HEIDENHAIN TNC 620 Programming Station

Programming contours | Path contours — Cartesian coordinates
5
Example: Circular movements with Cartesian coordinates
0 BEGIN PGM CIRCULAR MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
Define the workpiece blank for the machining simulation
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 1 Z S4000
Tool call with spindle axis and spindle speed
4 L Z+250 R0 FMAX
Retract the tool in the spindle axis at rapid traverse FMAX
5 L X-10 Y-10 R0 FMAX
Pre-position the tool
6 L Z-5 R0 F1000 M3
Move to working depth at feed rate F=1000mm/min
7 APPR LCT X+5 Y+5 R5 RL F300
Approach the contour at point1 on a circular path with
tangential connection
8 L X+5 Y+85
Program the first straight line for corner2
9 RND R10 F150
Program a rounding with R= 10mm, feed rate F=150mm/
min
10 L X+30 Y+85
Move to point 3: starting point of the circular path CR
11 CR X+70 Y+95 R+30 DR-
Move to point 4: end point of the circular path CR, with radius
R= 30mm
12 L X+95
Move to point 5
13 L X+95 Y+40
Move to point 6: starting point of the circular path CT
14 CT X+40 Y+5
Move to point 7: end point of the circular path CT, arc with
tangential connection to point6; the control calculates the
radius automatically
15 L X+5
Move to last contour point 1
16 DEP LCT X-20 Y-20 R5 F1000
Depart contour on a circular path with tangential connection
17 L Z+250 R0 FMAX M2
Retract the tool, end program
18 END PGM CIRCULAR MM
166
HEIDENHAIN | TNC620 | Klartext Programming User's Manual | 01/2022