
09 00.11.21 K.Yamamuro Revised to edition 09
08 00.06.22 T.Watanabe Revised to edition 08 T.Endo
01 99.03.10 K.Yamamuro New-registered T.Endo
A-63537E
ED DATE DESIG.
DESCRIPTION 10/134
SHEET
TITLE
FANUC Series 16i/18 i -TA
Compound Machining Function
TITLE
CUST.DRAW.NO.
Though the following G codes are handled in the same manner, the system
must be cancelled (switching to OFF) before changing command modes.
Otherwise, the P/S alarm 5253 occurs.
G10/G11 Programmable data input ON/OFF
G12.1/G13.1 Polar coordinate interpolation ON/OFF
G15/G16 Polar coordinate command ON/OFF
G22/G23 Stored stroke check function ON/OFF
G25/G26 Spindle speed fluctuation detection ON/OFF
G40.1/G41.1/G42.1 Normal direction control ON/OFF
G40/G41/G42
Tool nose radius compensation, Cutter compensation
ON/OFF
G43/G44/G49 Tool length compensation ON/OFF
G50/G51 Scaling ON/OFF
G50.2/G51.2 Polygon turning ON/OFF
G68/G69 Coordinate system rotation ON/OFF
G66/G67 Macro modal call ON/OFF
G96/G97 Constant surface speed control ON/OFF
G73 - G89 Canned cycle for drilling ON/OFF
2.2.2 F code
F codes for both command modes are also independent the same as G codes.
They cannot be common especially because the values have different
meanings depending on the current mode (feed/min. or feed/rev.), increment
unit and so on.
For example, the F code commanded in turning mode is valid only for the
mode and never affects the milling mode’s.
Example)
O0002 ;
N10 M80 ; ←Turning mode start
N20 M03 S300 ;
N30 G01 G42 X100. Z100. F10. ; ←Tool nose R compensation valid
(G42 mode)
N40 X200. Z200. ;
N50 M81 ; ←Milling mode start
P/S alarm 5253 occurs
because tool nose R compensation is
still effective.
N60 Z200. ;
Example)
O0003 ;
N10 M80 ; ←Turning mode start
N20 M03 S300 ;
N30 G99 G01 X130. F10. ; ←10.0000 mm/rev.
N40 M81 ; ←Milling mode start
N50 G01 X200. F600 ; ←600.000 mm/min.
N60 M80 ; ←Turning mode start