Siemens SINUMERIK 840D sl Programming Manual page 93

The programmed tool cutting speed is independent of path feedrate F and G function group 15
(feedrate type). The direction of rotation and the spindle start are implemented via M3 and M4,
and the spindle stop via M5.
A change to the tool radius data in the offset memory will be applied the next time a tool offset
is selected or the next time the active offset data is updated.
Changing the tool or selecting/deselecting a tool offset data set generates a recalculation of the
effective spindle speed.
Requirements
Programming of the tool cutting speed requires:
● The geometric ratios of a rotating tool (milling cutter or drilling tool)
● An active tool offset data set
Syntax
T... D... SVC[<n>]=<Value>
...
S... M3/M4
Meaning
SVC:
[<n>]:
<Value>:
T... D...:
S... M3/M4:
NC programming
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
Keyword for programming of the tool cutting speed
Number of spindle
This address extension specifies which spindle the programmed cutting speed
is to be applied for. In the absence of an address extension, the rate is always
applied to the master spindle.
Note:
A separate cutting speed can be preset for each spindle.
Note:
Programming SVC without an address extension requires that the master spin‐
dle has the active tool. If the master spindle changes, the user will need to select
a tool accordingly.
Value of tool cutting speed
Unit: m/min (for G71/G710) or ft/min (for G70/G700)
The tool radius must be established in the block with SVC. Thus, a correspond‐
ing tool including tool offset data block must either be active or selected in the
block. There is no fixed sequence for SVC and T/D selection during program‐
ming in the same block.
Programming of the spindle speed will effect deselection of the tool cutting
speed.
Note:
Switching between SVC programming and S programming is possible at any
time, even while the spindle is rotating. In each case, the value that is not active
is deleted.
Fundamentals
2.6 Spindle motion
93