HEIDENHAIN MANUALplus 4110 - Manual (Page 301)

HEIDENHAIN MANUALplus 4110 301
6.7 T
ool-Tip / Milling-Cut
ter Radius Compensation
G40: Switch off TRC/MCRC
„ 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).
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 taken into account from the next path of traverse.
G41: Internal machining (with traverse in negative Z direction)—
compensation of the tool-tip / cutter radius to the left of the contour in
traverse direction.
G42: External machining (with traverse in negative Z direction)—
compensation of the tool-tip / cutter radius to the right of the contour
in traverse direction.
Parameters
 Q plane (default: 0)
„ Q=0: TRC on the turning plane (XZ plane)
„ Q=1: MCRC on the face (XC plane)
„ Q=2: MCRC on the lateral surface (ZC plane)
 H output (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
Example: G40, G41, G42
%40.nc
[G40, G41, G42]
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X0 Z2
N3 G42
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
END