G85: Boring Cycle

This cycle performs boring. When the bottom of the hole is reached, cutting feed is used for retraction.

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 G85 command, the spindle rotation must be activated with an M code. The M code given on the same line as G85 is processed once during the first positioning. However, the drilling operation proceeds without waiting for the completion of the M code. If multiple threading operations are performed with the same command, the M code given on the same line as G85 is executed only once during the first operation.

For the boring operation to be carried out, one of the axes, X, Y, Z, R, or others, must be specified as a command.

When programming the G85 code, the R value must be specified in the first line of consecutive G85 commands. It is not mandatory to provide the R value in the following boring lines.

When tool radius compensation is enabled, the G85 code cannot be executed. Before using the G85 code, disable tool radius compensation by using the G40 command. Tool length compensation commands can be used with G85.

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 S100 (SPINDLE CW ROTATION)

(PERFORM BORING OPERATION AT X100 Y-250)

(RETURN TO THE R POINT AFTER THE OPERATION)

G90 G99 G85 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)