Sinumerik 810 CNC Mill Radius/Chamfer Program Example

Siemens Sinumerik 810 cnc mill programming example which shows how cnc machinists can machine/program Radius and Chamfer.

Sinumerik 810 Radius/Chamfer Programming

U+ values are used for Radius programming.
U- values are used for Chamfer programming.

Sinumerik 810 Radius/Chamfer Programming Example

Sinumerik 810 CNC Mill Radius Chamfer Program

Sinumerik 810 CNC Mill Radius Chamfer Program

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 X40 Y0 U5
N45 X40 Y30 U8
N50 X70 Y30 U-2
N55 X70 Y50 U-2
N60 X0 Y50 U6
N65 X0 Y0
N70 G40 X-20 Y-20
N80 G00 Z50
N85 Y100
N90 M30

Finished Part

After completing the above machining process, component will look like this,

Finished Component

Finished Component

Explanation of Codes Used in Program

G00 : Rapid traverse.
G54 : Zero Offset no. 1.
G64 : Continuous-path mode.
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 : Axises motion feed
M : Cutter motion (3=clockwise, 4=anti-clockwise)
D : Tool no
M30 : End of main program