Copyright Goodheart-Willcox Co., Inc. 198 CNC Manufacturing Technology a .250″ diameter hole that is more than 1″ deep. The peck drilling cycle drives the tool down to a partial depth and then fully retracts above the part to remove chips and allow coolant to enter. Then it reenters the hole and goes to a deeper depth. Without the G83, the code looks like this: G90 G54 X1. Y1. M3 S2500 T1 M6 G43 H1 Z.5 M8 G1 Z.1 F10. Z−.25 G0 Z.1 G1 Z−.5 G0 Z.1 G1 Z−.75 G0 Z.1 G1 Z−1. G0 Z.1 This tool drills −.25″ deep a total of four times and finishes at Z−1 deep. This is not terribly difficult, but imagine if you wanted to drill only .100″ deep with each peck or if you had ten holes to drill. This code gets very long and difficult to edit. Compare this method to one using a G83 cycle: G90 G54 X1. Y1. M3 S2500 (X1. Y1. is location of first hole) T1 M6 G43 H1 Z1. M8 G0 Z.25 G99 G83 Z−1. R.1 Q.25 F10. (First hole drilled) X2. Y2. (Second hole) X3. Y3. (Third hole) G80 By adding the X and Y locations after the G83 line, the same drill- ing pattern is applied at those locations. If the drilling conditions require changing the peck depths to .1″ instead of .25″, just change the Q to .1″, and all the holes are edited. A G80 cancels this canned cycle. The compo- nents to this cycle are as follows: ■ G98: Returns to last Z position (.25″ in this case) between holes. ■ G99: Returns to reference return position (.1″ in this case) between holes. ■ G83: Turns on 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.