Haas lathe programming example to illustrate the use and programming of Haas G72 Type I Rough Facing Cycle/ G70 Finish Cycle.
The above code will also work on cnc lathe machines with Fanuc cnc control with little or no change.
All the G-code / M-code which are used in this Haas lathe programming example are given below with description.
Haas G72 Type I Rough G70 Finish Facing Cycle Program Example
Haas G72 Type I Rough and G70 Finish Facing Program Example
O00096 N1 (G72 ROUGHING FACE) N2 G53 G00 X0. Z0. T0 (Sending home for a tool change) N3 T101 (O.D. TOOL x .031 TNR) (Select Tool 1 Offset 1) N4 G50 S3000 N5 G97 S450 M03 N6 G54 G00 X3.1 Z0.1 M08 (Rapid to start point above part stock) N7 G96 S370 N8 G72 P9 Q18 U0.01 W0.01 D0.06 F0.012 (G72 Rough Facing Cycle with TNC) N9 G41 G00 Z-1.6 (Starting sequence number defined by P8 in G72 and G70) N10 G01 X2. F0.008 N11 X1.4 Z-0.9 N12 X1. N13 Z-0.6 N14 G03 X0.8 Z-0.5 R0.1 N15 G01 Z-0.1 N16 X0.6 Z0. N17 X-0.062 N18 G40 G00 Z0.1 (End of part path geometry defined with P17 in G72 and G70) N19 G97 S450 M09 N20 G53 G00 X0. Z0. T0 (Sending home for a tool change) N21 M01 (Optional Stop) N22 (G70 FINISHING FACE) N23 G53 G00 X0. Z0. T0 (Sending home for a tool change) N24 T202 (O.D. TOOL x .015 TNR) (Select Tool 2 Offset 2) N25 G50 S3000 N26 G97 S450 M03 N27 G54 G00 X3.1 Z0.1 M08 (Rapid to start point) N28 G96 S420 N29 G70 P9 Q18 (Finish Facing with G70 Finish Cycle) N30 G97 S450 M09 N31 G53 G00 X0. Z0. T0 (Sending home for a tool change) N32 M30 ( End of Program and Reset)
G-Codes
G00 Rapid traverse motion.
G01 Linear interpolation motion.
G03 Circular Interpolation – Counterclockwise.
G41 Tool Nose Compensation LEFT of the programmed path.
G40 Tool Nose Compensation CANCEL.
G50 Spindle Maximum RPM Limit.
G53 Machine Zero Positioning Coordinate Shift.
G54 Work Offset Positioning Coordinate #1 (Setting 56)
G72 End Face Stock Removal Cycle.
G70 Finishing Cycle.
G96 Constant Surface Speed On.
G97 Constant Surface Speed Cancel.
M-Codes
M01 Optional Program Stop.
M03 Starts the Spindle FORWARD.
M30 Program End and Reset to the beginning of program.
