HEIDENHAIN TNC 640 (34059x-05) Cycle programming - Manual (Page 237)

Programming Examples 8.6
8
TNC 640 | User's Manual Cycle Programming | 1/2015
237
Example: Cylinder surface with Cycle 28
Cylinder centered on rotary table
Machine with B head and C table
Datum at center of rotary table
Description of the midpoint path in the
contour subprogram
Y (Z)
X (C)
0 BEGIN PGM C28 MM
1 TOOL CALL 1 Z S2000
Tool call, tool axis Z, diameter 7
2 L Z+250 R0 FMAX Retract the tool
3 L X+50 Y+0 R0 FMAX
Position tool at rotary table center
4 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN FMAX
Tilting
5 CYCL DEF 14.0 CONTOUR GEOMETRY
Define contour subprogram
6 CYCL DEF 14.1 CONTOUR LABEL 1
7 CYCL DEF 28 CYLINDER SURFACE
Define machining parameters
Q1=-7 ;MILLING DEPTH
Q3=+0 ;ALLOWANCE FOR SIDE
Q6=2 ;SET-UP CLEARANCE
Q10=-4 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR PLNGNG
Q12=250 ;FEED RATE FOR MILLING
Q16=25 ;RADIUS
Q17=1 ;DIMENSION TYPE
Q20=10 ;SLOT WIDTH
Q21=0.02 ;TOLERANCE Remachining active
8 L C+0 R0 FMAX M3 M99 Pre-position rotary table, spindle ON, call the cycle
9 L Z+250 R0 FMAX
Retract the tool
10 PLANE RESET TURN FMAX
Tilt back, cancel the PLANE function
11 M2
End of program
12 LBL 1 Contour subprogram, description of the midpoint path
13 L X+60 Y+0 RL Data for the rotary axis are entered in mm (Q17=1)
14 L Y-35
15 L X+40 Y-52.5
16 L Y-70
17 LBL 0
18 END PGM C28 MM