9 NC Programming Routines
9.6 Canned Cycle Programming
139
G0X1Y1Z.1; RAPID TO 1,1,.1
G82G98Z-.5R0P5F2; DRILL TO DEPTH OF -.5, RAPID TO INITIAL POINT AFTER DWELL OF
5 SECONDS.
G80; CANCEL CANNED CYCLE
M2; END PROGRAM
Code
Explanation
G82G98Z-
.5R0P5F2; DRILL
TO DEPTH OF -.5,
RAPID TO INITIAL
POINT AFTER
DWELL OF 5
SECONDS.
G82
Straight drill with dwell
G98
Rapid move to initial tool position after canned
cycle complete.
Z-.5
Drill to depth of 0.5 inches
R0
Retract to Z0 after canned cycle complete.
P5
Dwell for 5 seconds at bottom of drilled hole.
F2
Feed rate of 2 inches per minute.
9.6.4.
G84: Thread Tapping
A G84 code is used for tapping threads. The tap reaches the specified depth and is then pulled out at a
rate 1.6 times the rate of insertion (60% faster).
A tapping head with a reversing mechanism is required when using a G84 code.
The use of the G84 code is shown in following example.
NC Code Example:
G0X1Y1Z.1; RAPID TO 1, 1, .1
G84G98Z-.5R0F2; TAP TO DEPTH OF -.5, RAPID TO INITIAL POINT
G80; CANCEL CANNED CYCLE
M2; END PROGRAM
Code
Explanation
G84G98Z-.5R0F2;
TAP TO DEPTH OF
-.5, RAPID TO
INITIAL POINT
G84
Start Thread Tapping cycle
G98
Rapid move to initial tool position after canned
cycle complete.
Z-.5
Drill to depth of 0.5 inches
R0
Retract to Z0 after canned cycle complete.
F2
Feed rate of 2 inches per minute.
9.6.5.
G85: Boring
The G85 code specifies a boring cycle. After the tool plunges, it retracts at the same feed to point R. This
sometimes gives a better surface finish on the hole. The tool then rapids to the initial point.
