HEIDENHAIN TNC 320 - Example: Contour Train

Fixed Cycles: Contour Pocket
7.12 Programming Examples
7
216
HEIDENHAIN | TNC 320 | User’s manual for cycle programming | 9/2016
Example: Contour train
0 BEGIN PGM C25 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
Definition of workpiece blank
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 1 Z S2000
Tool call: Diameter 20
4 L Z+250 R0 FMAX
Retract the tool
5 CYCL DEF 14.0 CONTOUR
Define contour subprogram
6 CYCL DEF 14.1 CONTOUR LABEL 1
7 CYCL DEF 25 CONTOUR TRAIN
Define machining parameters
Q1=-20 ;MILLING DEPTH
Q3=+0 ;ALLOWANCE FOR SIDE
Q5=+0 ;SURFACE COORDINATE
Q7=+250 ;CLEARANCE HEIGHT
Q10=5 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR PLNGNG
Q12=200 ;FEED RATE FOR MILLNG
Q15=+1 ;CLIMB OR UP-CUT
8 CYCL CALL M3
Cycle call
9 L Z+250 R0 FMAX M2
Retract the tool, end program
10 LBL 1
Contour subprogram
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