Time-Controlled Commands; Dwell Time (G04) - Siemens Sinumerik 840D sl Programming Manual

3.3

Time-controlled commands

3.3.1

Dwell time (G04)

One can use G04 to interrupt workpiece machining between two NC blocks for a
programmed time/number of spindle revolutions, e.g. for backing off.
One can set with MD20734 $MC_EXTERN_FUNCTION_MASK, whether the dwell time for
Bit 2 is to be interpreted as time (s or ms) or alternatively as spindle revolutions. If
$MC_EXTERN_FUNCTION_MASK, Bit 2=1 is set, the dwell time is interpreted in seconds if
G94 is active; it is specified in spindle revolutions (R) if G95 is selected.
Format
G04 X_; or G04 P_;
X_: Time display (commas possible)
P_: Time display (commas not possible)
● The dwell time (G04 ..) must be programmed alone in a block.
If the values of X and U are programmed in the standard notation (without decimal point),
they are converted to internal units, depending on IS B, IS C (for input resolution, see
Chapter "Decimal point programming"). P is always interpreted in internal units.
N5 G95 G04 X1000
Standard notation: 1000*0.001 = 1 Spindle revolution
Calculator notation: 1000 spindle revolutions
ISO Milling
Programming Manual, 06/09, 6FC5398-7BP10-1BA0
Motion commands
3.3 Time-controlled commands
53