G84: Tapping Cycle
This cycle performs tapping operations. Once the hole bottom is reached, the spindle starts rotating in the reverse direction.
|
Format: |
G84 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
The tapping operation is performed by rotating the spindle in the clockwise direction. When the hole bottom is reached, the spindle is rotated counterclockwise for the retraction movement, thus completing the tapping process.
During this process, the cutting feed rate cannot be adjusted. Program pause is disabled until the operation is completed.
Before issuing the G84 command, the spindle rotation must be set with an M code. The M code provided on the same line as G84 will be processed once during the first positioning. However, the hole-making process will begin without waiting for the M code to complete. If multiple taps are performed with the same command, the M code given on the same line as G84 will only be executed once during the first operation.
To perform the hole drilling operation, one of the coordinates X, Y, Z, R, or other axes must be specified as a command.
When programming the G84 code, the R value must be specified in the first line of successive G84 commands. For subsequent tapping lines, it is not mandatory.
G84 code cannot be executed when tool radius compensation is enabled. Before using G84, turn off tool radius compensation with the G40 code. Tool length offset commands can be used with G84.
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 TAPPING OPERATION AT X100 Y-250)
(RETURN TO R POINT AFTER OPERATION)
G90 G99 G84 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)