HEIDENHAIN TNC 310 (286 140) - Manual (Page 100)

7 Programming: Miscellaneous functions 88
The distance in each axis from the scale reference point to the
machine datum is defined by the machine tool builder in a machine
parameter.
Standard behavior
The TNC references coordinates to the workpiece datum (see
“Datum setting”).
Behavior with M91 — Machine datum
If you want the coordinates in a positioning block to be referenced
to the machine datum, end the block with M91.
The coordinate values on the TNC screen are referenced to the
machine datum. Switch the display of coordinates in the status
display to REF (see section 1.4 “Status Displays”).
Behavior with M92 — Additional machine datum
In addition to the machine datum, the machine tool
builder can also define an additional machine-based
position as a reference point.
For each axis, the machine tool builder defines the
distance between the machine datum and this additional
machine datum. Refer to the machine manual for more
information.
If you want the coordinates in a positioning block to be based on
the additional machine datum, end the block with M92.
Radius compensation remains the same in blocks that
are programmed with M91 or M92. The tool length,
however, is not compensated.
Effect
M91 and M92 are effective only in the blocks in which they are
programmed with M91 or M92.
M91 and M92 become effective at the start of block.
Workpiece datum
The figure at right shows coordinate systems with the machine
datum and workpiece datum.
Z
X
Y
Z
Y
X
M
7
.3 Miscellaneous F
unctions f
or Coor
dinat
e D
a
ta