The Traori Command - Siemens SINUMERIK 828D Manual

Important functions for 3- to 5-axis machining

3.5.2 The TRAORI command

The TRAORI command activates the 5-axis transformation. This enables the simultaneous 5-
axis machining without the disadvantages described in the previous section. The programming of
TRAORI changes the reference variables in the NC program. The coordinates of the X, Y, Z
linear axes now refer to the position of the tool tip.
If orientation changes are programmed in addition to the linear positions, the effects of the rotary
axis movements on the position of the tool tip are compensated by movements of the linear axes.
In addition to the explicit programming of swivel axis positions, TRAORI enables the use of
orientation information which allows also the orientation to be programmed and interpolated
independently of the kinematics.
If tools are used with a different length, the new tool data is automatically taken from the tool
table, calculated and the programmed feedrate always refers to the movement of the tool tip
relative to the workpiece.
Programming
TRAORI(n)
TRAFOOF
Explanation of the commands
TRAORI
TRAORI(n)
n
TRAFOON(<transformatio
n name>)
TRAFOOF
Depending on the configuration (depending on the machine manufacturer), TRAORI can
reset the active zero offset (e.g. G54) and the tool edge compensation (D1). Therefore it is
recommended that the zero offset and the tool edge compensation be activated again
after TRAORI is called up.
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Activates the first configured orientation transformation. The
command must be programmed alone in an NC block.
Activates the orientation transformation configured with n.
The number of the transformation (n = 1 or 2), TRAORI(1)
corresponds to TRAORI.
If TRAORI is defined via a kinematic chain, TRAORI can also be
activated with TRAFOON(<transformation name>).
Deactivate transformation
3.5
; Transformation On
; Transformation Off
85