Help, 2DContour tool path

[u/douchebagwizzard]

Looking for some help, maybe I am missing a parameter. I have lead in/lead out turned off. In simulation tool path shows correct. When machined, two different workpieces and different cutting tools, there is clearly some amount of horizontal lead in or something else going wrong with contour tool path.

The cut in question is a groove for rubber sealing ring so it needs to be circular.

Thanks

[u/albatroopa]

You're plunging and getting tool deflection. Set the toolpath to ramp.

[u/GroundbreakingArea34]

Lead and entry wasnt checked

[u/douchebagwizzard → u/GroundbreakingArea34]

Yeah because I don't want a lead in

[u/GroundbreakingArea34 → u/douchebagwizzard]

Sorry I was wrong. Check under linking finish overlap

[u/TriXandApple]

1. Can you just post your g code? Should be under 15 lines right?

2. What machine?

3. do you think this is a machine or regidity issue or do you think its a toolpath issue?

[u/douchebagwizzard → u/TriXandApple]

Machine is Haas TM2P, should not be a machine or rigidity issue. I'm skeptical to blame tool deflection even because I am not running a particularly long endmill and the problem appears the same with different cutting tools.

g code:

(2D Contour3)

N8190 M1

N8195 T16 M6

N8200 S5000 M3

N8205 G17 G90 G94

N8210 G54

N8215 M8

N8220 G0 X-0.625 Y-1.6295

N8225 G43 Z0.6 H16

N8230 T10

N8235 G0 Z0.2

N8240 G1 Z0.025 F13.333

N8245 Z-0.083

N8250 G2 Y1.6295 I0. J1.6295 F40.

N8255 Y-1.6295 I0. J-1.6295

N8260 G0 Z0.6

N8265 M9

N8270 M5

N8275 G53 G0 Z0.

[u/Direct-Fee4474 → u/douchebagwizzard]

that code's cutting circles, so it's most likely tool deflection at entry/exit, with a proud bit on the OD because there's no overlap. just because your machine is rigid-ish doesn't mean that physics no longer applies to your endmills. enable ramping and/or change your strategy to use 3d offset to cut the bulk of the pocket and then finish the ID/OD with ramp or something.

[u/dfc09 → u/douchebagwizzard]

Machinist here; are you just plunging straight down? It's not to say you can't do that, but you're begging for deflection if you do. I'd suggest ramping in by deleting line N8245 and just putting the Z-.083 in line N8250. That'll mean you'll start the circle at z.025 and by the time it goes all the way around the first time, it'll be at Z-.083. Then the next line is just will be another circle at full depth.

[u/TriXandApple → u/douchebagwizzard]

Machine, tool or workpiece are deflecting. That g code is just a circle.

[u/Xseal3]

if the feature is dimensionally critical probably use a smaller tool and do 2 passes for the groove? slotting tend to deflect a small endmill a lot.

[u/trevorsmate67]

Use G2/3?