Add M1 codes for same tool

[ian1196]

At different tool changes an M1 is added and I like that.

In somewhere like "Edit Notes"

I would like to add.. say

G0 Z5

G0 Y12

M1

(Add bolts and press red button)

However, when I do that, I get

(M1)... etc.

Is "Edit notes"  the place for adding g code and if so, how does one get it to post without the brackets?

[seth.madore]

Simplest way would be to use Manual NC > Pass-Through 

And then just type your preferred set of code into the box that pops up. It will execute that line of code wherever you insert it.

[ian1196]

Seth,

I tried that earlier , I think, and now I tried it again,

Setup =>Manual NC+> Pass Through

On your behalf, I entered the following:

M1 (SETH)

I posted the code  (only "Manual NC1" ) and I got the following:

(Generated by DOUG )
(Saturday, March 02, 2019 11:15:57)
(O1001
G40 G80 G90 G94 G17
G20

M05
G00 Z400.
M02

It is not there...

[seth.madore]

What post processor are you using? It doesn't sound like it's configured properly for Pass Through NC code.

You "should" be able to use the Optional Stop pass through, but that won't do everything you want it to..

[ian1196]

I am using okumaDoug.cps a modified version of okuma.cps.

I went to Fusion360 and copied okuma.cps and added it to my OKUMA/okuma.cps so it would be the unmodified version in the event it was changed by me.

In the pass through box, I added the following:

S555

M4(SETH)

What I got from the processor was...

O1001
G40 G80 G90 G94 G17
G20

M05
G00 Z400.
M02

Please try it on your machine using OKUMA/okuma.cps

[ian1196]

I just tried several post processor codes on the Fusion360 list and have not seen the written code.

[ian1196]

I just saw on the web that there was a pass through bug a month or so ago. My fusion 360 was getting stupid about a week ago and I reinstalled it.

[ian1196]

I found a solution. There is a function snippet that is needed.

function onPassThrough(text) {
  var commands = String(text).split(",");
  for (text in commands) {
    writeBlock(commands[text]);
  }
}

[engineguy · Accepted solution]

@ian1196 

For what it`s worth I couldn`t get the comments to work as I liked, I wanted it after the M1 when the machine had stopped, spindle off, coolant off etc, etc.

They would output OK but right after the G28 G91 Z0 line, there is probably a way in the PP to move it but beyond my limited PP knowledge

So, a simple "workaround" does it for me, may not suit you or anyone else but it does output an operator instruction where I prefer it, after everything has stopped and right at the start of the next operation, what I did was simply type the operator instruction into the operations name, see sample code below, it is good enough for us for now

G0 Z10.
G28 G91 Z0.
G90
M5
M9
M1

(POCKET-1 FINISH CONTOUR - **! OPERATOR !** CHECK AND CHANGE CLAMPING)
T2 M6
(8MM FLAT END MILL-ALUZIP)
S3000 M3
G59
A0.
M8

Regards

Rob

[ian1196]

Great work around!