G87: Boring Cycle, Backboring

This cycle performs a boring operation in the reverse direction. After a rapid move to the hole center, the spindle stops at a predefined angle. Then, the tool moves in the opposite direction for retraction, followed by a rapid move to the R point, and the operation continues. After a retraction move toward the tool direction to the hole center, the spindle rotates. This process continues until the Z coordinate is reached. Upon reaching the Z coordinate, the spindle repositions according to the predefined angle, and then the retraction movement is performed in the opposite direction of the tool. This way, a rapid movement towards the starting point is made. Once the starting point is reached, another retraction movement is made in the tool direction, and the spindle rotation is released.

X: Hole position X-axis coordinate

Y: Hole position Y-axis coordinate

Z: Hole bottom coordinate

R: The Z safe rapid descent coordinate

Q: Distance from the surface at the bottom of the hole

P: Dwell time at the bottom of the hole (unit: ms)

F: Cutting feedrate

K: Number of repetitions

The M-code must be issued to start the spindle rotation before executing the G87 command.

The M-code specified on the same line as the G87 command is executed once during the initial positioning. However, the drilling operation begins without waiting for the M-code to complete. If multiple boring operations are to be performed with the same command, the M-code specified with the G87 command 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 in the command. 

When programming the G87 code, the R and Q values must be specified in the first line of consecutive G87 commands. In subsequent boring lines, this is not mandatory. Since the Q value is used as the pecking distance in G73 and G83 cycles, care should be taken when using it with the G87 cycle. The previously defined Q value is retained in memory.

The G87 code cannot be executed while the tool radius compensation is active. Deactivate the tool radius compensation using G40 before issuing the G87 code. Tool length compensation commands can be used with the G87 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.

For this command to work properly, spindle orientation parameter settings and ladder program implementation must be completed. The axis and direction of the retraction movement at the bottom of the hole can be adjusted with PRM314.

           Example:

M3 S500 (SPINDLE CW ROTATION)

(PERFORM BORING OPERATION AT X100 Y-250)

(RETURN TO R POINT AFTER THE BORING OPERATION)

G90 G98 G87 X100. Y-250. Z10. R-50. Q5. 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)