Probe for corner

Thanks John. I set the retract to an absurdly large value like .25, and I get the same result FWIW, the hysteresis on the probe is visually imperceptible to me.

John, not 100% sure. I guess I should print it out and try stepping through it one thing at a time.

Where would I look to see what those variables' values (e.g. #5070) are? There's an emc.var file in my machine directory, but it doesn't have any lines for values under 5161 or something like that.

FWIW I tried the center probing routine that was posted earlier in this forum, and that worked fine....

Hello,

Where would I look to see what those variables' values (e.g. #5070) are?

Take a look here ...
linuxcnc.org/docs/html/gcode/gcode.html#sec:G38-probe

Try increasing the
#<Probepause> = #17 (=.05 pause) ; Probe pause, amount of time to pause between probe moves to wait for probe to settle/ stop bouncing
also try reducing
#<Fastprobe> = #1 (=10 Fast prb) ; Fast probe speed
#<Slowprobe> = #2 (=5 Slow prb) ; Slow probe speed

It looks like an early version is posted but this may help...

#<Fastprobe> = #1 (=10 Fast prb) ; Fast probe speed
#<Slowprobe> = #2 (=5 Slow prb) ; Slow probe speed
#<Probedist> = #3 (=.50 Prb dis) ; Probe distance
#<Retract> = #4 (=.050 Prb ret) ; Probe retract distance
#<Diam> = #5 (=.117 Prb Diam) ; Probe diameter
#<Xcord> = #6 (=.25 X Pcord) ; future ignore
#<Ycord> = #7 (=.25 Y Pcord) ; future ignore
#<Xcorr> = #8 (=0.00 X cor) ; correction to X coordinate to fine tune result
#<Ycorr> = #9 (=0.00 Y cor) ; correction to Y coordinate to fine tune result
#<Zcorr> = #10 (=0.00 Z cor) ; correction to Z coordinate to fine tune result
#<Ymax> = #11 (=1.00 Y Smax) ; maximum distance to search for Y
#<Yinc> = #12 (=.125 Y S inc) ; size of step to search in Y
#<Xfin> = #13 (=0.00 X fin) ; X Location to go to when finished
#<Yfin> = #14 (=0.00 Y fin) ; Y Location to go to when finished
#<Zfin> = #15 (=.125 Z fin) ; Z Location to go to when finished
#<Zsafe> = #16 (=.250 Z Safe) ; Safe Z travel location
#<Probepause> = #17 (=.05 pause) ; Probe pause, amount of time to pause between probe moves to wait for probe to settle

Rick G

G38.5 F#1 Y-.010 (retract till probe clears)
G4 P#17
G38.3 F#1 Y[0 - #4] (retract to set up for slow probe)
G4 P#17
O103 IF [#5070 gt 0]
(MSG, Probe not complete unexpected Y hit on retract)
G90
M2
O103 ENDIF
If this is where you are having a problem it is possible that the probe is bouncing on and off on the retract steps.
A slower speed may help or you could try to retract with a G1 move instead. The G38.5 and G38.3 retract moves are for safety and information if there is an unexpected contact or the probe sticks.
You could also try changing the Y-.010 to Y -.025.

Rick G

Thanks. I tried changing the delay but it had no effect. I think the G38.5 was the problem. By the time I was done I ended up writing my own version of this using G1 moves and it seems to be working well. IIRC, LinuxCNC errors if the probe is tripped during a G1 move, or is that only when the G1 is issued from the MDI? I haven't tried tripping it during a programmed G1 move.

As John said a G1 move should trigger an error with Linuxcnc, however if you normally work in G90 absolute distance mode and the routine is working in G91incremental distance mode you may be left in the G91 mode on error.
G38.5 is to retract the probe from the contact to non contact, if the probe sticks on or bounces back on the move should fail.
IIRC G38.3 will not work if you issue it when the probe is already in contact.
The idea of the two step approach is again for safety, let you know where the problem is and return you to the mode you would normally work in.

Rick G