HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 197)

HEIDENHAIN CNC PILOT 4290 197
4.15 T
ool-Tip and Cut
ter Radius Compensation
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
G41/G42: Switch on TRC/MCRC
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.
Please note:
„ Program a straight line segment (G0/G1) in or after the block
containing G41/G42.
„ The TRC/MCRC is taken into account from the next path of traverse.
. . .
N.. G0 X10 Z10
N.. G41 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
. . .
Example: G40, G41, G42
. . .
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X0 Z2
N3 G42 [TRC on, to the right of the
contour]
N4 G1 Z0
N5 G1 X20 B-0.5
N6 G1 Z-12
N7 G1 Z-24 A20
N8 G1 X48 B6
N9 G1 Z-52 B8
N10 G1 X80 B4 E0.08
N11 G1 Z-60
N12 G1 X82 G40 [TRC off]
. . .
Parameters
Q Plane (default: 0)
„ Q=0: TRC on the turning plane (XZ plane)
„ Q=1: MCRC on the front face (XC plane)
„ Q=2: MCRC on the lateral surface (ZC plane)
„ Q=3: MCRC on the front face (XY plane)
„ Q=4: MCRC on the lateral surface (YZ plane)
H Output (only with TRC) – (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