05.91 9 Tool Offsets
9.5 G40/G41/G42 Intersection cutter radius path compensation (CRC)
The cutter radius compensation (G41 or G42) in linear blocks (G00, G01) can be cancelled
with G40. In order to effect the required compensations, at least one axis in the selected plane
must be programmed.
The length compensation is cancelled with D0 and is active if the length compensation axis is
programmed.
Example: Cancellation
N25 G17 G01 F . . .
L
F
N30 G40 X . . .
L
F
N35 D0 Z . . .
L
F
N30 Cancellation of cutter/tool nose radius compensation (only the radius compensation
value).
N35 Length compensation value = 0 is active.
or
N25 G17 G01 G41 D1 F . . .
L
F
N30 D0 X . . .
L
F
N35 Z . . .
L
F
N30 Cancellation of all compensations.
Only the radius compensation value = 0 is active.
N35 Length compensation value = 0 is active.
Prior to selecting another plane, CRC must be cancelled.
Change from G41 to G42
N10 G01 G17 G41 D12 X . . . Y . . .
L
F
N15 Z . . .
L
F
N20 G42 X . . . Y . . .
L
F
N25 Z . . .
L
F
N10 Incorporation of radius compensation
N15 Incorporation of length compensation
N20 Radius compensation changed (e.g. change in direction of movement to workpiece;
line-by-line milling)
N25 No change in length compensation
Change in tool offset number
The G function need not be reentered.
N10 G01 G17 G41 D12 X . . . Y . . .
L
F
N15 Z . . .
L
F
N20 D10 Z . . .
L
F
N25 X . . . Y . . .
L
F
N20 Change in length compensation
N25 Change in cutter radius compensation
If CRC is selected, it is not permissible to program G58, G59 or G33.
© Siemens AG 1991 All Rights Reserved 6ZB5 410-0HD02 9–9
SINUMERIK 880, (PG)
To Next Page
Loading...
Need help?
General
