Siemens Sinumerik 840D sl Programming Manual page 84

Spindle motion
7.2 Cutting rate (SVC)
Note
Changing between SVC and S
Changing between SVC and S programming is possible at will, even while the spindle is turning.
In each case, the value that is not active is deleted.
Note
Maximum tool speed
System variable $TC_TP_MAX_VELO[<tool number>] can be used to preset a maximum tool
speed (spindle speed).
If no speed limit has been defined, there will be no monitoring.
Note
SVC programming is not possible if the following are active:
● G96/G961/G962
● GWPS
● SPOS/SPOSA/M19
● M70
Conversely, programming one of these commands will lead to the deselection of SVC.
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 SVC programming.
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
84
Comment
; Selection of milling tool with, e.g.
$TC_DP6[1,1] = 6 (tool radius = 6 mm)
; Cutting rate = 100 m/min
Resulting spindle speed:
S = (100 m/min * 1000) / (6.0 mm * 2 * 3.14) =
2653.93 rpm
; SVC and tooth feedrate
Comment
Programming Manual, 01/2015, 6FC5398-1BP40-5BA2
Fundamentals