Yx z cc – HEIDENHAIN TNC 360 User Manual User Manual
Page 103
5-19
TNC 360
5
Programming Tool Movements
5.4
Path Contours – Cartesian Coordinates
Example for exercise: Milling a full circle in one block
Circle center CC:
X
= 50 mm
Y
= 50 mm
Beginning and end
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 coordi-
nates 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
–5
50
50
Y
X
Z
CC