HEIDENHAIN SW 54843x-03 DIN Programming - Manual (Page 525)

HEIDENHAIN MANUALplus 620, CNC PILOT 640 525
6.6 Linear and cir
c
ular mo
v
e
ments in the Y axis
Milling: Circular movement G2, G3—incremental
center coordinates
G2/G3 moves the tool in a circular arc at the feed rate to the "end
point."
The execution of G2/G3 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 Steuerung 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 Incremental center point (radius)
J Incremental center point
K Incremental center point
R Radius
Q Point of intersection. End point if the circular arc intersects a
line segment or another circular arc (default: 0):
 0: Near point of intersection
 1: Far point of intersection
BR Chamfer/rounding. Defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point.
 No entry: Tangential transition
 BR=0: No tangential transition
 BR>0: Radius of rounding
 BR<0: Width of chamfer
BE Special feed factor for chamfer/rounding arc (default: 1)
Special feed rate = active feed rate * BE (0 < BE <= 1)
Programming X, Y, Z: Absolute, incremental, modal or "?"