Simple Inclined Surface Machining Command; Outline - Mitsubishi Electric M800VW Series Programming Manual

M800V/M80V Series PLC Programming Manual (2/2)
14 PLC Help Function

14.26 Simple Inclined Surface Machining Command

14.26 Simple Inclined Surface Machining Command

14.26.1 Outline

In a lathe with three orthogonal axes and one rotary axis on the tool side, this function enables simultaneous 4-axis control
milling on an inclined surface along workpiece end face.
To facilitate machining on an inclined surface, this function uses three commands: simple inclined surface control (G176),
simple tool center point control (G174), and tool axis direction control (G53.1) as follows. The tool axis direction can be turned
at right angles to the inclined surface by issuing the tool axis direction control command (G53.1) after the simple inclined
surface control command (G176). When G174 is given after G176, the direction of tool length is compensated in accordance
with the tool angle.
For a machine configured with a turret, this function allows you to use any tool on the turret to carry out simple inclined surface
machining.
 Simple inclined surface control (G176)
G176 enables a new coordinate system (called "feature coordinate system") to be defined. Feature coordinate system is
obtained by rotating and parallel translating a plane using the X, Y and Z axes configuring the workpiece coordinate system as
a rotary axis. Consequently, there is no need to calculate the coordinate position in accordance with the inclined surface
angle. This simplifies creation of a machining program.
 Simple tool center point control (G174)
G174 allows a tool length offset in the tool axis direction even when the tool axis direction is not parallel to the orthogonal
coordinate system after rotation of the rotary axis. Consequently, the nose of the tool mounted on the rotary axis can be kept
in the programmed position at all times. This simplifies creation of a complicated-shape machining program.
 Tool axis direction control (G53.1)
G53.1 aligns the tool with the + Z direction of the feature coordinate system. This eliminates the need for you to mind the
feature coordinate system's direction or tool axis' rotation direction, resulting in greater ease of programming.
[Feature coordinate system]
X
Workpiece
coordinate system
(X', Y', Z')
Y'
For details of each G code command, refer to the programming manual.
IB-1501668-B
X"
Y"
Rotation center coordinate = Feature coordinate zero point
(X',Y',Z') = (0.0, 0.0, 100.0)
728
Z"
Rotation angle 45°
Z'
Feature coordinate
system
(X", Y", Z")