G88 Cycle Introduction
G88 cycle is used in CNC turning machines with driven tool for tapping holes from the side to the workpiece. In this tapping cycle, when the bottom of the hole has been reached, the spindle is rotated in the reverse direction. It is the same as the G84 cycle as a command format, the only difference is that it is used for tapping holes in the X axis direction, not in the Z axis direction.
After the command is used, tapping to the other coordinates is continued by positioning the Z axis or C axis. The G88 cycle continues to run until the G80 command arrives.
|You may be interested also:|
|“CNC Lathe | G87 Cycle | Side Drilling”|
G88 Cycle Format
|G88 X(U)_ R_ P_ F_ Q_ K_ M_ ;|
|G88: Side Tapping|
|X_ or U_ : Final drilling depth (X for absolute, U for incremental)|
|R_ : The distance from the initial level to point R level|
|P_ : Dwell time at the bottom of a hole|
|Q_ : Depth of cut for each cutting feed (For Fanuc controller; Bit 6 (PCT) of parameter No. 5104 = “1”)|
|F_ : Cutting feedrate|
|K_ : Number of repeats (When it is needed.)|
|M_ : M code for C-axis clamp (when it is needed.)|
When you use Q in cycle line, it’s automatically switch to Peck tapping cycle. If depth of cut (Q) is not specified for each tapping, the normal tapping cycle is used. Same format can be use for G84 cycle also to drill from Z axis side.
G88 Cycle Examples
G88 CNC Program Example – 1
M51 ; Setting C-axis index mode ON
M3 S2000 ; Rotating the drill
G00 X50.0 C0.0 Z-20.0 ; Positioning the drill along the Z- and C-axes
G88 X20.0 R10.0 Q5000 F5.0 M31 ; Tapping hole 1
C90.0 Q5000 M31 ; Tapping hole 2
C180.0 Q5000 M31 ; Tapping hole 3
C270.0 Q5000 M31 ; Tapping hole 4
G80 M05 ; Canceling the tapping cycle and stopping tapping rotation
M50 ; Setting C-axis index mode off
M30 ; Program end
Note: M31 is used for C axis Clamp in this example. Could be change due to machine builder.