G82: Drilling Cycle/Reverse Boring
This cycle performs a standard drilling operation. The cutting motion is executed at the specified cutting feed rate until reaching the bottom of the hole. After waiting for the duration specified by P at the bottom, the tool retracts with a rapid motion.
|
Format: |
G82 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 programming the G82 command, the spindle rotation must be activated using an M code.
The M code specified on the same line as the G82 command is executed once during the initial positioning. However, the drilling operation starts without waiting for the completion of the M code. If multiple drilling operations are to be performed with the same command, the M code specified with G82 is executed only once during the first operation.
To perform the drilling operation, one of the axes, such as X, Y, Z, R, or any other, must be specified as a command.
When programming the G82 code, the R value must be specified in the first line of consecutive G82 commands. It is not mandatory in the subsequent drilling lines.
The G82 code cannot be executed while the tool radius compensation is active. Disable the tool radius compensation with G40 before using the G82 code. Tool length compensation commands can be used with the G82 code.
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)
(DRILL A HOLE AT X100 Y-250)
(RETURN TO POINT R AFTER THE DRILLING OPERATION)
G90 G99 G82 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)