HEIDENHAIN TNC 407 (280 580) ISO Programming User Manual
Page 277
8-57
8
Cycles
TNC 426/TNC 425/TNC 415 B/TNC 407
Activation
Cycle G80 becomes effective immediately after definition in part program-
ming. If the function TILTING PROGRAM RUN is set to ACTIVE in the
MANUAL mode (see page 2-26), the angular value entered in this menu
is overwritten by Cycle G80.
Input data
ROTARY AXIS AND TILT ANGLE:
The tilted axes of rotation together with the associated tilt angles.
The axes A, B and C are programmed using soft keys.
Entering an axis of rotation together with the associated tilt angle in Cycle G80 does not cause movement of the axis.
The axis must be positioned to the required angle – for example with a G00 block.
Cancellation
To cancel Cycle G80, program G80 without entering an axis of rotation.
Pre-positioning
The following note applies to the TNC 426:
The machine manufacturer determines whether Cycle G80 positions the axes of rotation automatically or whether
they must be pre-positioned in the part program. Your machine manual provides more detailed information.
If the axes are positioned automatically in Cycle G80:
• The TNC can only position controlled axes
• You can only use preset tools (with the full tool length defined in the
G99 block or in the tool table)
• The position of the tool tip as referenced to the workpiece surface
remains nearly unchanged after tilting
• The TNC tilts the working plane at the last programmed feed rate. The
maximum feed rate that can be reached depends on the complexity of
the swivel head or tilting table.
If the axes are not positioned automatically in Cycle G80, position them
before defining the cycle, for example with a G00 block.
NC blocks
G00 G40 G90 Z+100*
X+25 Y+10*
G01 A+15 F1000
Pre-position in axis of
rotation
G80 A+15*
Define angle for compensat-
ing the slant
G00 G40 Z+80*
Activate compensation for
Z axis
X–7.5 Y–10*
Activate compensation for
X/Y axes