HEIDENHAIN CNC Pilot 4290 - Manual (Page 127)

HEIDENHAIN CNC PILOT 4290 115
4.6.5 Cutter Radius Compensation (TRC/MCRC)
Tooth and cutter 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 (see section ”
1.5 Tool Dimensions”).
With Q=0, the TRC reduces the feed rate at arcs (G2, G3, G12, G13)
and rounding arcs if the ”shifted radius < original radius”. The ”special
feed rate” is corrected when a rounding as transition to the next
contour element is machined.
Reduced feed rate:
Feed rate * (offset radius / original radius)
Milling cutter radius compensation (MCRC)
Without the MCRC function, the system defines the center of the
cutter as the zero point for the paths of traverse. With the TRC
function, the CNC PILOT accounts for the outside cutting radius when
moving along the programmed paths of traverse (see ”
1.5 Tool
Dimensions”).
Recessing, area clearance and milling cycles already include TRC/
MCRC calls. You must therefore ensure that TRC/MCRC is disabled
before you call these cycles. There are a few exceptions to this rule
that will be described where concerned.
G40: Switch off TRC/MCRC
■ The TRC is effective up to the block before G40
■ In the block with G40 or in the block after G40, only a line is
permissible (G14 is not allowed)
G41/G42: Switch on TRC/MCRC
■ A straight line segment (G0/G1) must be programmed in the block
containing G41/G42 or after the block containing G41/G42
■ The TRC/MCRC is effective beginning with the next positioning
command
G41: Switch on TRC/MCRC – compensation of the tool-tip/cutter
radius to the left of the contour in traverse direction.
G42: Switch on TRC/MCRC – compensation of the tool-tip/cutter
radius to the right of the contour in traverse direction.
Parameters (G41/G42)
Q:
Machining plane – default: 0
■ Q=0: TRC on the turning plane (X-Z plane)
■ Q=1: MCRC on the face (X-C plane)
■ Q=2: TRC on the lateral surface (Z-C plane)
■ Q=3: TRC on the ace (X-Y plane)
■ Q=4: TRC on the lateral surface (Y-Z plane)
H: Output (only with MCRC) – default: 0
■ H=0: Intersecting areas which are
programmed in directly successive contour
elements are not machined.
■ H=1: The complete contour is machined –
even if certain areas are intersecting.
O: Feed rate reduction – default: 0
■ O=0: Feed rate reduction active
■ O=1: No feed rate reduction
■ If the tool radii are larger than the contour
radii, the TRC/MCRC might cause endless
loops.Recommendation: Use the finishing
cycle G890 / milling cycle G840.
■ Never select MCRC during a
perpendicular approach to the respective
plane.
■ Remember when calling subprograms
with ”active TRC/MCRC”:
Switch the TRC/MCRC off
– in the subprogram in which it was
switched on
– in the main program if it was switch on
there.
. . .
N.. G0 X10 Z10
N.. G41 G0 Z20
N.. G1 X20
N.. G40 G0 X30 Z30
. . .
4.6 Machining Commands
Function of the TRC/MCRC
Path of traverse: from X10/Z10 to X10+TRC/Z20+TRC
The path of traverse is ”shifted” by the TRC
Path of traverse from X20+TRC/Z20+TRC to X30/Z30