Mitsubishi Electric M700V Series Programming Manual page 89

6. Interpolation Functions
(11) A program error (P486) will occur if the cylindrical interpolation or the pole coordinate
interpolation is commanded during the pole coordinate interpolation mode.
(12) During pole coordinate interpolation, if X axis moveable range is controlled in the plus side, X
axis has to be moved to the plus area that includes "0" and above before issuing the polar
coordinate interpolation command. If X axis moveable range is controlled in the minus side, X
axis has to be moved to the area that does not include "0" before issuing the polar coordinate
interpolation command.
Example of program
N07
<Program>
:
N01 G17 G90 G0 X40.0 C0 Z0;
N02 G12.1;
N03 G1 G42 X20.0 F2000;
N04 C10.0;
N05 G3 X10.0 C20.0 R10.0;
N06 G1 X-20.0;
N07 C-10.0;
N08 G3 X-10.0 C-20.0 I10.0 J0;
N09 G1 X20.0;
N10 C0;
N11 G40 X40.0;
N12 G13.1;
:
:
M30 ;
6.10 Polar Coordinate Interpolation; G12.1, G13.1
Hypothetical C axis
C axis
N05
N06
N08 N09
Hypothetical C axis
C axis
Tool
N04
N01
N03
N02
X axis
N10 N11
Path after tool radius compensation
Program path
Setting of start position
Polar coordinate interpolation mode: Start
Actual machining start
Shape program
(Command the position with the orthogonal
coordinate on X-C hypothetical axis plane.)
Polar coordinate interpolation mode: Cancel
77
X axis
Z axis