Siemens SINUMERIK 840D sl Programming Manual page 94

Spindle motion
6.2 Cutting rate (SVC)
Syntax
SVC[<n>]=<value>
Note
In the block with SVC, the tool radius must be known; in other words, a corresponding tool
including a tool offset data record must be active or selected in the block. There is no fixed
sequence for SVC and T/D selection during programming in the same block.
Significance
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.
94
Cutting rate
Number of spindle
[<n>]:
This address extension specifies which spindle the programmed
cutting rate 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 rate can be preset for each spindle.
Note:
Programming SVC without an address extension requires that the
master spindle has the active tool. If the master spindle changes,
the user will need to select a tool accordingly.
Unit: m/min or ft/min (dependent upon G700/G710)
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Fundamentals