Example: Contour Train - HEIDENHAIN TNC 640 User Manual

7

Example: Contour train

0 BEGIN PGM C25 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 1 Z S2000
4 L Z+250 R0 FMAX
5 CYCL DEF 14.0 CONTOUR
6 CYCL DEF 14.1 CONTOUR LABEL 1
7 CYCL DEF 25 CONTOUR TRAIN
Q1=-20
Q3=+0
Q5=+0
Q7=+250
Q10=5
Q11=100
Q12=200
Q15=+1
8 CYCL CALL M3
9 L Z+250 R0 FMAX M2
10 LBL 1
11 L X+0 Y+15 RL
12 L X+5 Y+20
13 CT X+5 Y+75
14 L Y+95
15 RND R7.5
16 L X+50
17 RND R7.5
18 L X+100 Y+80
19 LBL 0
20 END PGM C25 MM
256
;MILLING DEPTH
;ALLOWANCE FOR SIDE
;SURFACE COORDINATE
;CLEARANCE HEIGHT
;PLUNGING DEPTH
;FEED RATE FOR PLNGNG
;FEED RATE FOR MILLNG
;CLIMB OR UP-CUT
Fixed Cycles: Contour Pocket | Programming Examples
Definition of workpiece blank
Tool call: Diameter 20
Retract the tool
Define contour subprogram
Define machining parameters
Cycle call
Retract the tool, end program
Contour subprogram
HEIDENHAIN | User's manual for cycle programming | 10/2017