Programming - Siemens SINUMERIK 840D Function Manual

To ensure that the reference axis for G96 / G961 / G962 is retained during a reset, end of part
program or start of part program, the following setting must be made:
● Channel reset or part program end: MD20110 $MC_RESET_MODE_MASK, bit 18 = 1
● Part program start: MD20112 $MC_START_MODE_MASK, bit 18 = 1
A reference axis for G96 / G961 / G962 can also be assigned without the parameterization of
a transverse axis in MD20100 via SCC[AX]. For this scenario, the constant cutting speed must
not already be activated with G96. For additional information, see the following:
Further information
Programming Manual Fundamentals, Feedrate Control and Spindle Motion
"Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC)
4.3

Programming

Transverse axes can be programmed with respect to both diameter and radius. Generally, they
are diameter-related, i.e. programmed with doubled path dimension so that the corresponding
dimensional information can be transferred to the part program directly from the technical
drawings.
Figure 4-2
Switching the diameter programming on/off
Channel-specific diameter programming
The activating or deactivating of the diameter programming is done via the modally active part
program statements of the G group 29:
● DIAMON: Diameter programming ON
● DIAMOF: Diameter programming OFF, in other words, radius programming ON
● DIAM90: Diameter or radius programming depending on the reference mode:
– Diameter programming ON in connection with absolute dimensioning G90
– Radius programming ON in connection with incremental dimensioning G91
● DIAMCYCOF: Radius programming for G90 and G91 ON, for the HMI, the last active G
command of this group remains active
Axes and spindles
Function Manual, 06/2019, A5E47437747B AA
Transverse axis with diameter information (D1, D2)
P1: Transverse axes
4.3 Programming
121