Circular Interpolation Programming Example 2

Although this example drawing looks a bit complex, but it is very easy to program. Before going through this exercise you must fist read circular interpolation articles

Circular Interpolation Concepts & Programming articles

and exercise no. 1

After reading that you will be comfortable to understand this program example. it is very simple and basic work.

Circular Interpolation Programming Example 2

Circular Interpolation Programming Example 2

Circular Interpolation Programming Example 2

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 M08
N40 X80 Y0 
N45 X60 Y30 U10 
N50 X80 Y50 
N55 X50 Y50 
N60 G02 X30 Y30 U20 
N65 G01 X10 Y30 U8
N70 X0 Y0
N75 G40 X-20 Y-20 
N80 G00 Z50 M09
N85 Y100
N90 M30

Finished Part
After completing the machining process, your job will look like this.

Completed Part

Completed Part

Explanation of CNC G-Code

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
G02 : Circular Interpolation clockwise
G03 : Circular Interpolation anti-clockwise (counter clockwise)
S : Spindle speed
F : Axis motion feed
M : Cutter motion (3=clockwise, 4=anti-clockwise)
D : Tool no
M08 : Coolant on
M09 : Coolant off
M30 : End of main program