Table of Contents
Advertisement
04.97
6
Tool Offsets
6.1
Tool offset G43, G44
With the tool offset, an existing machining program can still be used, even after the tool
dimensions have changed. Normally, the programming refers to the tool zero point. Through
tool wear or exchange of the tool, the position of the tool tip may change. This change can be
compensated through the tool offset, without requiring any changes in the machining program.
Programming:
N5 G90 (G43) (G44) G01 X50.000 F4000.00 D5
N10 X80.000
N15 X150.000 D6
N20 X200.000
N25 X300.000 D0
N5:
The tool offset is selected by means of the D-number D5. With the optional
indications G43 or G44, the direction of action of the tool offset can be fixed. As G43
is active in basic position, G43 need only be entered to deselect an active G44. The
axis positions on X50.000, taking into account the tool offset memory D5.
N10:
The tool offset D5 remains active.
N15:
Through new selection of D6, D5 is deselected. The axis positions on X150.000,
taking into account the tool offset memory D6.
N20:
The tool offset D6 remains active.
N25:
Through deselection of the tool offset by means of D0, D6 becomes inactive. The
axis positions on X300.000, without tool offset.
A selected tool offset is deselected by:
•
New selection of another D-number
•
Deselection through D0
•
Program end or through M30 or M02
•
Operating-mode change
•
Program abortion through a WF traversing error message
•
Block search forwards, as the program is newly decoded
•
The control signal "reset axis" [RST]
•
Switch-on of the follow-up mode [NFB]
A selected tool offset is maintained in:
•
Jumps into subroutines or returns to the main program
•
Program continuous loops through M18 or G04 (dwell time in the last traversing block)
The calculation of the tool offset is only taken into account in absolute-
dimension programming (G90).
©
Siemens AG 1997 All Rights Reserved
WF 723 C (Programming Guide)
6ZB5 440-0VU02
Tool Offsets
Selection
New selection
Deselection
6 – 1
Advertisement
Table of Contents
