Siemens SINUMERIK 840D sl Programming Manual page 766

Work preparation
3.13 Tool offsets
Note
The G commands for selecting the 3D TRC are evaluated in the approach block, i.e. typically
in the block that contains G41 or G42.
G41 or G42 can also be programmed in blocks without traversing movement in geometry axes
relevant for the compensation. In this case, the approach block is the first traversing block
following such a block.
A change of the 3D TRC variant with active tool radius compensation is ignored without alarm.
Example
Program code
N10 $TC_DP1[1,1]=120
N20 $TC_DP6[1,1]=10
N30 $TC_DP15[1,1]=-3
...
; Processing with cylindrical milling tool and CUT3DCCD
N110 TRAORI
N120 A4=0 B4=0 C4=1
N130 X0 Y0 Z0 A0 C0 T1 D1 F20000
N140 X10 Y0 Z0 G41 CUT3DCCD CDOF2 G64
N150 X20
N160 X30 A45
N170 X40 A-45
N180 X55
N190 Y10 Z10
N200 Y20
N210 C45
N220 Y30 C90
N230 A5=-1 B5=0 C5=2 Y40
N240 Y50 G40
...
Further information
Tool type
The tool type (tool parameter $TC_DP1) is evaluated. Only milling tools with cylindrical shank
(cylinder or end mill, toroidal miller and, in the limit case, cylindrical die mill) are permitted. This
corresponds to the tool types 1 - 399, with the exception of the numbers 111 and 155 to 157.
766
Comment
; Cylindrical milling tool
; Activation of the transformation.
; Definition of the surface normal of the
limitation surface at the start of the
block.
; Activate 3D circumferential milling,
taking into account the limitation sur-
face + switching off collision detection.
; Obtuse angle ==> no infeed
; Acute angle ==> infeed
; Movement in the tool direction.
; Pure change in orientation.
; Change of the surface.
; Deactivation of the tool radius compen-
sation.
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming