HEIDENHAIN SW 548328-05 DIN Programming - Manual (Page 249)

HEIDENHAIN MANUALplus 620, CNC PILOT 620/640
249
4.12 T
ool-tip and cut
ter r
a
dius compensation
4.12 Tool-tip and cutter radius
compensation
Tool-tip radius compensation (TRC)
If TRC is not used, the theoretical tool tip is the reference point for the
paths of traverse. This might lead to inaccuracies when the tool moves
along non-paraxial paths of traverse. The TRC function corrects
programmed paths of traverse.
The TRC (Q=0) reduces the feed rate for circular arcs if the shifted
radius < the original radius. The TRC corrects the special feed rate
when a rounding arc is machined as transition to the next contour
element.
Reduced feed rate = feed rate * (shifted radius / original radius)
Milling cutter radius compensation (MCRC)
When the MCRC function is not active, the system defines the center
of the cutter as the zero point for the paths of traverse. With the
MCRC function, the Control accounts for the outside diameter of the
tool when moving along the programmed paths of traverse. The
recessing, roughing and milling cycles
already include TRC/MCRC
calls. The TRC/MCRC must be switched off when these cycles are
called.
G40: Switch off TRC/MCRC
G40 is used to deactivate TRC/MCRC. Please note:
 The TRC/MCRC remains in effect until a block with G40 is reached.
 The block containing G40, or the block after G40 only permits a
linear path of traverse (G14 is not permissible).
Function of the TRC/MCRC
 If the tool radii are > than the contour radii, the TRC/
MCRC might cause endless loops. Recommendation:
Use the finishing cycle G890 or milling cycle G840.
 Never program the MCRC during a perpendicular
approach to the machining plane.
. . .
N.. G0 X10 Z10
N.. G41
Activate TRC to the left of the contour
N.. G0 Z20
Path of traverse: from X10/Z10 to X10+TRC/
Z20+TRC
N.. G1 X20
The path of traverse is "shifted" by the TRC
N.. G40 G0 X30 Z30 Path of traverse from X20+TRC/Z20+TRC to X30/
Z30
. . .