switching between 3 & 4 axis modes

[CRM]

I have recently gotten my 4th axis Hardinge 5C indexer functioning on my Prototrak DPM mill. Everything homes fine...when the indexer is hooked up. But that isn't always going to be the case. I have an Amphenol plug installed in the Centroid electronics cabinet matching the cable from the indexer so I am able to remove the indexer and store it elsewhere when I'm doing 3 axis work.
Now, it's been about a year since I started the physical installation of the 4th axis drive and wiring, and at the time I asked how Centroid would handle an axis that is not always part of the system and I thought I remember saying by changing a particular parameter, a button would appear on the setup screen to toggle to toggle between 3 & 4 axes. That all works, displaying and removing the 4th (A axis) DRO. I was under the impression that it also would then ignore the homing commands for the 4th axis in the home file. I just tried homing for the first time with the indexer disconnected (and set to 3 axis mode in the setup screen) but I get an "invalid parameter" alarm in line M106/A P7F3000. of the cncm.hom file:
M109/1/2
M92/Z
M26/Z
M91/X
M26/X
M92/Y
M26/Y
M106/A P7F3000.
M92/A
M26/A
M108/1/2

Because I'm running CNC11, there is no "home jog speed" parameter in the motor parameters tab, so the M106 line is there to speed the jog speed up to get close to the home switch.
On a hunch, I edited the home file and deleted that line...and it now homes fine in 3 axis mode. (But super slow for the A axis if it is active) So apparently the toggle for 3/4 axis causes the controller to recognize and ignore the M92 & M26 codes for a disabled axis... but only for those two particular M codes. Is that correct? Any options to work around this short of buying an upgrade license to CNC12, which if I understand correctly allows you to specify homing feedrates for each individual axis?

[cncsnw]

When you use the features associated with Parameter 131 to switch between 3-axis and 4-axis mode, CNC12 does silently ignore the 4th-axis homing commands ("M92/A" and "M26/A"). Unfortunately, that exemption does not extend to all other uses of the 'A' axis.

You could make your other A command(s) conditional on the axis label. CNC system variable #20104 holds the ASCII code for the fourth axis label, which would be 65 for 'A'.

So:

Code: Select all

IF [#20104==65] THEN M106/A P7 f3000

would only run the M106 command if the 4th axis label was 'A'.