System information

SECTION FOUR - PREPARATORY FUNCTIONS (G CODES)

Notes on Circular and Linear Milling

The feedrate in circular and linear is equal to the feedrate specified by the F address. This

feedrate is the tangential feedrate along the arc and the vector feed on the linear moves.

Note 1: I0, J0, and K0 can be omitted.

Note 2: If X, Y, and Z are all omitted – or if the end point is located at the same position

as the start point and the center is commanded by I, J and K – an arc of 360° (a

complete circle) is assumed.

G02I _____; (a complete circle)

G02 R____

When only R is used, an arc of 0° is programmed.

G02R _____; (The cutter does not move.)

Note 3: The feedrate is measured along the arc after the cutter compensation is applied.

Note 4: If I, J, K, and R addresses are specified simultaneously, the arc radius specified

by address I, J, K takes precedence and the R is ignored.

Note 5: The X Y Z I J K R AA AB commands are retained by the control. If an

interpolation block is left incomplete, the missing axis information will be

defaulted to the value previously entered.

Helical cutting (G02, G03)

Helical interpolation is enabled by specifying another axis which moves synchronously with the

circular interpolation. That is, the tool can be moved helically.

G17 or X____ Y____ or Z____ F____;

G03 I____ J____

G18 or X____ Z____ or Y____ F____;

G03 I____ K____

G02 R____

G19 or Y____ Z____ or X____ F____;

G03 J____ K____

214