G84 cycle is used in CNC turning machines for tapping holes from the front 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 G88 cycle as a command format, the only difference is that it is used for tapping holes in the Z axis direction, not in the X axis direction.
After the command is used, tapping to the other coordinates is continued by positioning the X axis or C axis. The G84 cycle continues to run until the G80 command arrives.
G84 Z(W)_ R_ P_ F_ Q_ K_ M_ ;
G84: Tapping cycle
Z_ or W_ : Final drilling depth (Z for absolute, W 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 G88 cycle also to drill from X axis side.
O1234; Program no M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the tap G00 X50.0 C0.0 ; Positioning the tapping along the X- and C- axes G84 Z-40.0 R-5.0 P500 F5.0 M31 ; Tapping hole 1 C90.0 M31 ; Tapping hole 2 C180.0 M31 ; Tapping hole 3 C270.0 M31 ; Tapping hole 4 G80 M05 ; Canceling the tapping cycle and stopping tap rotation M50 ; Setting C-axis index mode off M30 ; Program end
Note: M31 : C axis Clamp
Vote to create best CNC source on the web all together!
Do you think the content is understandable, good and contain everything?
- Yes, the article is perfect and enough.
- No, it’s need to improve.
(If a article voted mostly for “need to improve”, we moves article to development category and all members can add-edit to article to create best content. More details)