HEIDENHAIN TNC 620 User Manual page 468

12
Multiple axismachining
12.5 Peripheral Milling: 3-D radius compensation with M128 and radius
compensation (G41/G42)
12.5 Peripheral Milling: 3-D radius
compensation with M128 and radius
compensation (G41/G42)
Application
With peripheral milling, the TNC displaces the tool perpendicular
to the direction of movement and perpendicular to the tool
direction by the sum of the delta values DR (tool table and T block).
Determine the compensation direction with radius compensation
G41/G42 (direction of movement Y+).
For the TNC to be able to reach the set tool orientation, you
need to activate the M128 function and subsequently the tool
radius compensation. The TNC then positions the rotary axes
automatically so that the tool can reach the orientation defined by
the coordinates of the rotary axes with the active compensation.
Further Information:
positioning with tilted axes (TCPM): M128 (option 9)", page 463
This function is possible only on machines for which
you can define spatial angles for the tilting axis
configuration. Refer to your machine manual.
The TNC is not able to automatically position the
rotary axes on all machines.
Refer to your machine manual.
Note that the TNC makes a compensating
movement by the defined
radius R defined in the tool table has no effect on the
compensation.
Danger of collision!
On machines whose rotary axes only allow limited
traverse, sometimes automatic positioning can
require the table to be rotated by 180°. In this case,
make sure that the tool head does not collide with
the workpiece or the clamps.
You can define the tool orientation in a G01 block as described
below.
Example: Definition of the tool orientation with M128 and the
coordinates of the rotary axes
N10 G00 G90 X-20 Y+0 Z+0 B+0 C+0*
N20 M128*
N30 G01 G42 X+0 Y+0 Z+0 B+0 C+0 F1000*
N40 X+50 Y+0 Z+0 B-30 C+0*
468
"Maintaining the position of the tool tip when
delta values. The tool
Pre-position
Activate M128
Activate radius compensation
Position the rotary axis (tool orientation)
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016