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

5 Programming Tool Movements
5.4 Path Contours – Cartesian Coordinates
TNC 360
Example for exercise: Milling a full circle in one block
Circle center CC: X = 50 mm
Beginning and end
Y = 50 mm
of a circle center C: X = 50 mm
Y = 0 mm
Milling depth: Z = –5 mm
Tool radius: R = 15 mm
Part program
0 BEGIN 360519 MM ............................................ Begin program
1 BLK FORM 0.1 Z X+0 Y+0 Z–20 ........................ Define workpiece blank
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 6 L+0 R+15 ...................................... Define tool
4 TOOL CALL 6 Z S500 ......................................... Call tool
5 CC X+50 Y+50 .................................................... Coordinates of the circle center CC
6 L Z+100 R0 FMAX M6 ....................................... Insert tool
7 L X+50 Y–40 FMAX ............................................ Pre-position the tool
8 L Z–5 FMAX M3
9 L X+50 Y+0 RL F100 .......................................... Move under radius compensation to the first contour point
10 RND R10 ............................................................. Smooth approach
11 C X+50 Y+0 DR– ................................................ Mill circular arc C around circle center CC; end point coordinates
X = +50 mm and Y = 0; negative direction of rotation
12 RND R10 ............................................................. Smooth departure
13 L X+50 Y–40 R0 FMAX
14 L Z+100 FMAX M2
15 END PGM 360519 MM ...................................... Retract tool and end program
Y
50
–5
Z
CC
50
X
5-19