Tool Offsets; Spindle Motion; Feed Control; Program Header - Siemens SINUMERIK 840D sl Programming Manual

3.3

Program header

The NC blocks that are placed in front of the actual motion blocks for the machining of the
workpiece contour, are called the program header.
The program header contains information/statements regarding:
• Tool change
•

Tool offsets

•

Spindle motion

•

Feed control

• Geometry settings (zero offset, selection of the working plane)
Program header for turning
The following example shows the typical structure of an NC program header for turning:
Program code
N10 G0 G153 X200 Z500 T0 D0
N20 T5
N30 D1
N40 G96 S300 LIMS=3000 M4 M8
N50 DIAMON
N60 G54 G18 G0 X82 Z0.2
...
Program header for milling
The following example shows the typical structure of an NC program header for milling:
Program code
N10 T="SF12"
N20 M6
N30 D1
N40 G54 G17
N50 G0 X0 Y0 Z2 S2000 M3 M8
...
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Comment
; Retract toolholder before tool turret is
rotated.
; Swing in tool 5.
; Activate cutting edge data record of the tool.
; Constant cutting rate (Vc) = 300 m/min, speed
limitation = 3000 rpm, direction of rotation
counterclockwise, cooling on.
; X axis will be programmed in diameter.
; Call zero offset and working plane, approach
starting position.
Comment
; Alternative: T123
; Trigger tool change
; Activate cutting edge data record of the tool
; Zero offset and working plane
; Approach to the workpiece, spindle and coolant
on
Creating an NC program
3.3 Program header
47