G81: Simple Drilling Cycle

This cycle performs normal drilling operation. Cutting motion is carried out with the given cutting feed rate until the hole bottom is reached.

X: Hole position X-axis coordinate

Y: Hole position Y-axis coordinate

Z: Hole bottom coordinate

R: The Z safe rapid descent coordinate

F: Cutting feedrate

K: Number of repetitions

Before executing the G81 command, spindle rotation must be enabled with an M code. The M code given in the same line as G81 is executed once during the first positioning. However, the drilling operation begins without waiting for the M code to complete. If multiple drilling operations are performed with the same command, the M code given in the same line as G81 is executed only once during the first operation.

To perform the boring operation, one of the X, Y, Z, R, or other axes must be specified as a command.

When programming the G81 code, the R value must be provided in the first line of consecutive G81 commands. It is not mandatory in subsequent drilling lines.

When tool radius compensation is active, the G81 code cannot be executed. Before using the G81 code, disable tool radius compensation with the G40 command. Tool length compensation commands can be used with G81.

Canned cycle commands should not be programmed on the same line as Group 1 G-codes (G0, G1, G2, G3). If they are, the canned cycle commands will be canceled.

Example:

M3 S2000 (SPINDLE CW ROTATION)

(DRILL A HOLE AT X100 Y-250)

(RETURN TO POINT R AFTER THE DRILLING OPERATION)

G90 G99 G81 X100. Y-250. Z-150. R10. F120.

X200.       (2ND DRILLING OPERATION)

Y0.         (3RD DRILLING OPERATION)

X100.       (4TH DRILLING OPERATION)

G98 Y250.   (5TH DRILLING OPERATION)

G80 G53 Z0. (GO TO Z AXIS REFERENCE)

M5          (SPINDLE STOP)