Siemens SINUMERIK 840D sl Programming Manual page 806

Work preparation
3.13 Tool offsets
Program code
N100 $TC_CARR10[2]=0 $TC_CARR11[2]=0
$TC_CARR12[2]=1
N110 $TC_CARR13[2]=0
N120 $TC_CARR14[2]=0
N130 $TC_CARR21[2]=X
N140 $TC_CARR22[2]=X
N150 $TC_CARR23[2]="M"
N160 TCOABS CUTMOD=0
N170 G18 T1 D1 TCARR=2
N180 X0 Y0 Z0 F10000
N190 $TC_CARR13[2]=30
N200 TCARR=2
N210 X0 Y0 Z0
N220 G42 Z–10
N230 Z–20
N240 X10
N250 G40 X20 Z0
N260 CUTMOD=2 X0 Y0 Z0
N270 G42 Z–10
N280 Z–20
N290 X10
N300 G40 X20 Z0
N310 M30
The numerical values in the comments specify the end of block positions in the machine coordinates
(MCS) in the sequence X → Y → Z.
Explanations
In block N180, initially the tool is selected for CUTMOD=0 and non-rotated tool holders that can
be orientated. As all offset vectors of the tool holder that can be orientated are 0, the position
that corresponds to the tool lengths specified in $TC_DP3[1,1] and $TC_DP4[1,1] is
approached.
The tool holder that can be orientated with a rotation of 30° around the B axis is activated in
block N200. As the cutting edge position is not modified due to CUTMOD=0, the old cutting edge
reference point is decisive just as before. This is the reason why in block N210 the position is
approached, which keeps the old tool nose reference point at the zero (i.e. the vector (1, 12) is
rotated through 30° in the Z/X plane).
In block N260, contrary to block N200, CUTMOD=2 is effective. As a result of the tool holder
rotation that can be orientated, the modified cutting edge position becomes 8. Deviating axis
positions also result from this.
The tool radius compensation (TRC) is activated in blocks N220 and/or N270. The different
cutting edge position in both program sections has no effect on the end positions of the blocks
806
Comment
; C axis
; X Y
; 12.000 0.000
; 10.892 0.000
; 8.696 0.000
; 8.696 0.000
; 12.696 0.000
; 30.892 0.000
; 8.696 0.000
; 8.696 0.000
; 8.696 0.000
; 12.696 0.000
; 28.696 0.000
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
Z
1.000
-5.134
–17.330
–21.330
–21.330
–5.134
–7.330
–17.330
–21.330
–21.330
–7.330
NC programming