Mitsubishi Electric M700V Series Programming Manual page 84

6. Interpolation Functions
Detailed description
(1) Command G12.1 and G13.1 in an independent block. A program error (P33) will occur if this
command is issued in the same block as another G code.
(2) Linear interpolation or circular interpolation can be commanded during the pole coordinate
interpolation mode.
(3) The coordinates can be commanded with either an absolute command or incremental
command.
(4) Tool radius compensation can be applied on the program command. Pole coordinate
interpolation will be executed on the path after tool radius compensation.
(5) Command the segment feed in the pole coordinate interpolation plane (orthogonal coordinate
system) with F. The F unit is mm/min or inch/min.
(6) When the G12.1 command is issued, the deceleration check is executed.
(7) Plane selection
The linear axis and rotation axis used for pole coordinate interpolation must be set beforehand
with the parameters.
(a) Determine the deemed plane for carrying out pole coordinate interpolation with the
parameter (#1533) for the linear axis used for pole coordinate interpolation.
#1533 setting value
Blank (no setting)
(b) A program error (P485) will occur if the plane selection command (G16 to G19) is issued
during the pole coordinate interpolation mode.
(Note) Depending on the model or version, parameter (#1533) may not be provided. In this case,
the operation will be the same as if the parameter (#1533) is blank (no setting).
6.10 Polar Coordinate Interpolation; G12.1, G13.1
Deemed plane
X G17 (XY plane)
Y G19 (YZ plane)
Z G18 (ZX plane)
G17 (XY plane)
72