HEIDENHAIN TNC 360 User Manual - Manual (Page 115)

5-31 TNC 360
5 Programming Tool Movements
5.5 Path Contours – Polar Coordinates
Example exercise: Milling a full circle
Circle radius: 50 mm
Circle center
coordinates:
X = 50 mm
Y = 50 mm
Milling depth: Z = – 5 mm
Tool radius: R = 15 mm
Part program
0 BEGIN PGM 360531 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z–20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+15
4 TOOL CALL 1 Z S1000
5 CC X+50 Y+50
6 L Z+100 R0 FMAX M6
7 LP PR+70 PA+280 FMAX
8 L Z–5 FMAX M3
9 LP PR+50 PA–90 RL F100
10 RND R10 ............................................................. Smooth approach
11 CP PA+270 DR– ................................................. Circle to end point PA = 270°, negative direction of rotation
12 RND R10 ............................................................. Smooth departure
13 LP PR+70 PA–110 R0 FMAX
14 L Z+100 FMAX M2
15 END PGM 360531 MM
–5
100
100
50
50
Y
X
Z
CC
General data and first contour point
Retract tool and end program