Programmable Data Input (G10); Changing The Tool Offset Value; Working Area Limitation (G22, G23) - Siemens Sinumerik 840D sl Programming Manual

Additional functions

4.2 Programmable data input (G10)

4.2 Programmable data input (G10)
4.2.1

Changing the tool offset value

Existing tool offsets can be overwritten via G10. It is not possible to create new tool offsets.
Format
G10 L10 P... R... ; Tool length compensation, geometry
G10 L11 P... R... ; Tool length compensation, wear and tear
G10 L12 P... R... ; Tool radius compensation, geometry
G10 L13 P... R... ; Tool radius compensation, wear and tear
P: Number of tool offset memory
R: Value statement
L1 can also be programmed instead of L11.
4.2.2

Working area limitation (G22, G23)

G22/G23
G22/G23 limits the working area (working area, working space) in which the tool can
traverse, limited to the channel axis. The areas outside the working area limitations defined
with G22/G23 are inhibited for any tool movement.
While using the commands G22 and G23, a protection zone as per the setting in the
machine data must be available and it must be active.
18190 $MN_NUM_PROTECT_AREA_NCK = 1
28210 $MC_NUM_PROTECT_AREA_ACTIVE = 1
Further, the following machine data must be set:
18190 $MN_NUM_PROTECT_AREA_NCK = 2 (minimum)
28210 $MC_NUM_PROTECT_AREA_ACTIVE = 2 (minimum)
One upper limit (G23) and a lower limit (G22) is defined for each axis for the working area.
These values are effective right away and they remain active even after RESET or POWER
ON.
Consideration of the tool radius must be activated separately. This takes place over
MD21020 $MC_WORKAREA_WITH_TOOL_RADIUS.
If the tool reference point lies outside the working area limitation defined by the working
space or if this area is left, the program sequence is stopped.
110
Programming Manual, 06/09, 6FC5398-7BP10-1BA0
ISO Milling