G74: Reverse Tapping Cycle for Milling
This cycle performs reverse tapping. When the bottom of the hole is reached, the spindle begins to rotate in the reverse direction.
|
Format: |
G74 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: The dwell time at the hole bottom
F: Cutting feed rate
K: Number of repetitions
The tapping operation is performed by rotating the spindle counterclockwise. When the hole depth is reached, the spindle is rotated clockwise for the retraction process. This creates the reverse thread.
During this process, the cutting feed rate setting cannot be adjusted. Program pause is disabled until the operation is completed.
Before issuing the G74 command, the spindle rotation must be enabled with an M code. The M code given on the same line as G74 is executed once during the initial positioning. However, the drilling operation proceeds before the M code is completed. If multiple taps are performed with the same command, the M code given on the same line as G74 is only executed once during the first operation.
One of the axes, such as X, Y, Z, R, or others, must be specified as a command for the drilling operation to be performed.
When programming the G74 code, the R value must be specified in the first line of consecutive G74 commands. It is not required in subsequent tapping lines.
While tool radius compensation is enabled, the G74 code cannot be executed. Before using the G74 code, disable tool radius compensation with G40. Tool length compensation commands can be used with G74.
Canned cycle commands should not be programmed on the same line as Group 1 G-codes (G0, G1, G2, G3). If they are, the canned cycle commands will be canceled.
Example:
M4 S100 (SPINDLE CCW ROTATION)
(PERFORM THREAD CUTTING AT THE X100 Y-250 POINT)
(RETURN TO THE R POINT AFTER THE DRILLING OPERATION)
G90 G99 G74 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)