HEIDENHAIN CNC Pilot 4290 Description of the Y axis - Manual (Page 26)

Y Axis 26
Circular path – milling
G2, G3 – incremental, G12, G13 – absolute dimensioning of
center
The tool moves in a circular arc at the feed rate to the ”end point.”
The direction of rotation of G2/G3 or G12/G13 is shown in the
graphic support window.
”Chamfer/rounding B” defines the transition to the next contour
element. When entering a chamfer/rounding, program the
theoretical end point of the contour element.
”Intersection selection Q” specifies the end point if the arc
intersects a line or an arc and the end point is not defined.
If you do not program the center, the CNC PILOT automatically
calculates the possible solutions for the center and chooses that
point as the center which results in the shortest arc.
The special feed rate applies to the chamfer/rounding.
The execution of G2/G3 or G12/G13 varies depending on the
working plane:
G17
■ Interpolation in the XY plane
■ Infeed in Z direction
■ Center point definition: with I, J
G18 ■ Interpolation in the XZ plane
■ Infeed in Y direction
■ Center point definition: with I, J
G19 ■ Interpolation in the YZ plane
■ Infeed in X direction
■ Center point definition: with J, K
Parameters
X, Y, Z: End point (X diameter value)
R:
Radius
Q: Selection of intersection – default: Q=0
■ Q=0: Far intersection
■ Q=1: Near intersection
B: Chamfer/rounding
■ B no entry: Tangential transition
■ B=0: Nontangential transition
■ B>0: Radius of rounding
■ B<0: Width of chamfer
E: Special feed-rate factor (0 < E † 1) – default: 1
(special feed rate = active feed rate * E)
With G2, G3:
I, J, K: Center point incremental – (distance from starting point to
center point; I radius)
With G12, G13:
I, J, K: Absolute center (I radius)
Programming X, Y, Z: Absolute, incremental, modal or
”?”
2.3.3
Simple
Linear
and
Circular
Paths
Example: G2 – XY plane
Example: G2 – YZ plane
Example: G13 – YZ plane
Y_4290BH.pm6 08.03.2005, 08:36 26