PostProcessor or ISO a script to insert M0 for "Z" (Linuxcnc & BobCad v23)

Many thanks for any help.

I am using (I have a dongle, for convenience) BobCad v23 (it is what it is) and would like to have a pause for change in "Z", this is manually set, on a mill. I have read about "creating a script" and a few other links below, and copied a "EMC2" post processor to the correct place in the bobcad file location (and can select this option, in the list with other postprocessor inside Bobcad), but still not complete.

Any suggested reading or other links. Suggestions would be warmly welcomed. If I have not understood the issue please clue me in. I have read about line 26 set to debug "on", when trying to test/debug posts.

My hope it should be possible to create a script that could automatically insert an M0 code to pause the machine where ever there is a change in Z depth.

(how to modify Bobcad postprocessor)

bash.cyberciti.biz/guide/Hello,_World!_Tutorial (To create a shell script)

Many, many Thanks!

I'm not totally sure but I think that you may be able to just open up your gcode file in a text editor, not a word processor, and do a "search and replace" of the Z lines and replace with M0. You would have to do it for each file but if it works it would only take seconds.

andypugh, many thanks, you for the advise!

I have read the link several times is it possible to have something to start with, like a pattern or do I use the example from the link?

This is from the link:
"" #! /usr/bin/env python

import sys

def main(argv):

openfile = open(argv[0], 'r')
file_in = openfile.readlines()
openfile.close()

file_out = []
for line in file_in:
# print line
if line.find('Z') != -1:
words = line.rstrip('\n')
words = words.split(' ')
newword = ''
for i in words:
if i[0] == 'Z':
newword = 'W'+ i[1:]
if len(newword) > 0:
words.append(newword)
newline = ' '.join(words)
file_out.append(newline)
else:
file_out.append(line)
for item in file_out:
print "%s" % item

if __name__ == "__main__":
main(sys.argv[1:]) ""

I have been reviewing some linuxcnc examples like the "nc_files/holecircle.py" (a python script MIME .type of file) and others like the "Skeleton.ngc". The python code was in several colors, is that from the type of file it is or the way it was written? The hal file has the "png=image-to-gcode" plus several other lines under the [FILTER] area of the file, close to the top of page.
As per Bobcad suffix it is a .MILLPST post processor type of file.

many thank, all comments suggestions are warmly welcomed.

The colors are from the text editor that was used to view it. (Some have filters geared towards programming languages.)

I have a bash script that uses sed to automatically convert ordinary XYZ g-code to XYZW code on loading for a two headed carving machine. (It also inserts a pre- and post- amble.)

Todd,Thanks, so good to here from you!

I have my sheet of g code commands and see how they reflect to the "x,y,z" like g53 (just an example). Am I looking for the bash script, to understand your "echo" or "sed" part? I am looking at bash script now, any other suggested reading?

many thanks

The echo lines are just inserted at the beginning or end of the file.

The sed line does all the work. finding all of the Z commands and adding an identical W command after it.
I have to be honest I did not write that miraculous line of sed code. Someone else here on the list wrote it for me.

But I have since used some other sed scripts to convert code made for one machine to run on another.
Here is a good tutorial.
www.grymoire.com/Unix/Sed.html

The s in the sed line designates a search and replace, what is between the 1st two pipes (|) is what is searched for, between the 2nd and 3rd pipe is what is replaced back. The parenthesis designates a varialbe in this case a string how ever long of containing 0-9, . and -. The /1 means to insert 1st variable string that was found. The little g at the end designates that it is a global command.

Save the script as a filename.sh and put it in the path called in your ini file.

The script above I have set up to be automatically ran on any file I open with Linuxcnc with the extention ngczw.

A sed script for your purpose might look something like this

Many Thanks for all the great advise!

I have read many parts of the of (www.grymoire.com/Unix/Sed.html) link, thank you Todd! As a complete newbie to "scripts" I am offering my very 1st effort. All constructive comments warmly welcomed.

[FILTER]
PROGRAM_EXTENSION = .png,.gif,.jpg Greyscale Depth Image
PROGRAM_EXTENSION = .py Python Script
png = image-to-gcode
gif = image-to-gcode
jpg = image-to-gcode
py = python

###################################################
#!/bin/bash

echo "G92.1 G54 G49"
echo "M111"
echo "G53 G0 Z0 W0"
echo "G90"
echo "G64 P0.005"
echo "F80"
echo "M3 S18000"
echo

# The main part
sed 's|\(.*\)Z\([-,0-9,\.]*\)|M0 \1(Z\2)|g' "$1"

echo
echo "G53 G0 Z0 W0"
echo "G53 G0 X0 Y65"
echo "G49 G92.1"
echo "M5"
echo "M30"
echo "%"
#################################################

I tried this with the sample "g code" and all worked except the "z" did not pause. I have read there may need to be some permissions "granted" so the file is loaded. The very top part was in the .hal file all ready.

Many thanks!

Did you add the above to your ini file?

What you need to do is save the bash script as a file (file_name.sh). Save it in a good place (such as your machine's config folder)
After you've moved the file where it goes, in a file manager, right click on the script file, select properties, then permissions, and click the box for "Allow this file to run as a program".
Then in your ini file under the [FILTER] section add a line referencing it.
For example if your script is saved as "z-pause.sh" in your config dir and your config dir is called "my_mill" you would add this line to run the script on all files you open with Linuxcnc that end with the extension ".ngc"You can also control what files the script is ran on by the extension. Lets say you want all ngc files to be opened normally, but want all files with the extension ".ncz" to be opened using the script.
Make your [FILTER] section look like this.
Also, does your machine have an M111 custom m-code configured? If not you'll need to take that out.
And that particular script won't quite work on the default file that opens with Linuxcnc. The problem is that parameter values are used for the Z depth in many places, and those won't be replaced by that script.
But it should work fine for most "normal" files that just have a number for Z moves.