Milling: Circular Movement G2, G3—Incremental Center Coordinates - HEIDENHAIN MANUALPLUS 620 User Manual

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
Parameters
X Final point (diameter)
Y Final point
Z Final 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: Rounding radius
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)
If you do not program the center, MANUALplus automatically
calculates the possible solutions for the center and chooses that point
as the center which results in the shortest arc.
Programming X, Y, Z: Absolute, incremental or modal or
"?"
HEIDENHAIN MANUALplus 620 409