Spindle Motion - Siemens SINUMERIK 828D Programming Manual

Note
The tool paths of "standard tools" generated e.g. using CAD systems which already take the
tool radius into account and only contain the deviation from the standard tool in the tool nose
radius are not supported in conjunction with
Examples
The following shall apply to all examples: Toolholder = spindle (for standard milling)
Example 1: Milling cutter 6 mm radius
Program code
N10 G0 X10 T1 D1
N20 SVC=100 M3
N30 G1 X50 G95 FZ=0.03
...
Example 2: Tool selection and SVC in the same block
Program code
N10 G0 X20
N20 T1 D1 SVC=100
N30 X30 M3
N40 G1 X20 F0.3 G95
Example 3: Defining cutting rates for two spindles
Program code
N10 SVC[3]=100 M6 T1 D1
N20 SVC[5]=200
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
programming.
SVC
Comment
; Selection of milling cutter with e.g.
$TC_DP6[1,1] = 6 (tool radius = 6 mm)
; Cutting rate = 100 m/min
⇒ Resulting spindle speed:
S = (100 m/min * 1,000) / (6.0 mm * 2 * 3.14) =
2653.93 rpm
; SVC and tooth feedrate
Comment
; Tool and offset data record selection together with
SVC in block (no specific sequence)
; Spindle start with CW direction of rotation,
cutting rate 100 m/min
; SVC and revolutional feedrate
Comment
; The tool radius of the active tool offset is the
same for both spindles. The effective speed is
different for spindle 3 and spindle 5.

Spindle motion

6.2 Cutting rate (SVC)
97