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

PROGRAMMING
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
B–62764EN/01
188
This cycle performs peck drilling.
It performs intermittent cutting feed to the bottom of a hole while
removing shavings from the hole.
G83 (G98) G83 (G99)
G83 X_ Y_ Z_ R_ Q_ 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
Q_ : Depth of cut for each cutting feed
F_ : Cutting feedrate
K_ : Number of repeats
dq
dq
q
dq
dq
q
Initial level
Point R
Point Z
Point R level
Point R
Point Z
Q represents the depth of cut for each cutting feed. It must always be
specified as an incremental value.
In the second and subsequent cutting feeds, rapid traverse is performed
up to a d point just before where the last drilling ended, and cutting feed
is performed again. d is set in parameter (No.5115).
Be sure to specify a positive value in Q. Negative values are ignored.
Before specifying G83, use a miscellaneous function (M code) to rotate
the spindle.
When the G83 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.
14.1.6
Peck Drilling Cycle
(G83)
Format
Explanations

Leave a Reply

Your email address will not be published.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