HEIDENHAIN TNC 360 User Manual - Manual (Page 108)

TNC 360 5-24
5 Programming Tool Movements
5.4 Path Contours – Cartesian Coordinates
X 5 0 e.g.
CT
Example for exercise: Circular arc connecting to a straight line
Coordinates of the
transition point from
the line to the arc:
X = 10 mm
Y = 40 mm
Coordinates of the
arc end point:
X = 50 mm
Y = 50 mm
Milling depth: Z = –15 mm
Tool radius: R = 20 mm
100
–15
100 40
50
10
50
Y
X
Z
90
Part program
0 BEGIN PGM 360524 MM ................................... 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+20 ...................................... Define the tool
4 TOOL CALL 2 Z S 1000 ...................................... Call the tool
5 L Z+100 R0 FMAX M6 ....................................... Insert the tool
6 L X+30 Y–30 FMAX ............................................ Pre-position the tool
7 L Z–15 FMAX M3
8 L X+50 Y+0 RL F100 .......................................... First contour point
9 L X+10 Y+40 ...................................................... Straight line connecting tangentially to the arc
10 CT X +50 Y +50 .................................................. Arc to end point with coordinates X = 50 mm and Y =
50 mm; Connects tangentially to the straight line in block 9
11 L X+100 .............................................................. End of contour
12 L X+130 Y+70 R0 FMAX
13 L Z+100 FMAX M2 ............................................. Retract tool and end program
14 END PGM 360524 MM
To program a circular path CT with tangential connection:
COORDINATES?
Enter the coordinates of the arc end point, for example IX = 50 mm,
IY = –10 mm.
If necessary, enter also:
• Radius compensation
• Feed rate
• Miscellaneous function
Resulting NC block: CT IX+50 IY-10 RR
Y +/ 1 0
ENT