Siemens SINUMERIK 840D Programming Manual page 236

Turning Cycles
4
4.5 Stock removal cycle – CYCLE95
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 operation will
lead to a contour violation, it is aborted after alarm
61604 "Active program violates programmed
contour" is output.
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.
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.
4-236
X
Sum of the final machining
allowance in X+_VRT
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
12.98
4
START POINT
of the cycle
Sum of final mach.
allow. in Z+_VRT
Z
 Siemens AG 2000 All rights reserved.