GSK GSK988TA, Manual

Page: 69 / 531

Chapter 2 G Commands
51
Ⅰ
Programming
……….;
N500 M30;
Note 1: When the system is turned on or resets, the polar coordinate interpolation is cancelled (G13.1); G12.1
and G13.1 are modal;
Note 2: The axis undefined by the parameter does not execute the polar coordinate interpolation in spite of
specifying the movement value in the polar coordinate interpolation mode;
Note 3: The used plane (selected by G17, G18 or G19) before G12.1 is cancelled; after G13.1 cancels the polar
coordinate interpolation, the plane recovers; when the system resets, the polar coordinate
interpolation is cancelled and the system uses the plane;
Note 4: In the polar coordinate interpolation mode, the program codes use the rectangular coordinate code in
the polar coordinate plane. The linear axis in the plane uses the diameter or radius programming and
the turn axis uses the radius programming;
Note 5: The arc interpolation executing the arc radius address is determined by the linear axis of the
interpolation plane in the polar coordinate interpolation plane as follows:
Use I and J when the linear axis is X or its parallel axis, and the turn axis uses J;
Use J and K when the linear axis is X or its parallel axis, and the turn axis uses J;
Use K and I when the linear axis is Z or its parallel axis, and the turn axis uses I;
Also use R code;
Note 6: Must set a workpiece coordinate system before using G12.1, the center of the turn axis is the origin of
the coordinate system. The coordinate system must not be changed in G12.1 mode.
Note 7: Cannot start or cancel the polar coordinate interpolation mode; code G12.1 or G13.1 in G40; otherwise,
an alarm occurs;
Note 8: When the tool traverses near to the workpiece center in the polar coordinate interpolation mode, C
weight of feedrate changes, which exceeds max. C cutting speed to cause an alarm;
Note 9: The program code uses the rectangular coordinate code in the polar coordinate plane. The axis
address of the turn axis is taken as the one of the 2nd axis (imaginary axis) in the plane.
Note 10: The current position displays the actual coordinates in the polar coordinate interpolation. However,
the remainder distance is displayed according to the coordinates in the polar coordinate
interpolation plane (rectangular coordinate plane);
Note 11: When the system executes G12.1, the tool position of the polar coordinate interpolation starts from
the angle 0. So, the spindle must be positioned before the polar coordinate interpolation is
executed;
Note 12: Must not switch the spindle gear in the polar coordinate interpolation. The system must be in the
spindle speed control mode when the gear shifting is needed.
2.10 Metric/Inch Switch G20, G21
Command function: G code selects the metric or inch system.
Command format: G20; inch input
G21; metric input
Command explanation: G20/G21 must be specified in a single block before a program begins to
set a coordinate system.
After metric/inch switch G code is specified, unit of input data is changed into least inch/metric