Cutter comp w/ Helix Bore

[Guyinthedesert]

I've used Helix bore quite often, but I don't recall ever having this problem before. When I use Helix Bore, I select perpendicular entry and the comp turns on fine, just like in threadmill. But when I post it, it puts the G40 on the last Arc move, which generates an error on the control. My control def is set to not allow comps on arc moves. I tried reposting using MPFAN, outputs like this:

 

N120 T5 M6

N130 G0 G90 G54 X-1.4047 Y0. A0. S9000 M3

N140 G43 H5 Z4. M8

N150 Z2.725

N160 G1 Z2.625 F20.

N170 G41 D5 X-1.354 F60.

N180 G3 X-1.4555 I-.0507 J0.

N190 Z2.575 I.1015 J0.

N200 Z2.525 I.1015 J0.

N210 Z2.475 I.1015 J0.

N220 Z2.425 I.1015 J0.

N230 Z2.375 I.1015 J0.

N240 Z2.325 I.1015 J0.

N250 Z2.275 I.1015 J0.

N260 Z2.225 I.1015 J0.

N270 Z2.175 I.1015 J0.

N280 Z2.125 I.1015 J0.

N290 Z2.075 I.1015 J0.

N300 Z2.025 I.1015 J0.

N310 X-1.2525 Z2. I.1015 J0.

N320 I-.1015 J0.

N330 G40 X-1.354 I-.0508 J0.

N340 G0 Z4.

N350 M5

N360 G91 G28 Z0. M9

 

 

 

I don't see any option for adding an Exit move. Any ideas?

[gcode]

what version are you running.

 

I think X5 introduced a bug in helix bore.. that was fixed in X5 MU1

[Guyinthedesert]

what version are you running.

 

I think X5 introduced a bug in helix bore.. that was fixed in X5 MU1

 

I'm running X5 MU1

 

I tried it with different posts, same result. I couldn't find anything in the post relative to comps on arcs.

I was just going to switch to using a threadmill cycle, with the direction from top to bottom. It's almost the same, only the treadmill cycle doesn't make a full pass at the bottom depth. I could always add that in by hand, but that's something I'm trying to avoid.

[gcode]

I use helix bore with cutter comp daily with no problem, but I don't use perpendicular entry.

I check the start at center box, set the entry arc to 90 degrees and always get good code.

[NOTW Programmer]

Could breaking the arcs get you an extra line where the G40 does work, can you set the control to allow Comp to be turned off on arc ? I also use it daily without any problems, both perpendicular and at 90deg. Could be a bug in your post also.

[Guest CNC Apps Guy 1]

I check the start at center box, set the entry arc to 90 degrees and always get good code.

 

 

As do I and I have no issues. I use derivitaves of MPMaster for posts.

 

 

[Guyinthedesert]

Many thanks to all. Unchecking perpendicular entry box moves the G40 from the last arc move to AFTER the retract move. I'll have to mess around with it, I don't know if the placement of the G40 is a post issue? I want the G40 on the last linear move, same as with threadmill. But this eliminates the control error.

 

Thanks

[Guyinthedesert]

Many thanks to all. Unchecking perpendicular entry box moves the G40 from the last arc move to AFTER the retract move. I'll have to mess around with it, I don't know if the placement of the G40 is a post issue? I want the G40 on the last linear move, same as with threadmill. But this eliminates the control error.

 

Thanks

 

No wait!! I looked at the wrong post, it did indeed put the G40 on the exit linear move. Great!!