[baldysm]

I am having a problem with a g-code program and it's driving me bonkers.

You run a graphic simulation, and the program runs through with no errors, everything looks fine. You run the program, the machine gets to line 440 and stops (just before it Z ups). No error messages, no warnings, nothing, just stops moving. What's really weird is that it does 2 pockets before this one that are basically the same and it runs through those fine.

Line 330 is basically the same thing, and runs through with no issues.

Code is below. I truncated it just for brevity.

Any ideas?

%
O1000


N100 G20
N110 G0 G17 G40 G49 G80 G90
( ROUGH AND FINISH THE POCKETS )
N120 T1 M6
N130 G0 G90 G56 X.6177 Y-.7875 A0. S8000 M3
N140 G43 H1 Z2.
N150 Z.1
N160 G1 Z-1.1436 F32.5
N170 G41 D1 Y-.3125
N180 G3 X.6172 Y-.312 I-.0005 J0.
N190 X.6167 Y-.3125 I0. J-.0005
N200 G1 Y-.7875
N210 G3 X.6172 Y-.788 I.0005 J0.
N220 G40 X.6177 Y-.7875 I0. J.0005
N230 G0 Z.8564
N240 Z2.
N250 X1.2603
N260 Z.1
N270 G1 Z-.8786
N280 G41 D1 Y-.3125
N290 G3 X1.2598 Y-.312 I-.0005 J0.
N300 X1.2593 Y-.3125 I0. J-.0005
N310 G1 Y-.7875
N320 G3 X1.2598 Y-.788 I.0005 J0.
N330 G40 X1.2603 Y-.7875 I0. J.0005
N340 G0 Z1.1214
N350 Z2.
N360 X1.9235
N370 Z.1
N380 G1 Z-.6704
N390 G41 D1 Y-.3125
N400 G3 X1.923 Y-.312 I-.0005 J0.
N410 X1.9225 Y-.3125 I0. J-.0005
N420 G1 Y-.7875
N430 G3 X1.923 Y-.788 I.0005 J0.
N440 G40 X1.9235 Y-.7875 I0. J.0005
N450 G0 Z1.3296
N460 Z2.
N470 X2.6022
N480 Z.1
N490 G1 Z-.5206
N500 G41 D1 Y-.3125
N510 G3 X2.6017 Y-.312 I-.0005 J0.
N520 X2.6012 Y-.3125 I0. J-.0005
N530 G1 Y-.7875
N540 G3 X2.6017 Y-.788 I.0005 J0.
N550 G40 X2.6022 Y-.7875 I0. J.0005
N560 G0 Z1.4794
N570 Z2.

[Machineit]

You can not start or stop Cutter Comp (g41, g42 or g40) in a circular move. Must be in a straight line move. Lucky it gets that far.

Mike

[mactec54]

baldysm

If you are not using the cutter comp, in the program, then turn it off in your cam program, the cutter comp off/cancel ( G40 ) is being used incorrectly

[beege]

Definitely turn off comp with a straight line, preferably perpendicular. My Haas had a few times where the tool table got corrupted, and the machine would lock up. If fixing the program doesn't do it for you, I'd write down all my tool and fixture offsets, clear both tables and re-enter the values. That solved my problem 6 months ago, with no recurrence.

[djr76]

add a G00 or G01 in the G40 line.

[Machineit]

add a G00 or G01 in the G40 line.

The G40 line is a circular move with I and J. ?????????

[fishinguy1]

I agree with first response, our try a g41 on the next z move after block 440.

[djr76]

The G40 line is a circular move with I and J. ?????????

I said to add a linear move within the G40 line, in which it would cancel out the circular move and the cutter comp.

[ghyman]

My $0.02:
You have some extremely small (.0005") moves in this program, which tells me your tool must be almost exactly the same size as the slots you are milling.
This is undoubtedly the source of the error... (I also agree with previous statements... cancelling cutter comp on arc moves is a bad thing!)
However... having so little room to move means the cutter comp never has time to "activate." Generally speaking, you should always have enough of a ramp-in for the control to be able to comp the tool. I usually use a linear move that is 2X the maximum expected comp.
If the program is being generated by a CAM program, then my guess is that the post is having an issue with little or no lead-in because the tool and pocket are nearly the same size.
If you remove the G41 and G40 calls completely, everything should work fine, but this will not allow you to comp your tool.
I would recommend going with a smaller diameter tool, so you are able to make moves that are larger than .0005"!
I don't know the sizes you are cutting, but the 8000RPM tells me it is a fairly small tool (~.093"?)
If possible, I would go with a tool that is at least .015" smaller than the slot, and then as suggested above, ramp in and ramp out with linear moves, and call the G41 and G40 commands ONLY on those linear moves.

[fishinguy1]

I very much agree with the Gyman response, also there is a online site called G WIZARD for a basic explanation of g and m codes for cnc programing. It could shed some light on this hang up.

[fishinguy1]

Please reply, on how things end up, so the head banging can stop.

[MachinistDan]

im having thie exact same issue as above ^^ ( baldsym )

[dcoupar]

im having thie exact same issue as above ^^ ( baldsym )

Are you running the exact same program? If not, please post it here.