Siemens SINUMERIK 840D Programming Manual page 275

4
03.96
Contour monitoring with respect to tool
clearance angle
Some turning cycles in which travel movements with
relief cutting are generated monitor the tool clearance
angle of the active tool for possible contour violation.
This angle is entered as a value in the tool offset
(under parameter P24 in the D offset).
An angle between 0 and 90 degrees is entered without
a sign.
When entering the tool clearance angle, remember
that this depends on whether machining is
longitudinal or facing. If a tool is to be used for
longitudinal and face machining, two tool offsets
must be applied if the tool clearance angles are
different.
A check is made in the cycle to determine whether
the programmed contour can be machined with the
selected tool.
If machining is not possible with this tool, then
• the cycle is terminated with an error message
(while cutting) or
• contour machining continues and a message is
output (in undercut cycles). The tool nose
geometry then determines the contour.
Note that active scale factors or rotations in the
current plane modify the relationships at the angles,
and that this cannot be allowed for in the contour
monitoring that takes place within the cycle.
If the tool clearance angle is specified as zero in the
tool offset, this monitoring function is deactivated.
The precise reactions are described in the various
cycles.
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
Turning Cycles
4.2 Preconditions
No contour violation
No contour violation
4
Contour violation
Contour violation
4-275