Copyright Goodheart-Willcox Co., Inc. Chapter 9 CNC Mill Programming 199 After learning the basics of when to use canned cycles and why, a good CNC machinist can make use of additional canned cycles. Common cycles are presented in the following sections. A complete list of all canned cycles for a particular machine can be found in the machine’s programming manual. 9.8.2 G73 Cycle (Chip Break Peck Drilling) The G73 canned cycle is similar to G83, but it does not retract the drill completely out of each hole, just a short amount to break off the chip. Here is a G73 program for the same hole we coded before: G90 G54 X1. Y1. M3 S2500 (X1. Y1. is location of first hole) T1 M6 G43 H1 Z1. M8 G0 Z.25 G98 G73 Z−1. R.1 Q.25 F10. X2. Y2. (Second hole) X3. Y3. (Third hole) G80 Since the G98 is programmed, the drill will return to Z.25 between holes and not the Z.1. ■ G98: Returns to last Z position (.25″ in this case) between holes. ■ G73: Turns on chip break peck drilling. ■ Z: Final depth of hole. Note: Different Z positions can be programmed on subsequent holes. ■ R: The rapid position in Z that spindle goes before drilling. ■ Q: The peck amount, always a positive number. ■ F: The feed rate while drilling. 9.8.3 G81 Cycle (Spot Drilling) The G81 is a standard drilling cycle that does not peck instead, it travels to a programmed Z depth. This cycle is often used for spot drilling or for holes with a depth less than four times greater than the diameter. This cycle should also be used for solid carbide drills, as they will shatter under peck- ing conditions. G90 G54 X1. Y1. M3 S2500 (X1. Y1. is location of first hole) T1 M6 G43 H1 Z1. M8 G0 Z.25 G98 G81 Z−1. R.1 F10. X2. Y2. (Second hole) X3. Y3. (Third hole) G80