Siemens SINUMERIK 808D Function Manual

Function Manual
180 01/2017
– Definition of a tool with a maximum of nine cutting edges (offset blocks) through D number
– Cutting edge is described by tool parameters:
Tool type
Geometry: Length/radius
Wear: Length/radius
Cutting edge position (for turning tools)
● Tool change selectable: Immediately with T command or through M6
● Tool radius compensation
– Compensation active for all interpolation types: linear and circular
– Compensation at outer corners selectable: transition circle (G450) or equidistant intersection (G451)
– Automatic detection of outer/inner corners
Reference:
SINUMERIK 808D/SINUMERIK 808D ADVANCED Programming and Operating Manual
19.2
Tool
Select a tool
A tool is selected in the program with the T function. Whether the new tool is immediately loaded with the T function or with
M6 depends on the setting in MD22550 TOOL_CHANGE_MODE (new tool offset with the M function).
Value range of T
The T function can assume integer values from T0 (no tool) to T32000 (tool with the number 32000).
Up to 64 tools can be stored in the control system simultaneously.
19.3
Tool offset
Tool compensation through D function
A tool can have up to nine cutting edges. The nine tool cutting edges are assigned to the D functions D1 to D9.
Up to 128 data fields (D numbers) for tool compensation blocks can be stored in the control system simultaneously.
The tool cutting edge is programmed with D1 (edge 1) to D9 (edge 9). The tool cutting edge always refers to the currently
active tool. An active tool cutting edge (D1 to D9) without an active tool (T0) is inactive. Tool cutting edge D0 deselects all
tool offsets of the active tool.
Selection of the cutting edge when changing tool
When a new tool (new T number) has been programmed and the old one replaced, the following options are available for
you to select the cutting edge:
● The cutting edge number is programmed
● The cutting edge number is not programmed D1 is active automatically.
Activating the tool offset
D1 to D9 activates the tool compensation (offset) for a cutting edge on the active tool. Tool length compensation and tool
radius compensation can be activated at different times:
● Tool length compensation (TLC) is performed on the first traversing motion of the axis on which the TLC is to act. This
traversing motion must be a linear interpolation (G0, G1).
● Tool radius compensation (TRC) becomes active when G41/G42 is programmed in the active plane (G17, G18 or G19).
The selection of tool radius compensation with G41/G42 is only permitted in a program block with G0 (rapid traverse) or
G1 (linear interpolation).
Reference:
SINUMERIK 808D/SINUMERIK 808D ADVANCED Programming and Operating Manual

Siemens SINUMERIK 808D Specifications

General

Brand	Siemens
Model	SINUMERIK 808D
Category	Control Unit
Language	English