HEIDENHAIN TNC 620 User Manual page 451

The PLANE function: Tilting the working plane (software option 8) 12.2
Specifying the positioning behavior of the PLANE
function
Overview
Independently of which PLANE function you use to define the tilted
machining plane, the following functions are always available for
the positioning behavior:
Automatic positioning
Selection of alternate tilting possibilities (not with PLANE AXIAL)
Selection of the type of transformation (not with PLANE AXIAL)
Danger of collision!
If you work with Cycle 28 MIRRORING in a tilted
system, please note the following:
If you program mirroring before the tilting of the
working plane, the mirroring also effects the tilting.
Exception: Tilting with Cycle 19 and AXIAL PLANE.
Mirroring a rotary axis with Cycle 28 only mirrors the
motions of the axis, but not the angles defined in the
PLANE functions. As a result, the positioning of the
axes changes.
Automatic positioning: MOVE/TURN/STAY (entry is
mandatory)
After you have entered all parameters for the plane definition,
you must specify how the rotary axes will be positioned to the
calculated axis values:
The PLANE function is to automatically position
the rotary axes to the calculated position values.
The position of the tool relative to the workpiece
is to remain the same. The TNC carries out a
compensation movement in the linear axes
The PLANE function is to automatically position
the rotary axes to the calculated position values,
but only the rotary axes are positioned. The TNC
does not
the linear axes
You will position the rotary axes later in a separate
positioning block
If you have selected the MOVE option (PLANE function is to position
the axes automatically), the following two parameters must still be
defined: Dist. tool tip – center of rot. and Feed rate? F =.
If you have selected the option TURN (PLANE function is to position
the axes automatically), the following parameter must still be
defined Feed rate? F =.
If you use PLANE together with STAY, you have to
position the rotary axes in a separate block after the
PLANE function.
Dist. tool tip – center of rot. (incremental): The TNC tilts the
tool (or table) relative to the tool tip. The DIST parameter shifts
the center of rotation of the positioning movement relative to
the current position of the tool tip.
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
carry out a compensation movement on
12
451