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

PROGRAMMING
20. HIGH SPEED CUTTING FUNCTIONS
B–62764EN/01
452
When bit 1 of parameter MSU No. 8403 is set to 1, G00, M, S, T, and B
codes can be specified even in HPCC mode. When specifying these codes
in HPCC mode, note the following:
(1) When a G00, M, S, T, or B code is specified in cutter compensation
mode, the offset vector created in the previous block is maintained.
(Example 1) When the following program is executed for
machining with offset value D1 set to 10 mm, the start
point of N6 is determined by the vector created
between N3 and N4:
N1
N2
N3
N4
N5 N6
N7
N8
O0001 ;
G92 G90 X–10. Y20. ;
G05 P10000 ;
N1 G01 G42 X0 D1 F1000 ;
N2 X20. ;
N3 X40. Y0 ;
N4 X60. Y20 ;
N5 M01 ;
N6 X80. ;
N7 X90. Y–20. ;
N8 G40 Y–50. ;
G05 P0 ;
M30
This vector is used as the vector
between N4 and N6.
Programmed path
Tool path
An incorrect offset value is
used in this range.
(Example 2) When the following program is executed for
machining with offset value D1 set to 10 mm, the start
point of N5 is determined by the vector created
between N3 and N4. If the simplified G00 execution
function is enabled (by setting bit 7 of parameter SG0
No. 8403 to 1), a correct vector can be obtained at the
intersection of N4 and N5.
N1
N2
N3
N4
N5
N6
N7
O0001 ;
G92 G90 X–10. Y20. ;
G05 P10000 ;
N1 G01 G42 X0 D1 F1000 ;
N2 X20. ;
N3 X40. Y0 ;
N4 X60. Y20 ;
N5 G00 X80. ;
N6 G01 X90. Y–20. ;
N7 G40. Y–50. ;
G05 P0 ;
M30
This vector is used as the vector between
N4 and N5, and N5 and N6.
Programmed path
Tool path
An incorrect offset value is
used in this range.
D Positioning and auxiliary
functions

Leave a Reply

Your email address will not be published.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