Siemens SINUMERIK 802D sl Programming Manual page 122

Enhanced Level Commands
4.1 Program support functions (1)
Explanations
Rapid traverse is performed to point R after positioning along the X and Y axes.
Tapping is carried out from point R to point Z. The spindle is stopped and a dwell is
performed once tapping has been completed. Subsequently, the spindle is rotated
in the normal direction. The tool is retracted to point R, and the spindle is stopped.
Rapid traverse to the initial level is then carried out.
The feedrate override and the spindle override are supposed to be 100% while tap-
ping is being carried out.
The speed of rotation, however, can be controlled through GUD _ZSFI[2] during
retraction. Example: _ZSFI[2]=120, the retraction takes place with 120% of the tap-
ping speed.
Thread lead
The thread lead is obtained from the expression 'feedrate spindle speed' in feed--
per--minute mode. The thread lead equals the feedrate speed when in feed--per--
revolution mode.
Tool length compensation
The offset is applied at the time of positioning to point R whenever a tool length
compensation (G43, G44, or G49) is specified in the canned cycle.
Axis switching
The canned cycle must always be canceled before the drilling axis can be chan-
ged. An alarm is issued if the drilling axis is changed into rigid mode.
S command
An alarm is issued if a speed that is higher than the maximum speed for the gear
currently in use is specified.
F command
An alarm is issued if a value overshooting the upper limit of cutting feedrate is spe-
cified.
Unit of F command
G94
G95
4-122
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
Metric input
1 mm/min 0.01 inch/min
0.01 mm/rev 0.0001 inch/rev
Inch input Remarks
Decimal point pro-
gramming allowed
Decimal point pro-
gramming allowed
© Siemens AG 2007 All rights reserved
04.07