HEIDENHAIN CNC Pilot 4290 Pilot - Manual (Page 50)

50
Tooth and cutter radius compensation (TRC/MCRC)
G40, G41, G42
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 one straight line
segment permitted (G14 is not permitted).
G41/G42: switch on TRC/MCRC
■ In the block with G41/G42 or after the block with G41/G42, one
straight line segment (G0/G1) is to be programmed.
■ The TRC/MCRC is included after the next contour element.
G41: Switch on TRC/MCRC – displacement of the tool radius in the
direction left of the contour.
G42: Switch on TRC/MCRC – displacement of the tool radius in the
direction right of the contour.
Parameters
Q:
Machining plane – default: 0
■ Q=0: TRC on the turning plane (X-Z plane)
■ Q=1: MCRC on the end face (X-C plane)
■ Q=2: MCRC on the cylindrical surface (Z-C plane)
■ Q=3: MCRC on the end face (X-Y plane)
■ Q=4: MCRC on the cylindrical 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
T
ooth and cut
ter r
adius
compensation (TR
C)
• If the tool radii > contour radii, it can result
in tool path loops during CRC/MCRC.
Recommendation: Use the finishing cycle
G890 / milling cycle G840.
• Never select MCRC during a perpendicular
approach to the plane.
• Note when calling subprograms with
active TRC/MCRC:
Switch the TRC/MCRC off in the main pro-
gram if it was switched on in the main pro-
gram. – Switch the TRC/MCRC off in the
subprogram in which it was switched on.