Spindle not switching on with 4th Axis

[suntravel]

Use the Centroid mill PP from swissi, that runs perfectly right after posting.

Uwe

[Ashsrdtuning]

I just found this like 2 mins ago ive got no idea how to instal it on fuson 360 any advice on how to use the post from swissi in fuson ?

[cnckeith]

why not use Intercon for this type of simple parts? as Intercon will create perfect Centroid G code.

[cnckeith]

i changed all the "(" in the program to ; and the program runs

[Ashsrdtuning]

Keith why do u think it has issues with the ( and not ; im new to g-code.

So did u have the same fault as me when u try to run it ??

Just making sure its not a problem with my acorn bord
Lol

Ash

[centroid467]

Centroid G Code processor accepts ; and : as comments. Using ( ) for comments is not supported. I would expect that to cause some problems when trying to run with a Centroid control.

[tblough]

Different machine tool vendors use different variations of G-code on their machines. Oftentimes this is to accommodate specific functionality and other times it is for simple things like what character denotes a comment within the g-code.

Fanuc and Haas uses parentheses. Centroid, Siemens, Heidenhain and others use semicolons.

Chapters 11, 12, and 13 in the user's manual cover the valid g-code for Centroid controls.

[cncsnw]

Centroid G Code processor accepts ; and : as comments. Using ( ) for comments is not supported. I would expect that to cause some problems when trying to run with a Centroid control.

As usual, the reality is a bit more nuanced.

In most situations, with current software and typical CNC programs, comments in ( ) should work just fine.

On a line by themselves, comments in parentheses have been supported since sometime back in the CNC7 years (late 1990's).
As a line-end comment following other G codes, comments in parentheses have been supported since sometime in the CNC10 era (early 2000's).
As a line-end comment following a variable assignment, comments in parentheses are not supported, because parentheses are considered to be part of a numeric expression.

Code: Select all

(no problem here)
G1 X1 (no problem here either)
#101 = 1.234 (this is a problem)
#101 = 1.234 ; but this is okay

[cncsnw]

For what it's worth, I was able to graph the program Ashsrdtuning posted here, without error, with no modifications.

But then, he was not reporting parse error problems. He was reporting PLC I/O problems or spindle drive problems, wherein his spindle would only start once. That is going to require a deeper dive into his PLC program and macros (but maybe first a simple check of the Alt-i display to see whether the spindle-run-forward output is in fact turning green on the subsequent spindle start request).

One thing that is slightly odd about the posted program, is that there are no M5 spindle-off commands prior to the subsequent tool changes. It relies on the M6 tool-change operation to turn the spindle off (which generally works just fine). But perhaps his PLC or macro logic depends on an M5 to perform some type of reset, without which subsequent M3 requests are ignored.

Try editing the program to include M5 on a line before every M6, and see if it works better that way.

[Ashsrdtuning]

All fixed after changing over to swissi post P so very happy thank u bud works perfect now

was a very glitchy problem as the PLC/i0 went down if i run the old Fuson 360 Centroid PP with the 4th Axis

many thanks all

Ash