Fanuc Series 15i/150i-MA (Programming) Operators Manual

B-63324EN/03 PROGRAMMING 13.FUNCTIONS TO SIMPLIFY PROGRAMMING
- 299 -
13.1.6 Peck Drilling Cycle (G83)
This cycle performs peck drilling.
It performs intermittent cutting feed to the bottom of a hole while
removing shavings from the hole.
Format
G83(G98) G83(G99)
G83 X_ Y_ Z_ R_ Q_ F_ L_ ;
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
L_ : Number of repeats (if required)
Initial level
d
Point Z
Point R
q
d
q
q
d
Point R level
q
d
q
q
Point R
Point Z
Explanation
- Operation
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.6211).
Be sure to specify a positive value in Q. Negative values are ignored.
- Spindle rotation
Before specifying G83, use a miscellaneous function (M code) to rotate
the spindle.
- Miscellaneous function
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.
When L 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.

Leave a Reply

Your email address will not be published.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