Haas cnc lathe uses one-line syntax of G71 roughing canned cycle.
This cnc program example shows the use of G71 turning cycle for ID roughing (Inside roughing).
You might like
- G71 Rough Turning Cycle One-line Format
- CNC Fanuc G71 Turning Cycle or Stock Removal Canned Cycle (Two-line format)
- Fanuc G70 G71 Rough and Finish Turning Cycle Program Example
- CNC Programming Example with Fanuc G71 Rough Turning Cycle and G70
1 – A boring bar is used for the whole the roughing operation with G71 Rough Turning Cycle.
2 – Same boring bar is used for finish cut with G70 Finishing Cycle.
Example of using a Haas G71 for I.D. Roughing and Finishing.
Haas CNC Program Example
O1136 N1 T101 N2 G97 S2000 M03 N3 G54 G00 X0.7 Z0.1 M08 N4 G71 P5 Q12 U-0.01 W0.005 D0.08 F0.01 N5 G00 X4.5 N6 G01 X3. R.25 F.005 N7 Z-1.75 R.5 N8 X1.5 R.125 N9 Z-2.25 R.125 N10 X.75 R.125 N11 Z-3. N12 X0.73 N13 G70 P5 Q12 N14 M09 N15 G53 X0 G53 Z0 M30
Haas CNC Program Explanation
N1 – Tool 1 Offset 1
N3 – Rapid to start position
N4 – U is a minus for G71 I.D. Roughing
N5 – N5 is start of part path geometry defined by P5 in G71 line
N12 – N12 is end of part path geometry defined by Q12 in G71 line
N13 – G70 Defines a finish pass for lines P5 through Q12
N15 – To send machine home for a tool change