CNC Z32 - Programming Guide (LATHES)
2.15.4
Suspending and resuming Tool change (G38, G39)
By programming
G39
it is possible to suspend the automatic execution of tool change.
When the function G39 is active, the M6 (tool change) is no more automatically executed, provoking instead a
machine STOP to allow the operator to manually change the tool. When the operator, after changing the tool,
presses the pushbutton START, the program will resume from the interruption point, and the tool change is
considered as done.
The programmed tool is thus considered in all its effects as already mounted on the spindle, with related acquisition
of its description, etc.
Example:
…
N10 G39
N12 T10 M6 (MANUALLY CHANGE WITH MILL R=10)
N13 G38
…
The function G39 is modal and it is deactivated by
G38
, which restores the automatic execution of tool change.
The function G38 is activated at reset.
2.15.5
Mounted tool reading (G104)
This function transfers the T value of the tool actually mounted on the spindle in the parameter HX.
The function is active only in the block where programmed.
Example:
…
N10 T101 M6
N11 G104
…
After execution of line N11, HX contains the value 101 (the tool actually mounted on the spindle is T101). If the
management for replacement tools is installed, and the tool actually mounted is a replacement for T101, the
parameter HX will contain the T code related to the tool actually mounted.
2.15.6
Real positions reading (G105)
The function
G105
transfers the physical measured positions in the axes position parameters, for all machine axes.
The function is active only in the block where programmed, with stop.
With G105 the measured positions (referred to the active origins and corrections) are transferred in the axes
position parameters. The positions transfer happens only for all continuous axes, including those not alive.
Warning:
The position transferred is the actual measured position, not the reference position. These two positions may differ
due to positioning errors (however very small to remain inside the positioning threshold).
For example, if X10 is commanded and the axis moves to position 9,998, G105 acquire the position 9,998 and not
10.
2.15.7
Radial programming (G106)
Modal, always active at reset for milling machines, canceled by G107.
This function is used in lathe machines when radial programming is desired. On milling machines the function is not
used, because automatically active at reset. After G106 the X axis and J parameter programming are considered
as radial. For an example, see G107,
31
Summary of Contents for CNC Z32 Florenz Series
Page 2: ......
