Tool Offset Call (D) - Siemens SINUMERIK 840D sl Programming Manual

5.6

Tool offset call (D)

Function
Cutting edges 1 to 8 (with active TOOLMAN 12) of a tool can be assigned different tool offset
data records (e.g. different offset values for the left and right cutting edge of a grooving tool).
Activation of the offset data (including the data for the tool length compensation) of a special
cutting edge is performed by calling the D number. When D0 is programmed, offsets for the
tool have no effect.
A tool radius compensation must also be activated via G41/G42.
Note
Tool length offsets take immediate effect when the D number is programmed. If no D number
is programmed, the default setting defined via the machine data is active for a tool change
( → see machine manufacturer's specifications).
Syntax
Activation of a tool offset data record:
D<number>
Activate the tool radius compensation:
G41 ...
G42 ...
Deactivation of the tool offsets:
D0
G40
Significance
D:
<number>:
D0:
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Command for the activation of an offset data record for the active tool
The tool length compensation is applied with the first programmed traverse
of the associated length compensation axis.
Notice:
A tool length compensation can also take effect without D programming,
when the automatic activation of a tool edge has been configured for the
tool change ( → see machine manufacturer's specifications).
The tool offset data record to be activated is specified via the <number>
parameter.
The type of D programming depends on the configuration of the machine
(see paragraph "Type of D programming").
Range of values: 0 - 32,000
Command for the deactivation of the offset data record for the active tool
Tool offsets
5.6 Tool offset call (D)
79