Peripheral Milling: 3-D Radius Compensation With Tcpm And Radius Compensation (Rl/Rr) - HEIDENHAIN TNC 620 User Manual

13
Peripheral milling: 3-D radius compensation with
TCPM and radius compensation (RL/RR)
The control displaces the tool perpendicular to the direction of
movement and perpendicular to the tool direction by the total
of the DR delta values (from the tool table and the TOOL CALL).
Determine the compensation direction with radius compensation
RL/RR (see figure, traverse direction Y+). For the control to be able
to reach the specified tool orientation, you need to activate the
M128 function.
Further information:
positioning with tilted axes (TCPM): M128 (option 9)", page 568
The control then positions the rotary axes automatically in such a
way that the tool can reach the specified tool orientation with the
active compensation.
Refer to your machine manual.
This function exclusively only available with spatial
angles. Your machine tool builder defines how these can
be entered.
The control is not able to automatically position the
rotary axes on all machines.
The control generally uses the defined
for 3-D tool compensation. The entire tool radius R +
DR) is only taken into account if you have activated the
FUNCTION PROG PATH IS CONTOUR function.
Further information:
path", page 588
Danger of collision!
The rotary axes of a machine may have limited ranges of
traverse, e.g. between -90° and +10° for the B head axis.
Changing the tilt angle to a value of more than +10° may result
in a 180° rotation of the table axis. There is a danger of collision
during the tilting movement!
Program a safe tool position before the tilting movement, if
necessary.
Carefully test the NC program or program section in the
Program run, single block operating mode
There are two ways to define the tool orientation:
In an LN block with the components TX, TY and TZ
In an L block by indicating the coordinates of the rotary axes
586
Multiple-Axis Machining | Three-dimensional tool compensation (option 9)
"Maintaining the position of the tool tip when
"Interpretation of the programmed
NOTICE
delta values
HEIDENHAIN | TNC 620 | Conversational Programming User's Manual | 10/2017