User's Manual TNC 360 (from 259 900-11) - heidenhain

5 Programming Tool Movements
5.4 Path Contours – Cartesian Coordinates
5-22
Example for exercise: Milling a concave semicircle
Semicircle radius:
Coordinates of the
R = 50 mm
arc starting point: X = 0
Coordinates of the
Y = 0
arc end point: X = 100 mm
Y = 0
Tool radius: R = 25 mm
Milling depth: Z = 18 mm
Part program
Y
100
50
–18
–20
0 BEGIN PGM 360522 M ...................................... Begin program
1 BLK FORM 0.1 Z X+0 Y+0 Z–20 ........................ Define the workpiece blank
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 2 L+0 R+25 ...................................... Define the tool
4 TOOL CALL 2 Z S2000 ....................................... Call the tool
5 L Z+100 R0 FMAX M6 ....................................... Insert and pre-position the tool
6 L X+25 Y–30 FMAX
7 L Z–18 FMAX M3
8 L X+0 Y+0 RR F100 ............................................ First contour point
9 CR X+100 Y+0 R+50 DR– .................................. Mill circular arc CR to the end point X = 100 mm, Y = 0; radius
R = 50 mm, negative direction of rotation
10 L X+70 Y–30 R0 FMAX
11 L Z+100 FMAX M2
12 END PGM 360522 MM ...................................... Retract the tool and end the program
Z
100
X
TNC 360