Sinumerik 810 Programming Example CNC Mill

Siemens Sinumerik 810 programming example to show how cnc machinists can machine corner Radius.

Sinumerik 810 CNC control uses U+ for radius (see example below).
Sinumerik 810 CNC control uses U- for chamfer.
U must be any positive numeric value like e.g U5, this will draw a radius of 5 mm.

For tool offset setting on Sinumerik 810 read Work Offset Setting on Hermle UWF 851 CNC Mill with Sinumerik Control

This cnc programming example works on,


Sinumerik 810 Programming Example

Sinumerik 810 Programming Example

Sinumerik 810 Programming Example

N5 G00 G54 G64 G90 G17 X-20 Y-20 Z50
N10 S450 M03 F250 D01 (12.5 MM DIA)
N15 C0
N20 Z5
N25 G01 Z0
N30 Z-5
N35 G42 X0 Y0
N40 X10 Y10 U4
N45 X80 Y0 U8
N50 X100 Y20 U8
N55 X60 Y80 U7
N60 X40 Y80 U7
N65 X30 Y55 U8
N70 X0 Y40 U20
N80 X0 Y0
N85 G40 X-20 Y-20
N90 G00 Z50
N95 Y100
N100 M30

Explanation of Sinumerik 810 G-Codes

G00 : Rapid traverse.
G54 : Zero Offset no. 1.
G64 : Continuous-path operation.
G90 : Absolute dimensioning system.
G17 : X-Y plan selection.
G42 : Cutter radius compensation activation (right hand side movement)
G40 : Cutter radius compensation de-active
S   : Spindle speed
F   : Axis motion feed
M   : Cutter motion (3=clockwise, 4=anti-clockwise)
D   : Tool no
M30 : End of main program