2019 linking settings

[So not a Guru]

Why is my toolpath not raising to the 3" clearance between passes?

[JParis]

Keep tool down on?

[So not a Guru]

Just now, JParis said:

Keep tool down on?

Nope.

[So not a Guru]

I know I can fix it by unchecking Retract, but I'm wanting to know if this is a bug I need to report. Not that CNC will fix an ancient version like 2019, but ...

[RLeuschen]

I'm kind of interested in this, running mc2021 for c/y axis lathe. I Just had my cross drilling cycles ignore the clearance value (tried both ways with 'use clearance only at start and stop of cycle') and it wants to start the cycle from my ref points position. I don't remember this behavior in mc2018.

[jeff]

1 hour ago, So not a Guru said:

I know I can fix it by unchecking Retract,

I've seen this too many times to count, even in v2020. The only fix that I've seen is either uncheck Retract or make Retract the same height as Clearance. 

[JoshC]

56 minutes ago, RLeuschen said:

I'm kind of interested in this, running mc2021 for c/y axis lathe. I Just had my cross drilling cycles ignore the clearance value (tried both ways with 'use clearance only at start and stop of cycle') and it wants to start the cycle from my ref points position. I don't remember this behavior in mc2018.

maybe just a display issue? You should see a G98 or G99 in the g-code, if you are seeing a G98 then your machine should retract to the first Z value prior to the drill cycle, my guess is it will still post correct and perhaps its just a problem with the way backplot is showing?

[RLeuschen]

Josh,

Thanks for that info. But the issue seems to be with putting any value in the 'ref points - approach/retract values' that have to do with a rapid to x value.

If any value is is x rapid, the g98 value is referenced from the rapid to point and not the clearance values placed in the linking parameters.

I'm starting to think maybe something got upset in the post from having it converted over from 2018 to 2021..

See below: 2 examples:

below with rapid values:

T1010
G19 G98
M28
M8
M39
G0 G28 H0.0 (FORCE C HOME)
G0 C90.
G0 X5. Z1.  (rapid points of x5. y0 z 1. )
Y0.
G97 S2500 M103
G87 X-.05 Y0. Z-.7316 C90. R-.0625 Q25 P1250 F.5 M38

(this would be referenced from the X5 value..meaning it would clearance to x4.875 not the .625 as set in clearance values of the cycle)

G80
X5.
Z1.
M9
M39
G28 U0 V0
G30 W0. H0. M105

 

below with out x rapids:

T1010
G19 G98
M28
M8
M39
G0 G28 H0.0 (FORCE C HOME)
G0 C90.
G0 X.75 Z1.  (no x rapid points, only y and z)
Y0.
G97 S2500 M103
G87 X-.05 Y0. Z-.7316 C90. R-.0625 Q25 P1250 F.5 M38

(this would be referenced from the X.75 value..meaning it would clearance to x.625 as it is in the linking parameters)

G80
X.75 Z1.
M9
M39
G28 U0 V0
G30 W0. H0. M105
T1000

 

 

thanks,

Rob