Milling: Circular Arc Cw G2, G3 - Incremental Center Coordinates - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO Programming for the Y axis | Linear and circular movements in the Y axis
Milling: Circular arc cw G2, G3 – incremental center
coordinates
G2 and G3 move the tool in a circular arc at the feed rate to the
Final point.
The execution of G2 and 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: Diameter – target point
Y: Length – target point
Z: Length – target point
I: Center, incremental (radius value)
J: Center, incremental
K: Center, incremental
Q: Intersect. pt. or Final point if the line segment intersects a
circular arc (default: 0)
0: Near point of intersection
1: Far point of intersection
BR: Chamf./round. – defines the transition to the next contour
element
When entering a Chamf./round., 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 rate factor for Chamf./round. (default: 1)
Special feed rate = active feed rate * BE (range: 0 < BE <= 1)
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.
Programming:
X, Y and Z absolute, incremental, modal or ?
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
6
591