Siemens SINUMERIK 840D sl Programming Manual page 94

Fundamentals
2.6 Spindle motion
Note
SVC programming is not possible if the following spindle feedrate movements are active:
● Constant cutting speed: G96/G961/G962 S... (Page 98)
● Constant grinding wheel peripheral speed: SUG (Page 103)
● Position spindle: SPOS/SPOSA/M19 (Page 117)
● ; Switch master spindle over to axis mode: M70 (Page 117)
Conversely, programming one of these functions will effect a deselection of SVC (tool cutting
speed).
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
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: Tool carrier = 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
94
Comment
; Selection of milling tool with, e.g.
$TC_DP6[1,1] = 6 (tool radius = 6 mm)
; Cutting speed = 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
; Tool and offset data set selection together with
SVC in block (no specific sequence).
; Spindle start with CW direction of rotation, cut-
ting speed 100 m/min
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming