Milling: Circular Movement G12, G13—Absolute Center Coordinates - HEIDENHAIN MANUALPLUS 620 User Manual

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
Parameters
X Final point (diameter)
Y Final point
Z Final point
I Absolute center point (radius)
J Absolute center point
K Absolute center point
R Radius
Q Point of intersection. Final 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)
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
"?"
410 DIN Programming for the Y Axis