bCNC - help - support - FAQ

X-Carve Upgrades
42

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)

1 Like
43

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? Donā€™t you want the bottom of your pluck to be Z0? If yes, and your pluck height is 21.089 then

g10l20p1z21.089

1 Like
44

Yupā€¦thereā€™s the issue. Youā€™re setting your new zero at 21.089 ABOVE your probe after the tool change.

I donā€™t use bCNC much, but I would guess that when you ā€œcalibratedā€ that tool change offset, you had not previously set your work zero. That value should be the probeā€™s Z location in your current WORK coordinate system. I think if you set that correctly, you should be fine.
I also agree with @EliasPolitisā€™s other comments with the tool change macro. Iā€™m not sure where that is setup in bCNCā€¦I typically use CNCjs.

45

As someone pretty new to this i cant thank you both enough, i have sorted this issue out and couldnā€™t be happier with the results.
Keep being great people and thanks for the replyā€™s! =)

2 Likes