pop;
    }    

    for @time_dirs {
        say "Removing: " , $processor_dir.Str , "/" ,  $_.Str;
        shell "rm -rf $_";
    }

    chdir "..";

}

[sharonyue]

You can use the following:

#!/bin/bash
for i in $(foamListTimes -case processor0); do
    reconstructPar -time ${i}
    rm -r processo*/${i}    
done

[missios]

Hi,


Have you considered setting

purgeWrite 1;

in your control dict?


Best

K

[missios]

Originally Posted by Bodo1993

Hi,
I am wondering if you figured out a better way.
I want this because I have a limitation on the number of files that I can write on the allocated space in clusters.
I would appreciate any assistance.
Thanks!

Hi,



there is a new option (introduced back in v1712) when running in parallel mode. It is called collated and reduces significantly the number of output files. What it doed in escence is that it collects the output in one master file. More info regarding that can be found here https://www.openfoam.com/news/main-n...v1712/parallel .



Watch out since this choice can affect the computational performance (see here https://www.archer2.ac.uk/training/c...4-openfoam-io/ ).



Best,

K

[JBeilke]

Originally Posted by missios

Hi,


Have you considered setting

purgeWrite 1;

in your control dict?


Best

K

But purge write just deletes the time directories without a reconstructPar before.

[Mahmoud Abbaszadeh]

I have the same problem. I use "decomposePar" first and then run snappyHexMesh in parallel. After that, I use recontructMeshPar and I would like to delete the old decomposed directories before running my simulation. Has anyone had the solution for it?