HEIDENHAIN ITNC 530 User Manual page 283

Automatic compensation of machine geometry
when working with tilted axes: M114 (software
option 2)
Standard behavior
The TNC moves the tool to the positions given in the part program. If
the position of a tilted axis changes in the program, the resulting offset
in the linear axes must be calculated by a postprocessor and traversed
in a positioning block. As the machine geometry is also relevant, the
NC program must be calculated separately for each machine tool.
Behavior with M114
The machine manufacturer must enter the machine
geometry in kinematic tables.
If the position of a controlled tilted axis changes in the program, the
TNC automatically compensates the tool offset by a 3-D length
compensation. As the geometry of the individual machine tools is set
in machine parameters, the TNC also compensates machine-specific
offsets automatically. Programs only need to be calculated by the
postprocessor once, even if they are being run on different machines
with TNC control.
If your machine tool does not have controlled tilted axes (head tilted
manually or positioned by the PLC), you can enter the current valid
swivel head position after M114 (e.g. M114 B+45, Q parameters
permitted).
The radius compensation must be calculated by a CAD system or by a
postprocessor. A programmed radius compensation RL/RR will result
in an error message.
If the tool length compensation is calculated by the TNC, the
programmed feed rate refers to the point of the tool. Otherwise it
refers to the tool datum.
If your machine tool is equipped with a swivel head that
can be tilted under program control, you can interrupt
program run and change the position of the tilted axis, for
example with the handwheel.
With the RESTORE POS. AT N function, you can then
resume program run at the block at which the part
program was interrupted. If M114 is active, the TNC
automatically calculates the new position of the tilted axis.
If you wish to use the handwheel to change the position
of the tilted axis during program run, use M118 in
conjunction with M128.
Effect
M114 becomes effective at the start of block, M115 at the end of
block. M114 is not effective when tool radius compensation is active.
To cancel M114, enter M115. At the end of program, M114 is
automatically canceled.
HEIDENHAIN iTNC 530
B
B
Z
dx
dB
dz
X
283