G88: Boring Cycle
This cycle performs a boring operation. When the bottom of the hole is reached, the spindle is stopped after waiting for the P value, and manual retraction of the hole axis is expected. Once the retraction is completed, the spindle is turned on again and the program proceeds to the next line.
|
Format: |
G88 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 G88 command, the spindle rotation must be set using an M code.
The M code given in the same line as G88 is processed once during the first positioning. However, the drilling operation starts before the M code is completed. If multiple boring operations are to be performed with the same command, the M code given in the same line as G88 is executed only once during the first operation.
One of the axes X, Y, Z, R, or other axes must be specified as a command in order to perform the boring operation.
When programming the G88 code, the R value must be specified in the first line of successive G88 commands. It is not mandatory in the subsequent boring lines.
G88 code cannot be executed while tool radius compensation is enabled. Turn off tool radius compensation with G40 before using the G88 code. Tool length compensation commands can be used with G88.
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 S500 (SPINDLE CW ROTATION)
(PERFORM BORING OPERATION AT POINT X100 Y-250)
(RETURN TO POINT R AFTER BORING OPERATION)
G90 G99 G88 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)