Cutter compensation woes

[sp1nm0nkey]

I'm attempting to machine this butterfly looking piece in mach 3, but the
last few moves seem to be getting messed up. I'm writing them the exact
same way as the previous ones but they still seem to be getting messed up.

My version of mach3 has the tool path stopping at the very end
of the arc "g3 x0 y-0.25 r0.25" at the coordinate 0, -0.25-[cutterrad],
and then linearly going to the point spec'd by "g1 x0 y-0.125", at the coordinate [cutterrad],-0.125-[cutterrad], rather than stopping at 0,-0.25-[cutterrad], curving to [cutterrad],-0.25, and THEN moving to the point
[cutterrad],-0.125-[cutterrad]. It's essentially clipping the corner of my part.

Any ideas? I've tried sprinkling g42s and g41s here and there but to no avail.
This is also my first hand written g-code program... I'd definitely appreciate
comments/criticism.

g42
g0 x0 y0 z0.1
f10

g1 x0.125 y0
g1 z-0.1
g1 x0.25 y0
g3 x0 y0.25 r0.25

g1 x0 y0.125
g3 x-0.125 y0 r0.125
g1 x-0.25 y0
g3 x0 y-0.25 r0.25

g1 x0 y-0.125
g3 x0.125 y0 r0.125

[Energy Rebel]

Do you have to use cutter comp?
If not, then get rid of G41 & 42's and it should be fine.
Comp can affect position in both axes, that's why when you have to use it, you have to compensate for that "move" where it turns off and on. Otherwise, you'll gouge your part.
Just make your program path .125 "bigger" (or whatever tool dia. you need) and essentially program to the cutter path centerline rather than the part outline.
If for some reason it still shows a gouge on the computer after you've removed all comp commands, then try it anyway. It (the computer) might be "lying" to you. LOL
It's been known to happen.

[ger21]

Depending on which version of Mach3 your using, this might not work. It works on test version 3.43, which has new comp code that the next version of Mach3 will use. It should work on other versions as well.

If your cutting out a part, you'll want to start outside the part, not inside. Imo, the easiest place to start on this part is to come in on a straight segment. See the attached pic. The black circle is where the tool is before the G42, the red circle is after the comp move is applied. The black line is the coded path, the red is the comped path. Also, in Mach3, there are 3 ways to call G42

G42 P.125 (P is the tool radius)
G42 D1 (use the tool radius for tool #1 in the tool table)
G42 (Use the tool radius in the tool table of the current tool)

Here's the code.

G20 G40 G90 G91.1
(1/4" tool)
M3
G0 Z0.1
G0 X0.125 Y-0.435 Z0.1
G1 X0.125 Y-0.435 Z0.0 F10 (start outside of part to allow room for comp to be applied)
G42P0.125 (P specifies the tool radius)
G1 X0.0 Y-0.31 Z-0.1 (Comp is applied during this move - I like to ramp in here)
G1 X0.0 Y-0.125
G3 X0.125 Y0.0 R0.125
G1 X0.25 Y0.0
G3 X0.0 Y0.25 R0.25
G1 X0.0 Y0.125
G3 X-0.125 Y0.0 R0.125
G1 X-0.25 Y0.0
G3 X0.0 Y-0.25 R0.25
G40
G1 X0.125 Y-0.250 (move past part by tool radius before turning off comp)
G0 X0.125 Y-0.250 Z0.100
M30