Programmable Data Input (G10); Changing Of Tool Offset Value; Setting The Workpiece Coordinate System Shift Data - Siemens SINUMERIK 802D sl Programming Manual

Enhanced Level Commands

4.2 Programmable data input (G10)

4.2 Programmable data input (G10)
4.2.1

Changing of tool offset value

Existing tool offsets can be overwritten by using the G10. New tool offsets, howe-
ver, cannot be created.
Format
G10 L10 P... R... ; Tool length compensation, geometry
G10 L11 P... R... ; Tool length compensation, wear
G10 L12 P... R... ; Tool radius compensation, geometry
G10 L13 P... R... ; Tool radius compensation, wear
P: Number of the compensation memory
R: Specifies the value
L1 can be programmed instead of L11.
Relevant machine data
Machine data 20382 $MC_TOOL_CORR_MOVE_MODE defines whether the com-
pensation is applied in the block containing the selection or the next time the axis is
programmed.
Machine data 20270 $MC_CUTTING_EDGE_DEFAULT = 0 defines that no tool
length compensation is active initially on a tool change.
Setting data $SC_TOOL_LENGTH_CONST must contain the value 17 for the as-
signment of tool length offsets to geometry axes to be independent of the plane
selection. Length 1 is then always assigned to the Z axis.
4.2.2

Setting the workpiece coordinate system shift data

With the commands of "G10 P00 X (U) ⋅⋅⋅ Y (V) ⋅⋅⋅ Z (W) ⋅⋅⋅ ;", it is possible
to write and update the workpiece coordinate system shift data using a part pro-
gram. If an address is omitted in the designation of data input block, the offset
amounts for the omitted addresses remain unchanged.
4-132
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
X, Z, C : Absolute or incremental setting data of the workpiece
coordinate system shift amount
U, W, H : Incremental setting data of the workpiece coordinate
system shift amount
© Siemens AG 2007 All rights reserved
04.07