G86: Boring Cycle

This cycle performs the boring operation. When the hole bottom is reached, the spindle stops, and the retraction is carried out in this way.

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 issuing the G86 command, the spindle rotation must be provided with an M code. The M code given on the same line as G86 is processed once during the initial positioning. However, the drilling operation begins without waiting for the completion of the M code. If multiple thread cutting operations are performed with the same command, the M code given with G86 on the same line will only be executed once during the first operation.

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

When programming the G86 code, the R value must be specified in the first line of consecutive G86 commands. It is not required in subsequent boring lines.

The G86 code cannot be executed when tool radius compensation is enabled. Before using the G86 code, disable tool radius compensation with G40. Tool length offset commands can be used with G86.

Canned cycle commands must not be programmed on the same line as group 1 G codes (G0, G1, G2, G3). If programmed, the repetitive cycle commands will be canceled.

Example:

M3 S2000 (SPINDLE CW ROTATION)

(PERFORM BORING OPERATION AT X100 Y-250)

(RETURN TO THE R POINT AFTER THE OPERATION)

G90 G99 G86 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)