Siemens SINUMERIK User Manual

Programming and Operating Manual (Turning)
01/2017
109
Remark:
If G94 instead of G95 was active before, a new appropriate F value must be written.
See the following illustration for constant cutting rate G96:
Rapid traverse
With rapid traverse G0, there is no change in speed.
Exception:
If the contour is approached at rapid traverse and the next block contains an interpolation type G1 or G2, G3,
CIP, CT (contour block), then the speed for the contour block is applied already in the approach block with G0.
Upper speed limit LIMS=
When machining from large to small diameters, the spindle speed can increase significantly. In this case, it is recommended
to program the upper spindle speed limitation LIMS=... . LIMS is only effective with G96 and G97.
By programming LIMS=..., the value entered into the setting data (SD43230: SPIND_MAX_VELO_LIMS) is overwritten. This
SD takes effect when LIMS is not written.
The upper limit speed programmed with G26 or defined via machine data cannot be overwritten with LIMS=.
Deactivate constant cutting rate: G97
The function "Constant cutting rate" is deactivated by G97. If G97 is active, a programmed
S word
is given in RPM as the
spindle speed
.
If no new S word is programmed, the spindle turns at the last defined speed with G96 function active.
Programming example
N10 M3 S1000
; Spindle's direction of rotation
N20 G96 S120 LIMS=2500
; Activate constant cutting speed, 120 m/min, speed limit 2,500
r.p.m.
N30 G0 X150
; no change in speed, because block N31 with G0
N40 X50 Z20
; no change in speed, because block N32 with G0
N50 X40
; Approach on contour, new speed is automatically set as is required
for the beginning of block N40
N60 G1 F0.2 X32 Z25
; Feedrate 0.2 mm/revolution
N70 X50 Z50
N80 G97 X10 Z20
; Deactivating constant cutting rate
N90 S600
; new spindle speed, r.p.m.
N100 M30
Information
The G96 function can also be deactivated with G94 or G95 (same G group). In this case, the last
programmed
spindle speed
S is active for the remaining machining sequence if no new S word is programmed.
The programmable offset TRANS or ATRANS (see Section "Programmable work offset: TRANS, ATRANS (Page 81)")
should not be used on the transverse axis X or used only with low values. The workpiece zero point should be located at the
turning center. Only then is the exact function of G96 guaranteed.

Siemens SINUMERIK Specifications

General

Interface	Ethernet, PROFIBUS, PROFINET, USB
Programming Languages	DIN/ISO
Display	TFT color display
Compatibility	Siemens drives and motors
Software	SINUMERIK Operate
Control Unit Type	CNC (Computer Numerical Control)
Safety Functions	Integrated safety functions up to SIL 3/PLe