I want to boring ID taper (big ID is 1.767" at Z0) and (small ID is 1.6858) with 1.3 inches length.
I drilled ID at 1 inch already... I want to cut .020 each time until to finish size...
Please give me a G-code for Haas Lathe SL, so I can learn it.
Thank you...
Here you go! I have a slightly different programming style than what you might glean from a book, etc., but it all works the same.
Often, I will separate roughing toolpaths from finishing toolpaths. When hand-coding I have become used to not using program restart, so that's where some of my habits come from. This is perhaps more 'conventional', if you will.
O00001 (TAPERED I.D. ROUGH/FINISH)
(TURN I.D.)
T606 M8 (Call up T6, Offset 6)
G54 (Call up G54 work coordinate offset)
G50 S2000 (Limit spindle speed to 2000 RPM max)
G96 S400 M03 (Enable constant surface speed mode at 400 SFM, turn spindle on forward)
G0 G41 X1. Z1. (Rapid to safe position; position before G71 canned cycle is where tool begins roughing from; IE, starting at X1. will begin roughing from 1" diameter, plus/minus any depth of cut or finish allowances; G41 turns on tool nose compensation, shifting the tool over based upon the radius and tool tip number in the tool geometry page, allowing for nose radius)
Z.05
G71 P10 Q20 U-.02 W.005 D.02 F.005 (Begins a G71 OD/ID stock removal canned cycle, using the profile contained between codes N10 and N20, with an X offset of -.02, a Z offset of .005, depth of cut of .020, feed rate of .005/rev)
N10 (Start of profile roughed by G71)
G0 X1.767 (Rapid up to first X)
G1 Z0. (Feed to face of part)
X1.6858 Z-1.3 (Feed from current position to X/Z position)
Z-1.35
X1. (Return to start diameter, can be just slightly smaller than ending X if there is no bottom face)
N20 (End of profile)
S500 (With G96 on, surface speed will increase to 500 SFM)
G70 P10 Q20 F.004 (Finish cycle referring to profile contained between N10 and N20, above)
G0 G40 Z1. M9 (Rapid to safe position, turn off tool nose compensation, turn coolant off)
X10. Z6. (Rapid to tool change or end position)
M1 / M30 (Option Stop if followed by another toolpath, program stop and rewind if finished)
