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

PROGRAMMING
B–62764EN/01
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
177
When the tool reaches the bottom of a hole, the tool may be returned to
point R or to the initial level. These operations are specified with G98 and
G99. The following illustrates how the tool moves when G98 or G99 is
specified. Generally, G99 is used for the first drilling operation and G98
is used for the last drilling operation.
The initial level does not change even when drilling is performed in the
G99 mode.
G98(Return to initial level ) G99(Return to point R level)
Initial level
Point R level
To repeat drilling for equally–spaced holes, specify the number of repeats
in K_.
K is effective only within the block where it is specified.
Specify the first hole position in incremental mode (G91).
If it is specified in absolute mode (G90), drilling is repeated at the same
position.
Number of repeats K The maximum command value = 9999
If K0 is specified, drilling data is stored, but drilling is not performed.
To cancel a canned cycle, use G80 or a group 01 G code.
Group 01 G codes
G00 : Positioning (rapid traverse)
G01 : Linear interpolation
G02 : Circular interpolation or helical interpolation (CW)
G03 : Circular interpolation or helical interpolation (CCW)
Subsequent sections explain the individual canned cycles. Figures in
these explanations use the following symbols:
Dwell
P
OSS
Positioning (rapid traverse G00)
Cutting feed (linear interpolation G01)
Manual feed
Shift (rapid traverse G00)
Oriented spindle stop
(The spindle stops at a fixed rotation position)
D Return point level
G98/G99
D Repeat
D Cancel
D Symbols in figures

Leave a Reply

Your email address will not be published.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