G87 Fine Back Boring Cycle

Format

G87 X_Y_Z_R_Q_P_F_K_

Machining Process

Machining process of G87 is as illustrated as follows:

  1. The tool moves to the specified hole position (X, Y) at G00 speed.
  2. After OSS, offsets cutting depth Q in a direction opposed to the direction of boring tool specified by parameter “Oriented Spindle Stop)”.
  3. The tool goes down to the specified point R at G00 speed.
  4. The tool shifts cutting depth Q (the offset distance).
  5. The spindle rotates CW.
  6. The tool retracts to point Z at G01 speed.
  7. The tool pauses for P.
  8. Offset cutting depth Q in a direction opposed to previous offset.
  9. The tool returns to the initial point (G98) or point R (G99) at G00 speed.
  10. Offset cutting depth Q.

Programming Example

F1200 S600

G90

G00 X0 Y0 Z10 'move to the initial point 

G17

M03  'spindle CW on

G90 G98 'specify the coordinates of point R, point Z and hole 1, with offset as 5, dwell time as 4s, and boring 
speed as 800


G87 X5 Y5 Z-10 R-5 Q5 P4000 F800

X25 'hole 2

Y25 'hole 3

X5 'hole 4, and set to return to the initial point

G80

M05 'spindle stops

M02