Siemens Sinumerik 840D sl Programming Manual page 87

Program code
N270 SVC[1]=300
...
Further information
Tool radius
The following tool offset data (associated with the active tool) affect the tool radius when:
● $TC_DP6 (radius - geometry)
● $TC_DP15 (radius - wear)
● $TC_SCPx6 (offset for $TC_DP6)
● $TC_ECPx6 (offset for $TC_DP6)
The following are not taken into account:
● Online radius compensation
● Allowance on the programmed contour (OFFN)
Tool radius compensation (G41/G42)
Although tool radius compensation (G41/G42) and SVC both refer to the tool radius, with regard
to function, they are not linked and are independent of one another.
Tapping without compensating chuck (G331, G332)
SVC programming is also possible in conjunction with G331 or G332.
Synchronized actions
SVC cannot be programmed from synchronized actions.
Reading the cutting rate and the spindle speed programming variant
The cutting rate of a spindle and the speed programming variant (spindle speed S or cutting
rate SVC) can be read using system variables:
● With preprocessing stop in the part program via system variables:
● Without preprocessing stop in the part program via system variables:
Fundamentals
Programming Manual, 01/2015, 6FC5398-1BP40-5BA2
Comment
; S1 = (300 m/min * 1,000) / (9.0 mm * 2 * 3.14) =
5307.86 rpm.
S3 = (50 m/min * 1,000) / (9.0 mm * 2 * 3.14) = 884.64 rpm.
$AC_SVC[<n>]
$AC_S_TYPE[<n>]
Cutting rate applied when the current main run record for spindle
number <n> was preprocessed.
Spindle speed programming variant applied when the current
main run record for spindle number <n> was preprocessed.
Value: Meaning:
1 Spindle speed S in rpm
2 Cutting rate SVC in m/min or ft/min
Spindle motion
7.2 Cutting rate (SVC)
87