Siemens sinumerik 840d Programming Manual page 334

Path Traversing Behavior
9
9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH
840D 840D
NCU 571 NCU 572
NCU 573
In the case of a minus sign, approach is behind
the interruption point or, with RMB, behind the
block start point.
The distance between interruption point and
approach point depends on the value of DISPR.
Even for higher values, this point can lie in the
block end point at the maximum.
Application example:
A sensor will recognize the approach to a clamp.
An ASUP is initiated to bypass the clamp.
Afterwards, a negative DISPR is repositioned on
one point behind the clamp and the program is
continued.
Approach with new tool
The following applies if you have stopped the
program run due to tool breakage:
When the new D number is programmed, the
machining program is continued with modified tool
offset values at the repositioning point.
Where tool offset values have been modified, it may
not be possible to reapproach the interruption point.
In such cases, the point closest to the interruption
point on the new contour is approached (possibly
modified by DISPR).
Approach contour
The motion with which the tool is repositioned on the
contour can be programmed. Enter zero for the
addresses of the axes to be traversed.
Commands REPOSA, REPOSQA and REPOSHA
automatically reposition all axes. Individual axis
names need not be specified.
When commands REPOSL, REPOSQ and
REPOSH are programmed, all geometry axes
are traversed automatically, i.e. they need not be
named in the command.
9-334
FM-NC 810D 840Di
Y
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Advanced (PGA) – 04.00 Edition
08.97
9
X
 Siemens AG 2000. All rights reserved