HEIDENHAIN ITNC 530 User Manual page 429

Example: Cylinder surface with Cycle 28
Notes:
Cylinder centered on rotary table
Datum at center of rotary table
Description of the midpoint path in the
contour subprogram
0 BEGIN PGM C28 MM
1 TOOL DEF 1 L+0 R+3.5
2 TOOL CALL 1 Y S2000
3 L Y+250 RO FMAX
4 L X+0 R0 FMAX
5 CYCL DEF 14.0 CONTOUR GEOMETRY
6 CYCL DEF 14.1 CONTOUR LABEL 1
7 CYCL DEF 28 CYLINDER SURFACE
Q1=-7 ;MILLING DEPTH
Q3=+0 ;ALLOWANCE FOR SIDE
Q6=2 ;SET-UP CLEARANCE
Q10=-4 ;INFEED DEPTH
Q11=100 ;FEED RATE FOR PLUNGING
Q12=250 ;FEED RATE FOR MILLING
Q16=25 ;RADIUS
Q17=1 ;DIMENSION TYPE
Q20=10 ;SLOT WIDTH
Q21=0.02 ;TOLERANCE
8 L C+0 R0 FMAX M3
9 CYCL CALL
HEIDENHAIN iTNC 530
Z
70
52.5
35
40
Define the tool
Call tool, tool axis is Y
Retract the tool
Position tool on rotary table center
Define contour subprogram
Define machining parameters
Remachining active
Pre-position rotary table
Call the cycle
60 157
C
429