Siemens SINUMERIK 802D sl Programming Manual page 108

Enhanced Level Commands
4.1 Program support functions (1)
Drilling
Drilling is not performed in a block that does not contain X, Y, Z, R, or any other
axes.
Cancel
G codes of group 01 (G00 to G03) and G83 must not be specified in a single block.
Otherwise, G83 is canceled.
Tool offset
Tool offsets are ignored in the canned cycle mode.
Example
M3 S2000;
G90 G0 Z100
G90 G99 G83 X200. Y--150. Z--100. R50. Q10. F150.;
Y--500.;
Y--700.;
X950.;
Y--500.;
G98 Y--700.;
G80;
G28 G91 X0 Y0 Z0; Return to the reference position return
M5;
After reaching the programmed depth of cut for each cutting feed Q, retraction to
reference level R is performed in rapid traverse. Approach movement for a rene-
wed cut is again carried out in rapid traverse up to a distance (d) which is set to
GUD7_ZSFR[10]. Distance d and the depth of cut for each cutting feed Q are tra-
versed with cutting feed. Specify Q incrementally implemented without sign.
Note
If _ZSFR[10]
S > 0 = value is used for anticipation distance "d" (distance minimal 0.001)
S = 0 The anticipation distance is 30 mm, the value of the anticipation distance is
always 0,6 mm. For larger drilling depths, the formula drilling depth/50 is used
(maximum value 7 mm).
4-108
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
Rotate spindle.
Position, drill hole 1, and return to point R.
Position, drill hole 2, and return to point R.
Position, drill hole 3, and return to point R.
Position, drill hole 4, and return to point R.
Position, drill hole 5, and return to point R.
Position, drill hole 6, and return to the initial level.
Cancel canned cycle
Spindle stop
© Siemens AG 2007 All rights reserved
04.07
06.01