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

This cycle is used for normal drilling. Cutting feed is performed to the
bottom of the hole. The tool is then retracted from the bottom of the hole
in rapid traverse.
G81 (G98) G81 (G99)
G81 X_ Y_ Z_ R_ 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
F_ : Cutting feedrate
K_ : Number of repeats
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 performed from point R to point Z.
The tool is then retracted in rapid traverse.
Before specifying G81, use a miscellaneous function (M code) to rotate
the spindle.
When the G81 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 performed
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.
Drilling Cycle, Spot
Drilling (G81)

Leave a Reply

Your email address will not be published.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