FANUC Series 16/18/160/180-Model C Machining Center Operators Manual

PROGRAMMING
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
B–62764EN/01
204
This cycle is used to bore a hole.
G89 (G98) G89 (G99)
G89 X_ Y_ Z_ R_ P_ F_ K_ ;
X_ Y_: Hole position data
Z_ : The distance from point R to the bottom of the hole
R_ : The distance from the initial level to point R level
P_ : Dwell time at the bottom of a hole
F_ : Cutting feed rate
K_ : Number of repeats
P
P
Point R
Initial level
Point R level
Point Z
Point R
Point Z
This cycle is almost the same as G85. The difference is that this cycle
performs a dwell at the bottom of the hole.
Before specifying G89, use a miscellaneous function (M code) to rotate
the spindle.
When the G89 command and an M code are specified in the same block,
the M code is executed at the time of the first positioning operation. The
system then proceeds to the next drilling operation.
When K is used to specify the number of repeats, the M code is executed
for the first hole only; for the second and subsequent holes, the M code
is not executed.
When a tool length offset (G43, G44, or G49) is specified in the canned
cycle, the offset is applied at the time of positioning to point R.
14.1.13
Boring Cycle
(G89)
Format
Explanations

Leave a Reply

Your email address will not be published. Required fields are marked *