Siemens SINUMERIK 840D Programming Manual page 301

4
03.96
12.98
Contour monitoring
The cycle performs contour monitoring of the
following:
• Clearance angles of the active tool
• Programming of arcs with an aperture angle of >
180 degrees
In the case of relief cut elements, the cycle checks
whether machining is possible with the active tool. If
the cycle detects that this machining is leading to a
contour violation, it outputs alarm 61604 "Active tool
violates the programmed contour" and machining is
aborted.
Contour monitoring is not performed if the clearance
angle has been defined as zero in the tool offset.
If the arcs in the offset are too large, alarm
10931 "Incorrect machining contour" is output.
Overhanging contours cannot be machined by
CYCLE95. Contours of this type are not monitored by
the cycle and consequently there is no alarm.
Starting point
The cycle determines the starting point of the
machining operation automatically. The starting point
is positioned on the axis in which infeed is performed
at a distance from the contour corresponding to final
machining allowance + liftoff distance (parameter
_VRT). In the other axis, it is positioned at a distance
corresponding to final machining allowance + _VRT
in front of the contour starting point.
The tool noise radius compensation is selected
internally in the cycle when the starting point is
approached.
The last point before the cycle is called must therefore
be selected such that it can be approached without risk
of collision and adequate space is available for the
compensating movement.
Approach strategy of the cycle
The starting point calculated by the cycle is always
approached in the two axes simultaneously for roughing
and one axis at a time for finishing. In finishing, the
infeed axis is the first to travel.
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
4.5 Stock removal cycle – CYCLE95
X
Example of an overhanging contour element
in relief cut which cannot be machined
X
Sum of the final machining
allowance in X+_VRT
4
Turning Cycles
Machining direction
Z
START POINT
of the cycle
Sum of final mach.
allow. in Z+_VRT
Z
4-301