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

This cycle is used to bore a hole.
G85 (G98) G85 (G99)
G85 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 feed rate
K_ : Number of repeats
Point R
Initial level
Point R level
Point Z
Point Z
Point R
After positioning along the X– and Y– axes, rapid traverse is performed
to point R.
Drilling is performed from point R to point Z.
When point Z has been reached, cutting feed is performed to return to
point R.
Before specifying G85, use a miscellaneous function (M code) to rotate
the spindle.
When the G85 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.
Boring Cycle

Leave a Reply

Your email address will not be published.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