What's new
What's new

HURCO G76 Boring Cycle

Sam I

Aluminum
Joined
Nov 6, 2020
Hi Guys,

Scratching my head on this one.

I've got a 2018 VM10i and I'm using a boring head in the machine. I'm programming in Fusion 360 and know the code may need a little alteration so I post just the boring op to verify the code. I change the Q value to an I-1. due to the orientation of my boring head in the machine. I run the program above the part as an actual program with a Z offset (not dry run as it doesn't do the shift so can't verify). Works perfectly. I go back to Fusion, post the full program, change the Q value to I-1. as before but this time after boring it stops and orients the spindle as it should but then it moves in Y by approx -35. mm and x 1. mm. Deedless to say the boring bar is now toast.

Thing is, I've compared the code and it appears to be identical. So does anyone have any suggestions? I can't help but think there's probably something really simple I'm missing here.
I've verified the same plane G17 for both ops, both in absolute G90, both in mm G21

Proven good code:

N1 G90 G17
N2 G21
N3 M59
N4 G53 X0. Y0.
(Drill2)
N5 T8100 M6
N6 S1447 M3
N7 G54
N8 M8
N9 G0 X17.5 Y-20.
N10 Z55. H8100
N11 Z45.
N12 G98 G76 X17.5 Y-20. Z6.5 R44. P0. I-1. F115.7
N13 G80
N14 X167.5 Z45.
N15 G76 X167.5 Y-20. Z11.5 R39. P0. I-1. F115.7
N16 G80
N17 Z55.

Code in the program that's giving me unexpected X and Y moves:

N21709 T8100 M6
N21710 T4005
N21711 S1447 M3
N21712 G54
N21713 M8
N21714 G0 X17.5 Y-20.
N21715 Z55. H8100
N21716 Z45.
N21717 G98 G76 X17.5 Y-20. Z6.5 R44. P0. I-1. F115.7
N21718 G80
N21719 X167.5 Z45.
N21720 G76 X167.5 Y-20. Z11.5 R39. P0. I-1. F115.7
N21721 G80
N21722 Z55.
 
A little update if anyone is interested.

Spoke to HURCO applications and couldn't get to the bottom of it. As a workaround if I add a J0. to the line it behaves as expected. After a few hours of troubleshooting we identified that something in the program above is causing the offset - if I block out the prior program in the editor then run it behaves as expected. Just not sure what yet - would be interested if anyone has any thoughts.

They're going to run it on their machines tomorrow and see if they can recreate it their end and try to work out the cause.
 
Is this actually a Hurco post? It looks like a mangled Fanuc post... Fusion has Hurco posts already?

Clues are the prestaging and the incorrect H offset calls, which are unnecessary on Hurco.

My proven Hurco post puts both I and J in a G76 line, even if one of them is zero.

Edit: You updated while I was typing :)

Anyhow, here is output from my proven post for you to compare against:
%
( G76 TEST )
( SETUP1 )
( 6-11-2024 )

G00G17G40G49G80G21
G91G28Z0
G90
G5.3P50

( BORE HOLE1 )
( ADJUSTABLE_BH_M50 )
G54G0X0.Y0.T1M6
M01
M68
G0X100.0Y100.0
S194M3
Z25.0M8
Z3.0
G76R3.0Z-25.0I0.J-0.25F19.71
G80
Z25.0
X200.0
Z3.0
G76R3.0Z-25.0I0.J-0.25F19.71
G80
Z25.0
M9M5

G91G28Z0
G90
G49
M30
%
 
Thanks for the input.

It's a modified version of the official Fusion post for HURCO machines. I was dealing with Fusions post writing guys and they made the post which I believe is now readily available (although I'm not sure if all the tweaks made it to the standard one - I think a few of them were semi machine specific). The stock one was pretty terrible and I have a feeling it was borrowed from elsewhere and modified to suit. The original ran fine for 3 axis but 4 axis was a headache. It runs fine though (although you have to check a few boxes to disable a few options when posting the program so the machine ignores the incorrect tool height offsets) and I've been using it for around 18 months now without any issues (until today).

Interestingly my post doesn't support the use of I and J values, only a Q value which in this instance wouldn't work due to the orientation of the bar. I think this could be a limitation within Fusion as they don't have anywhere to input separate X and Y moves, only a single retract amount which is then posted as a Q value. There is an option within fusion to orient the spindle by a specified amount however the post doesn't support this - not sure if the machine does or not.
 








 
Back
Top