Orientation Interpolation Between The Start Position And End Position - HEIDENHAIN TNC 620 User Manual

11
Multiple-axis machining | Compensating the tool angle of inclination with FUNCTION TCPM (option 9)
Orientation interpolation between the start position and
end position
With these functions, you define how the tool orientation between
the programmed start position and end position is to be interpolat-
ed:
PATHCTRL AXIS specifies that the rotary axes
between the start position and end position are
to be linearly interpolated. The surfaces that
arise through milling with the tool circumference
(peripheral milling) are not necessarily level, and
they depend on the machine kinematics.
PATHCTRL VECTOR specifies that the tool
orientation within the NC block always lies in the
plane that is defined through the start orientation
and end orientation. If the vector lies between the
start position and end position in this plane, then
milling with the tool circumference (peripheral
milling) will produce a level surface.
In both cases, the programmed tool reference point is moved along
a straight line between the start position and end position.
To obtain the most continuous multi-axis movement
possible, define Cycle 32 with a tolerance for rotary
axes.
Further information: User's Manual for Programming of
Machining Cycles
PATHCTRL AXIS
You can use the PATHCTRL AXIS variant for NC programs with small
orientation changes per NC block. In this case, the angle TA in Cycle
32 can be large.
You can use PATHCTRL AXIS both for face milling and also for
peripheral milling.
Further information: "Running CAM programs", Page 486
HEIDENHAIN recommends the PATHCTRL AXIS variant.
This enables smooth motion, which has a beneficial
effect on the surface quality.
PATHCTRL VECTOR
You can use the PATHCTRL VECTOR variant for peripheral milling
with large orientation changes per NC block.
Example
...
13 FUNCTION TCPM F TCP AXIS SPAT PATHCTRL AXIS
14 FUNCTION TCPM F TCP AXIS SPAT PATHCTRL VECTOR
...
472
The rotary axes are linearly interpolated between the start and
end positions of the NC block.
The rotary axes are interpolated such that the tool vector
within the NC block always lies in the plane that is specified
through the start orientation and end orientation.
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022