Specifications

_____________________________________________________________________

CONCISE GUIDE FANUC 110

7.4 PROGRAMMING IN REAL CO-ORDINATES

When functions M37 and G28 C0 (M237 and G28 A0 on machines with back spindle option) the machine

prepares to work in “real co-ordinates”.

X….. Z…… C (A)……

Where :

• X => Absolute co-ordinate of axis X, is to be programmed with a diametrical value.

• Z => Absolute co-ordinate of axis Z.

• C => Co-ordinate for axis C positioning on main spindle.

• A => Co-ordinate for axis C positioning on back spindle.

The positive direction corresponds to the spindle direction of rotation (M4). Code C is programmed as an

angle value in degrees up to a maximum of the third decimal digit.

Example: N51 G0 C180.123

Axis C, used in real co-ordinates makes it possible to drill front and radial holes, make front and radial

tapping, key seats, front concentric slots and helical milling on the workpiece outer diameter.

To make an incremental displacement of axis C, function H…. can be used.

Example: N32 G0 H90 (axis C moves incrementally by 90 degrees in relation to the point where it is

currently positioned)

Code H is also used to make axis C movements with a value over 360° (spirals, threads or to use the

motor driven module for grinding combined with the spindle rotation)

Example :N32 G1 H3600 (axis C moves incrementing by 3600 degrees, i.e. making 10 spindle

turns)

Z+

C+