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

PROGRAMMING
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
B–62764EN/01
186
This cycle is used for normal drilling.
Cutting feed is performed to the bottom of the hole. At the bottom, a dwell
is performed, then the tool is retracted in rapid traverse.
This cycle is used to drill holes more accurately with respect to depth.
G82 (G98) G82 (G99)
G82 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 Z
Point R
Point Z
Point R level
After positioning along the X– and Y–axes, rapid traverse is performed
to point R.
Drilling is then performed from point R to point Z.
When the bottom of the hole has been reached, a dwell is performed. The
tool is then retracted in rapid traverse.
Before specifying G82, use a miscellaneous function (M code) to rotate
the spindle.
When the G82 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.
14.1.5
Drilling Cycle Counter
Boring Cycle
(G82)
Format
Explanations

Leave a Reply

Your email address will not be published.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