HEIDENHAIN TNC 360 ISO Programming - Manual (Page 173)

8-20
8 Cycles
TNC 360
Fig. 8.17: Points of intersection S
1
and S
2
of
pockets A and B
8.3 SL Cycles
B
Right pocket
A B
S
1
S
2
A
Left pocket
Fig. 8.18: Outline is machined first Fig. 8.19: Surface is machined first
.
.
.
.
.
.
Cycle in a part program
%S820I G71 * ............................................................ Begin program
N10 G30 G17 X+0 Y+0 Z–20 * ................................... Define workpiece blank
N20 G31 X+100 Y+100 Z+0 *
N30 G99 T1 L+0 R+3 * .............................................. Tool definition
N40 T1 G17 S2500 * .................................................. Tool call
N50 G37 P01 1 P02 2 * .............................................. Define in cycle CONTOUR GEOMETRY that the contour
elements are described in subprograms 1 and 2
N60 G57 P01 –2 P02 –15 P03 –8 P04 100 P05 +0
P06 +0 P07 500 * ....................................................... Cycle definition ROUGH-OUT
N70 G00 G40 G90 Z+100 M06 * ............................... Retract the spindle, insert the tool
N80 X+50 Y+50 M03 * .............................................. Pre-positioning in the X/Y plane, spindle ON
N90 Z+2 M99 * .......................................................... Pre-positioning in Z to setup clearance, cycle call
N100 Z+100 M02 *
N110 G98 L1 *
N140 G98 L0 *
N150 G98 L2 *
N180 G98 L0 *
N9999 %S820I G71 *
Subprograms: Overlapping pockets
The pocket elements A and B overlap.
The control automatically calculates the points of intersection S1 and S2,
so these points do not have to be programmed.
The pockets are programmed as full circles.
N110 G98 L1 *
N120 G01 G41 X+10 Y+50 *
N130 I+35 J+50 G03 X+10 Y+50 *
N140 G98 L0 *
N150 G98 L2 *
N160 G01 G41 X+90 Y+50 *
N170 I+65 J+50 G03 X+90 Y+50 *
N180 G98 L0 *
N9999 % S820I G71 *
Depending on the control setup (machine parameters), machining starts
either with the outline or the surface: