G89: Boring Cycle
This cycle performs a boring operation. Upon reaching the bottom of the hole, the cutting speed is used for retraction. It is almost identical to the G85 command, with the only difference being an additional dwell at the bottom of the hole.
|
Format: |
G89 X_ Y_ Z_ R_ P_ F_ K_ |
X: Hole position X-axis coordinate
Y: Hole position Y-axis coordinate
Z: Hole bottom coordinate
R: The Z safe rapid descent coordinate
P: Dwell time at the bottom of the hole (unit: ms)
F: Cutting feedrate
K: Number of repetitions
Before issuing the G89 command, spindle rotation must be activated using an M code. The M code provided on the same line as the G89 command is processed once during the initial positioning. However, the drilling operation proceeds without waiting for the completion of the M code. If multiple tapping operations are to be performed with the same command, the M code on the same line as G89 is executed only once during the first operation.
To perform the boring operation, one of the axes, such as X, Y, Z, R, or others, must be specified as a command.
When programming the G89 code, the R value must be specified in the first line of consecutive G89 commands. In subsequent boring lines, it is not mandatory.
The G89 code cannot be executed while tool radius compensation is active. Before using the G89 code, cancel the tool radius compensation with G40. Tool length compensation commands can be used with G89.
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 POINT X100 Y-250)
(RETURN TO POINT R AFTER BORING OPERATION)
G90 G99 G89 X100. Y-250. Z-150. R10. P1000 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)