Programming Example For Turning Application - Siemens SINUMERIK 840DE Programming Manual
Hide thumbs
Also See for SINUMERIK 840DE:
- Operation & programming manual (233 pages) ,
- User manual (100 pages) ,
- Function manual (2184 pages)
Table of Contents
Advertisement
Fundamental Principles of NC Programming
2.6 Programming example for turning application
2.6
Programming example for turning application
Radius programming and tool radius compensation
The sample program contains radius programming and tool radius compensation.
Programming example
%_N_1001_MPF
N5 G0 G53 X280 Z380 D0
N10 TRANS X0 Z250
N15 LIMS=4000
N20 G96 S250 M3
N25 G90 T1 D1 M8
N30 G0 G42 X-1.5 Z1
N35 G1 X0 Z0 F0.25
N40 G3 X16 Z-4 I0 K-10
N45 G1 Z-12
N50 G2 X22 Z-15 CR=3
N55 G1 X24
N60 G3 X30 Z-18 I0 K-3
N65 G1 Z-20
N70 X35 Z-40
N75 Z-57
N80 G2 X41 Z-60 CR=3
N85 G1 X46
N90 X52 Z-63
N95 G0 G40 G97 X100 Z50 M9
N100 T2 D2
N105 G96 S210 M3
N110 G0 G42 X50 Z-60 M8
N115 G1 Z-70 F0.12
N120 G2 X50 Z-80 I6.245 K-5
N125 G0 G40 X100 Z50 M9
N130 G0 G53 X280 Z380 D0 M5
N135 M30
2-26
;Start point
;Zero offset
;Speed limitation (G96)
;Select constant cutting speed
;Select tool and offset
;Activate tool with tool radius compensation
;Rotate radius 10
;Rotate radius 3
;Rotate radius 3
;Rotate radius 3
;Deselect tool radius compensation and approach
tool change location
;Call up tool and select offset
;Select constant cutting speed
;Activate tool with tool radius compensation
;Rotate diameter 50
;Rotate radius 8
;Retract tool and deselect tool radius
compensation
;Move to tool change location
;Program end
Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1
Fundamentals
Advertisement
Table of Contents
