Siemens SINUMERIK 840D sl Programming Manual page 86

Fundamentals
2.5 Tool offsets
Example 3: Change of programming version from TOFFL to TOFF
The active tool is a milling tool. The active plane is G17.
Program code
N10 TOFFL[1]=3 TOFFL[3]=5
N20 TOFFL[2]=4
N30 TOFF[Z]=1.3
Example 4: Assignment of the offset values after a plane change
Program code
N10 $TC_DP1[1,1]=120
N20 $TC_DP3[1,1]= 100
N30 T1 D1 G17
N40 TOFF[Z]=1.0
N50 G0 X0 Y0 Z0
N60 G18 G0 X0 Y0 Z0
N70 G17
N80 TOFFL=1.0
N90 G0 X0 Y0 Z0
N100 G18 G0 X0 Y0 Z0
In this example, the offset of 1 mm in the Z axis is retained when changing to G18 in block N60;
the effective tool length in the Y axis is the unchanged tool length of 100 mm.
However, in block N100, the offset is effective in the Y axis when changing to G18 as it was
assigned to tool length L1 in the programming, and this length component is effective in the Y
axis with G18.
Example 5: Simultaneous tool length offset and tool radius offset
a, end milling cutter without corner rounding (tool type 120):
Program code
...
TOFFLR=0.1
...
b, end mill with corner rounding (tool type 121):
Program code
...
TOFFLR=0.1
...
86
Comment
; Effective offsets: L1=3, L2=0, L3=5
; Effective offsets: L1=3, L2=4, L3=5
; Effective offsets: L1=0, L2=0, L3=1.3
Comment
; Tool length L1=100 mm.
; Offset in Z direction (corresponds to L1 for G17).
; Machine axis position X0 Y0 Z101
; Machine axis position X0 Y100 Z1.
; Offset in L1 direction (corresponds to Z for G17).
; Machine axis position X0 Y0 Z101.
; Machine axis position X0 Y101 Z0.
Comment
; Effective offsets:
; Tool length offset (L1) = 5
; Tool radius offset = 5
Comment
; Effective offsets:
; Tool length offset (L1) = 0.1
; Tool radius offset = 0.1
; Offset corner radius = 0.1
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming