GSK GSK980TDc, Manual

Page: 64 / 470

GSK980TDc Turning CNC System User Manual
46
Ⅰ
Progra
mming
CHAPTER 3 G COMMANDS
3.1 Commands
G command consists of command address G and its following 1
～
2 bits command value, used
for defining the motion mode of tool relative to the workpiece, defining the coordinates and so on.
Refer to G commands as Fig. 3-1.
G □□
G words are divided into 9 groups (00, 01, 02, 03, 06
，
07
，
12
，
14
，
16
，
21). Except that commands
in the group 01 and 00 are not in the same block, G words in the different groups can be input to the
same block and the last one is valid when two or more G words in the same group are input. The
words in the different groups without the same parameter (word) can be in the same block and their
functions are valid without sequence at the same time. The system alarms when G words do not
belong to Table 3-1 or they are optional functions without being supplied.
Table 3-1 G command list
Word Group Function Remark
G00
01
Rapid traverse movement Initial modal G command
G01 Linear interpolation
Modal G commands
G02 Circular interpolation(CW)
G03 Circular interpolation(CCW)
G05 Three-point circular interpolation
G6.2 Ellipse interpolation (CW)
G6.3 Ellipse interpolation (CCW)
G7.2 Parabola interpolation (CW)
G7.3 Parabola interpolation (CCW)
G32 Thread cutting
G32.1 Rigid thread cutting
G33 Z tapping cycle
G34 Variable pitch thread cutting
G90 Axial cutting cycle
G92 Thread cutting cycle
G84 End rigid tapping
G88 Side rigid tapping
G94 Radial cutting cycle
G04
00
Dwell time preset
Non-modal G commands
G7.1 Cylinder interpolation
G10 Data input
G11 Data input cancel
G28 Machine reference point automatic return
G30 Machine 2nd, 3rd , 4th reference point
G31 Skip interpolation
G36 Automatic tool compensation X
G37 Automatic tool compensation Z
Command value
（
00
～
99
，
the leading zero can be omitted
）
Command address G