HEIDENHAIN ITNC 530 User Manual page 509

Interpolation type between the starting and end
position
The TNC provides two functions for defining the type of interpolation
between the starting and end position:
PATHCTRL AXIS determines that the tool point between
the starting and end position of the respective NC
block moves on a straight line (Face Milling). The
direction of the tool axis at the starting and end
position corresponds to the respective programmed
values, but the tool circumference does not describe
a defined path between starting and end position. The
surface produced by milling with the tool
circumference (Peripheral Milling), depends on the
machine geometry.
PATHCTRL VECTOR determines that the tool point
between the starting and end position of the
respective NC block moves on a straight line and also
that the direction of the tool axis between starting and
end position is interpolated so that a plane results
from machining at the tool circumference (Peripheral
Milling)
With PATHCTRL VECTOR, remember:
Any defined tool orientation is generally accessible
through two different tilting angle positions. The TNC uses
the solution over the shortest available path—starting
from the current position. Therefore, with 5-axis
machining it may happen that the TNC moves in the rotary
axes to end positions that are not programmed.
To attain the most continuous multiaxis movement
possible, define Cycle 32 with a Tolerance for rotary
axes (see "TOLERANCE (Cycle 32, software option 2)" on
page 479). The tolerance of the rotary axes should be
about the same as the tolerance of the contouring
deviation that is also defined in Cycle 32. The greater the
tolerance for the rotary axes is defined, the greater are the
contour deviations during peripheral milling.
Example NC blocks:
...
13 FUNCTION TCPM F TCP AXIS SPAT PATHCTRL AXIS
14 FUNCTION TCPM F TCP AXIS POS PATHCTRL VECTOR
...
HEIDENHAIN iTNC 530
Tool tip moves along a straight line
Tool tip and tool directional vector move in one plane
509