HEIDENHAIN CNC Pilot 4290 - Manual (Page 124)

4 DIN PLUS 112
Circular arc G13
Circular paths
G2, G3 – incremental center coordinates
G12, G13 – absolute center coordinates
The tool moves in a circular arc at the feed rate to the ”end point.”
Direction of rotation: see help graphic.
Parameters
X, Z: Diameter, length to end point (X diameter)
R: Radius (0 < R <= 200 000 mm)
Q: Selection of intersection – default: Q=0. End point, if the circular
arc intersects a circular arc.
■ Q=0: Far intersection
■ Q=1: Near intersection
B: Chamfer/rounding arc – transition to the next contour element.
Program the theoretical end point when you enter a chamfer/
rounding arc.
■ No entry in B: tangential transition
■ B=0: no tangential transition
■ B>0: Radius of the rounding arc
■ B<0: Width of chamfer
E: Special feed factor for chamfer/rounding
(0 < E <= 1) – default: 1
(special feed rate = active feed rate * E)
G2, G3 – incremental center :
I, K: Center (distance from starting point to center; I radius)
G12, G13 – center absolute:
I, K: Center (I radius)
Programming in the Y axis See ”CNC PILOT 4290 with Y Axis”
User's Manual.
Programming X, Z: Absolute, incremental, modal or ”?”
Danger of collision!
If V variables are used for calculating the address
parameters, a limited contour check is carried out. Ensure
that the variable values produce a circular arc.
Circular arc G2
4.6 Machining Commands