HEIDENHAIN MANUALplus 4110 - Manual (Page 517)

HEIDENHAIN MANUALplus 4110 517
9.6 DIN Pr
ogr
amming Example "Thr
eaded St
ud"
DIN program "threaded stud"
%888.nc Program number of the DIN program
DIN example "threaded stud" Program description
N1 G14 Q1 Approach the tool change position, insert the roughing tool
N2 G96 S150 G95 F0.4 T1 Call roughing tool, program spindle speed and feed rate
N3 G0 X62 Z2 Approach the workpiece
N4 G819 P4 H0 I0.3 K0.1 "Longitudinal contour roughing with recessing" cycle
N5 G0 X13 Z0 Start point of contour description (for roughing cycle G819)
N6 G1 X16 Z-1.5 Contour definition
N7 G1 Z-30
N8 G25 H7 I1.15 K5.2 R0.8 W30 FP1.5 Undercut contour (an element of the contour description)
N9 G1 X20
N10 G1 X40 Z-35
N11 G1 Z-55 B4
N12 G1 X55 B-2
N13 G1 Z-70
N14 G1 X60
N15 G80 End of contour description (for roughing cycle G819)
N16 G14 Q1 Move to tool change point, insert finishing tool
N17 G96 S220 G95 F0.2 T2 Call finishing tool, program spindle speed and feed rate
N18 G0 X62 Z2 Approach the workpiece
N19 G89 Contour finishing cycle
N20 G42 Tool is to the left of the contour
N21 G0 X13 Z0 Starting point of contour description (for finishing cycle G89)
N22 G1 X16 Z-1.5 Contour definition
N23 G1 Z-30
N24 G25 H7 I1.15 K5.2 R0.8 W30 FP1.5 Undercut contour (an element of the contour description)
N25 G1 X20
N26 G1 X40 Z-35
N27 G1 Z-55 B4
N28 G1 X55 B-2
N29 G1 Z-70
N30 G1 X60
N31 G80 End of contour description (for finishing cycle G89)
N32 G14 Q1 Move to tool change point, insert threading tool
N33 G97 S800 T3 Call threading tool, program (constant) spindle speed
N34 G0 X16 Z2 Move to thread starting point
N35 G350 Z-29 F1.5 U-999 "Simple longitudinal single-start thread" cycle