Siemens SINUMERIK 840D sl Programming Manual page 1018

Work preparation
3.24 User stock removal programs
Explanation of the column contents:
Line 0 Coding for the starting point:
Lines 1-n: Entries for contour pieces
Further information
Permitted traversing commands, coordinate system
The following G groups and G commands can be used for the contour programming:
G group 1:
G group 10:
G group 11:
G group 13:
G group 14:
G group 15:
In addition, the following are possible:
● Rounding and chamfer
● Circle programming using CIP and CT
The spline, polynomial and thread functions result in errors.
Changes to the coordinate system by activating a frame are not permissible between
CONTDCON and EXECUTE. The same applies for a change between G70 and G71 or G700 and
G710.
Replacing the geometry axes with GEOAX while preparing the contour table produces an alarm.
1018
Column 0: 10 (ones digit): G0 = 0
0
10 (tens digit): G70 = 0, G71 = 1, G700 = 2, G710 = 3
1
Column 1: Starting point abscissa
Column 2: Starting point ordinate
Column 3-4: 0
Column 5: Line index of last contour piece in the table
Column 0: 10 (ones digit): G0 = 0, G1 = 1, G2 = 2, G3 = 3
0
10 (tens digit): G70 = 0, G71 = 1, G700 = 2, G710 = 3
1
10 (hundreds digit): G90 = 0, G91 = 1
2
10 (thousands digit): G93 = 0, G94 = 1, G95 = 2, G96 = 3
3
10 (ten thousands digit): G60 = 0, G44 = 1, G641 = 2, G642 = 3
4
10 (hundred thousands digit): G9 = 1
5
Column 1: End point abscissa
Column 2: End point ordinate
Column 3: Center point abscissa for circular interpolation
Column 4: Center point ordinate for circular interpolation
Column 5: Feedrate
G0, G1, G2, G3
G60, G64, G641, G642
G9
G70, G71, G700, G710
G90, G91
G93, G94, G95, G96, G961
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming