To Next Page

To Previous Page

Enhanced Level Commands

4.1 Program support functions (1)

04.07

4-108

SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition

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; Rotate spindle.

G90G0Z100

G90 G99 G83 X200. Y--150. Z--100. R50. Q10. F150.;

Position, drill hole 1, and return to point R.

Y--500.; Position, drill hole 2, and return to point R.

Y--700.; Position, drill hole 3, and return to point R.

X950.; Position, drill hole 4, and return to point R.

Y--500.; Position, drill hole 5, and return to point R.

G98 Y--700.; Position, drill hole 6, and return to the initial level.

G80; Cancel canned cycle

G28 G91 X0 Y0 Z0; Return to the reference position return

M5; Spindle stop

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).

06.01

Siemens SINUMERIK 802D sl Programming Manual

Other manuals for Siemens SINUMERIK 802D sl