DIN/ISO programming | Tool-tip and cutter radius compensation
4
302
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4.12 Tool-tip and cutter radius compensation
Fundamentals
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 point of reference 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. Recessing, area clearance and milling cycles
already include TRC and MCRC calls. The TRC and MCRC must be
switched off when these cycles are called.
Programming notes:
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
Switch off TRC/MCRC G40
G40 is used to deactivate TRC and MCRC.
Please note:
The TRC and MCRC remain 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)
Example: G40
. . .
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
. . .
To Next Page
Loading...
