Siemens SINUMERIK 840D sl Programming Manual page 101

The SZS position of the face axis (radius) is the basis for calculating the spindle speed from the
programmed cutting rate.
Note
Frames between WCS and SZS (e.g. programmable frames such as SCALE, TRANS or ROT)
are taken into account in the calculation of the spindle speed and can bring about a change in
speed (for example, if there is a change in the effective diameter in the case of SCALE).
Speed limitation LIMS
If a workpiece that varies greatly in diameter needs to be machined, it is advisable to specify a
speed limit for the spindle with LIMS (maximum spindle speed). This prevents excessively high
speeds with small diameters. LIMS is only applied if G96, G961 and G97 are active. LIMS is not
applied if G971 is selected. On loading the block into the main run, all programmed values are
transferred into the setting data.
Note
The speed limits changed with LIMS in the part program are taken into the setting data and
therefore remain saved after the end of program.
However, if the speed limits changed with LIMS are no longer to apply after the end of program,
the following definition must be inserted in the GUD block of the machine manufacturer:
REDEF $SA_SPIND_MAX_VELO_LIMS PRLOC
Deactivating the constant cutting rate (G97/G971/G972/G973)
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 (respectively G961 or
G962) is retained.
The G96/G961 function can also be deactivated with G94 or G95. In this case, the last speed
programmed S... is used for subsequent machining operations.
G97 can be programmed without G96 beforehand. The function then has the same effect as
G95; LIMS can also be programmed.
Using G973, the constant cutting rate can be deactivated without activating a spindle speed
limitation.
Note
The transverse axis must be defined in machine data.
Rapid traverse G0
With rapid traverse G0, there is no change in speed.
Exception:
If the contour is approached in rapid traverse and the next NC block contains a G1/G2/G3/...
path command, the speed is adjusted in the G0 approach block for the next path command.
Other reference axis for G96/G961/G962
NC programming
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
Fundamentals
2.6 Spindle motion
101