Meaning
G96: Revolutional feedrate (as for G95 (Page 105)) and constant cutting speed
G95 is activated automatically with G96. If G95 has not been activated previously, a new
feedrate value F... has to be specified when G96 is called.
G961: Linear feedrate (as for G94 (Page 105)) and constant cutting speed
G962: Linear feedrate or revolutional feedrate and constant cutting speed
S...: In conjunction with G96, G961 or G962, S... is not interpreted as a spindle speed but
rather as a cutting speed. The cutting speed is always applied to the master spindle.
Unit: m/min (for G71/G710) or ft/min (for G70/G700)
Range of values: 0.1 m/min to 9999 9999.9 m/min
G97: Revolutional feedrate and constant spindle speed (constant cutting speed OFF)
G971: Linear feedrate and constant spindle speed (constant cutting speed OFF)
G972: Linear feedrate or revolutional feedrate and constant spindle speed (constant cutting
speed OFF)
G973: Revolutional feedrate without spindle speed limitation and constant spindle speed (G97
without LIMS for ISO mode)
Note:
After G97 (or G971 ... G973), S... is again interpreted as a spindle speed in rpm. In the
absence of a new spindle speed being specified, the last speed set with G96 (respec‐
tively G961 or G962) is retained.
LIMS: Speed limitation for the master spindle (only applied if G96/G961/G97 active)
On machines with selectable master spindles, limitations of differing values can be
programmed for up to four spindles within one block.
<spindle>: Number of spindle
<value>: Spindle speed upper limit in rpm
SCC: If any of the G96/G961/G962 functions are active, SCC[<axis>] can be used to assign
any geometry axis as a reference axis.
Note
If G96/G961/G962 is selected for the first time, a constant cutting speed S... must be entered;
if G96/G961/G962 is selected again, the entry is optional.
Note
The speed limitation programmed with LIMS must not exceed the speed limit programmed with
G26 or defined in the setting data.
Note
The reference axis for G96/G961/G962 must be a geometry axis assigned to the channel at the
time when SCC[<axis>] is programmed. SCC[<axis>] can also be programmed when any of
the G96/G961/G962 functions are active.
Fundamentals
2.6 Spindle motion
NC programming
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0 99
To Next Page
Loading...
Need help?
General
