HEIDENHAIN SW 548328-05 DIN Programming - Manual (Page 503)

HEIDENHAIN MANUALplus 620, CNC PILOT 620/640
503
6.6 Linear and cir
c
ular mo
v
e
ments in the Y axis
Milling: Circular movement G12, G13—absolute
center coordinates
G12/G13 moves the tool in a circular arc at the feed rate to the "end
point."
The execution of G12/G13 varies depending on the working plane:
 G17 Interpolation in the XY plane
 Infeed in Z direction
 Center definition: with I, J
 G18 Interpolation in the XZ plane
 Infeed in Y direction
 Center definition: with I, K
 G19 Interpolation in the YZ plane
 Infeed in X direction
 Center definition: with J, K
If you do not program the center, the Control automatically calculates
the possible solutions for the center and chooses that point as the
center which results in the shortest arc.
Parameters
X End point (diameter)
Y End point
Z End point
I Absolute center point (radius)
J Absolute center point
K Absolute center point
R Radius
Q Point of intersection. End point if the line segment intersects a
circular arc (default: 0):
 Q=0: Near point of intersection
 Q=1: Far point of intersection
B Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 B=0: No tangential transition
 B>0: Rounding radius
 B<0: Chamfer width
E Special feed factor for the chamfer/rounding (default: 1)
Special feed rate = active feed rate * E (0 < E <= 1)
Programming X, Y, Z : Absolute, incremental or modal or
"?"