Xy z – HEIDENHAIN TNC 360 User Manual User Manual
Page 97
5-13
TNC 360
5
Programming Tool Movements
5.4
Path Contours – Cartesian Coordinates
Example for exercise: Chamfering a corner
Coordinates of the
corner points
E
:
X
= 95 mm
Y
=
5 mm
Chamfer length:
L
= 10 mm
Milling depth:
Z
= –15 mm
Tool radius:
R
= +10 mm
85
X
Y
Z
95
100
E
15
5
100
–15
Part program
0
BEGIN PGM 360513 MM ................................... Begin program
1
BLK FORM 0.1 Z X+0 Y+0 Z–20 ........................ Workpiece blank MIN point
2
BLK FORM X+100 Y+100 Z+0 ........................... Workpiece blank MAX point
3
TOOL DEF 5 L+5 R+10 ...................................... Tool definition
4
TOOL CALL 5 Z S500 ......................................... Tool call
5
L Z+100 R0 FMAX M6 ....................................... Retract spindle and insert tool
6
L X–10 Y–5 FMAX ............................................... Pre-position in X, Y
7
L Z–15 FMAX M3 ............................................... Pre-position to the working depth
8
L X+0 Y+5 RR F200 ............................................ Move with radius compensation (RR) and reduced feed (F200)
to the first contour point
9
L X+95 Y+5 ........................................................ Program the first straight line for corner E
10
L 10 ..................................................................... Chamfer block: inserts a chamfer with L = 10 mm
11
L X+95 Y+100 .................................................... Program the second straight line for corner E
12
L X+110 Y+110 R0 FMAX .................................. Retract the tool in X, Y (12) and Z (13); return to block 1 (13)
and end program
13
L Z+100 FMAX M2
14
END PGM 360513 MM