From pic 1, it looks like
WCS Z-3 = MCS Z-5
By commanding WCS Z5 you want to move 8mm higher from current position which would be MCS Z3.
MCS Z can only be <=0 . In your case, according to your $132, your working Z range is from Z0 to Z-70 (MCS) and your code wants to go to Z5. This is out of range and triggers the out of range alarm (alarm 2).
(all numbers rounded for simplicity)
Two more comments.
comment #1 (optimization)
Why do you G38.2, then G.38.4, then G38.2 again (at the same feed f60)?
If you want to double probe, with the second time being slower try something along these lines:
M5 (spindle stop)
G91 (incremental mode)
G38.2 Z-20 F30 (probe down by -20 at 30 feed)
G0 Z1 (go up by 1)
G38.2 Z-2 F10 (probe again slower)
G10L20P1Z19.3 (set current Z to pluck height, which means pluck bottom is set to 0)
G0 Z5 (move up by 5)
G90 (absolute mode)
M0 (pause)
comment #2 (probable culprit for alarm 2)
Why do you
g10l20p1z-21.089
? Why minus? Donât you want the bottom of your pluck to be Z0? If yes, and your pluck height is 21.089 then
g10l20p1z21.089
YupâŚthereâs the issue. Youâre setting your new zero at 21.089 ABOVE your probe after the tool change.
I donât use bCNC much, but I would guess that when you âcalibratedâ that tool change offset, you had not previously set your work zero. That value should be the probeâs Z location in your current WORK coordinate system. I think if you set that correctly, you should be fine.
I also agree with @EliasPolitisâs other comments with the tool change macro. Iâm not sure where that is setup in bCNCâŚI typically use CNCjs.
As someone pretty new to this i cant thank you both enough, i have sorted this issue out and couldnât be happier with the results.
Keep being great people and thanks for the replyâs! =)
