[mikefalkner]

I want to cut slots in my CNC table top for T-Tracks. I use "Toolpath Transform" function in Mastercam X4 to generate the G-code. The resulting G-code is shown below. It appears to be simple enough, but when I loaded it into Mach3, I get a weird toolpath display with cuts 3 & 4, which use G57 & G58, and cuts 10 & 12 which use G59 P4 & G59 P5 (see attached photo). All other offsets (i.e., G54, G55, G56, ... ) are displayed correctly.

This occurs even with I delete the other cuts except G57 & G58. The same weird display occurs.

What am I doing wrong? What is causing this weird display?

G-CODE:
%
O0000(TABLE SLOT)

(SETUP)
N100 G17 G20 G90 G40 G80 G64 G49 G0 M05
N110 G8 P1
N120 G90 M05 Z0
N130 G52 X0. Y0. Z0.
N140 T1 M6
N150 S18000 M3
N155 G43 H2 Z.25

(1ST CUT)
N160 G0 G90 G54 X.625 Y.25
N170 G0 G54
N180 M98 P0001

(2ND CUT)
N190 G90 G55 X9.35 Y.25 Z.25
N200 G0 G55
N210 M98 P0001

(3RD CUT)
N220 G90 G56 X18.075 Y.25 Z.25
N230 G0 G56
N240 M98 P0001

(4TH CUT)
N250 G90 G57 X26.8 Y.25 Z.25
N260 G0 G57
N270 M98 P0001

(5TH CUT)
N280 G90 G58 X35.525 Y.25 Z.25
N290 G0 G58
N300 M98 P0001

(6TH CUT)
N310 G90 G59 X44.25 Y.25 Z.25
N320 G0 G59
N330 M98 P0001

(RAP UP)
N340 G90 G49 Z0. M05
N350 G52 X0. Y0. Z0.
N360 G8 P0
N370 G17
N380 M30

(SUBROUTINE)
O0001
N100 G91
N110 G1 Z-.69 F500.
N120 Y48.5
N130 X-.225
N140 Y-48.5
N150 X.225
N160 Z.69 F100.
N170 M99
%

[ger21]

First, are you aware that G59 P4 = G57 and G59 P5=G58?
P1-P6 are G54-G59.
If you want to use additional offsets beyond G59, start at G59 P7.

As for the display issues. Mach3 has always had some bugs in the toolpath display when using offsets. In these cases the machine should cut correctly even though the display is wrong.

[mikefalkner]

Thanks for the information regarding P1-P6 for G59. I had forgotten that.

NEW TEST CODE:
So, to test a possible solution, I wrote a simpler G-code (see below) for 10 offset cuts. These are well within my soft limits just to make sure that was not causing Mach3 any problems. I also used the G59 P7 and up after reaching G58.

CNC TABLE RESULTS:
When I took the code out to the CNC machine, the machine followed exactly what was being displayed in Mach3 – the weird display and cutout not what I wanted. In fact, the Mach3 on the machine computer displayed a completed different weird toolpath. So, each Mach3 software (although the exact same version R3.043.022) displayed a completely different weird toolpath for the exact same g-code. And the machine followed that weird toolpath exactly.

CONCLUSION SO FAR:
The only thing I can think of is that Mach3 has a bug regarding offsets. Now that hard for me to believe since it has been around a long time, and I am sure others users have used offsets many times and don't have this weird problem. So I am thinking I got something screwed up, and I am out of ideas. So any help or hints would be greatly appreciated.

Thanks,
Mike

SAMPLE G-CODE:
%
O0000(Z)
(DATE=DD-MM-YY - 16-06-13 TIME=HH:MM - 11:21)
(MCX FILE - C:\MASTERCAMX4\Z.MCX)
(NC FILE - C:\MASTERCAMX4\Z.NC)
(MATERIAL - WOOD INCH)
( T1 | 1/2 STRAIGHT BIT | H0 )

(**** SET UP ****)
N100 G17 G20 G90 G40 G80 G64 G49 G0 M05
N110 G8 P1
N120 G90 M05 Z0
N130 G52 X0. Y0. Z0.
N140 T1 M6
N150 S18000 M3
N160 G43 H0 Z.25

(**** CUT 1 ****)
N170 G0 G90 G54 X5.75 Y5.25 C0.
N180 M98 P0001

(**** CUT 2 ****)
N190 G90 G55 X7.25 Y5.25 Z.25 C0.
N200 G55
N210 M98 P0001

(**** CUT 3 ****)
N220 G90 G56 X8.75 Y5.25 Z.25 C0.
N230 G56
N240 M98 P0001

(**** CUT 4 ****)
N250 G90 G57 X10.25 Y5.25 Z.25 C0.
N260 G57
N270 M98 P0001

(**** CUT 5 ****)
N280 G90 G58 X11.75 Y5.25 Z.25 C0.
N290 G58
N300 M98 P0001

(**** CUT 6 ****)
N310 G90 G59 X13.25 Y5.25 Z.25 C0.
N320 G59
N330 M98 P0001

(**** CUT 7 ****)
N340 G90 G59 P7 X14.75 Y5.25 Z.25 C0.
N350 G59 P7
N360 M98 P0001

(**** CUT 8 ****)
N370 G90 G59 P8 X16.25 Y5.25 Z.25 C0.
N380 G59 P8
N390 M98 P0001

(**** CUT 9 ****)
N400 G90 G59 P9 X17.75 Y5.25 Z.25 C0.
N410 G59 P9
N420 M98 P0001

(**** CUT 10 ****)
N430 G90 G59 P10 X19.25 Y5.25 Z.25 C0.
N440 G59 P10
N450 M98 P0001

(**** RAP UP ****)
N460 G90 G49 Z0. M05
N470 G52 X0. Y0. Z0.
N480 G8 P0
N490 G17
N500 M30

(**** SUBROUTINE ****)
O0001
N100 G91
N110 Z-.15
N120 G1 Z-.54 F25.
N130 X.225 F50.
N140 Y4.5
N150 X-.225
N160 Y-4.5
N170 Z.1 F100.
N180 G0 Z.59
N190 M99
%

[mikefalkner]

FOUND SOLUTION. I had not zero the Offsets in the Offset Table in Mach3. I clicked on the "Offset" tab, clicked on "Save Work Offset" button, and put zeros in all the entries in the table. Now, everything works perfectly. Both copies of my Mach3 software had different numbers in this table, which is why I was getting weird displays and machine toolpaths. Hope this helps someone new to Mach3 Offsets.

Again, thanks for helping me.
Mike