Fanuc Series 15i/150i-MA (Programming) Operators Manual

B-63324EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 59 -
- Movement along axes not in the polar coordinate interpolation plane in the polar
coordinate interpolation mode
The tool moves along such axes normally, independent of polar
coordinate interpolation.
- Current position display in the polar coordinate interpolation mode
Actual coordinates are displayed. However, the remaining distance to
move in a block is displayed based on the coordinates in the polar
coordinate interpolation plane (Cartesian coordinates).
Limitation
- Coordinate system for the polar coordinate interpolation
Before G12.1 is specified, a local coordinate system (or workpiece
coordinate system) where the center of the rotary axis is the origin of
the coordinate system must be set. In the G12.1 mode, the coordinate
system must not be changed (G92, G52, G53, relative coordinate reset,
G54 through G59, etc.).
- Tool offset command
The polar coordinate interpolation mode cannot be started or
terminated (G12.1 or G13.1) in the tool offset mode (G41 or G42).
G12.1 or G13.1 must be specified in the tool offset canceled mode
(G40).
- Tool length offset command
Tool length offset must be specified in the polar coordinate
interpolation cancel mode before G12.1 is specified. It cannot be
specified in the polar coordinate interpolation mode. Furthermore, no
offset values can be changed in the polar coordinate interpolation
mode.
- Tool offset command
A tool offset must be specified before the G12.1 mode is set. No offset
can be changed in the G12.1 mode.
- Program restart
For a block in the G12.1 mode, the program cannot be restarted.
- Cutting feedrate for the rotation axis
Polar coordinate interpolation converts the tool movement for a figure
programmed in a Cartesian coordinate system to the tool movement in
the rotation axis (C-axis) and the linear axis (X-axis). When the tool
moves closer to the center of the workpiece, the C-axis component of
the feedrate becomes larger and may exceed the maximum cutting
feedrate for the C-axis (set in parameter (No. 1422)), causing an alarm
(see the warning below). To prevent the C-axis component from
exceeding the maximum cutting feedrate for the C-axis, reduce the
feedrate specified with address F or create a program so that the tool
(center of the tool when cutter compensation is applied) does not move
close to the center of the workpiece.

Leave a Reply

Your email address will not be published. Required fields are marked *