Siemens SINUMERIK 840D sl Function Manual page 710

W5: 3D tool radius compensation
19.3 Face milling
The shaft characteristics are not taken into account on any of the tool types. For this reason,
the two tool types 120 (end mill) and 155 (bevel cutter), for example, have an identical
machining action since only the section at the tool tip is taken into account. The only
difference between these tools is that the tool shape is represented differently (dimensions).
Figure 19-14 Tool types for face milling
The tool data are stored under the following tool parameter numbers:
Table 19-2
Tool data
d
r
a
Note
The geometry and wear values of a tool data are added.
The reference point for tool length compensation (also referred to as tool tip or tool center
point (TCP)) on all tool types is the point at which the longitudinal axis of the tool penetrates
the surface.
A new tool with different dimensions may be programmed only when the tool compensation is
activated for the first time (i.e. on transition from G40 to G41 or G42) or, if the compensation is
already active, only when G41 or G42 are reprogrammed.
In contrast to circumferential milling, therefore, there are no variable tool dimensions in one
block.
This restriction applies only to the tool shape (tool type, dimensions d, r and a).
A change in tool involving only a change in other tool data (e.g. tool length) is permitted
provided that no other restrictions apply. An alarm is output if a tool is changed illegally.
710
Tool parameter numbers for tool data
Geometry
$TC_DP6
$TC_DP7
$TC_DP11
Wear
$TC_DP15
$TC_DP16
$TC_DP20
Function Manual, 09/2011, 6FC5397-2BP40-2BA0
Special Functions