Siemens SINUMERIK 840D Programming Manual page 235

03.96
12.98
4
Machining must then be divided into several
machining sections each of which is represented by
its own contour subroutine and each cycle called
separately.
If the maximum diameter in one contour subroutine
is not within the programmed end point or starting
point of the contour, the cycle automatically extends
a paraxial straight line to the maximum point of the
contour at the end of the machining operation and
this part of the contour is then removed as a relief
cut.
If any of the following are programmed in the contour
subroutine:
• Radius compensation plane with G17/G18/G19
• Frames
• An axis of the plane in which machining is
performed is traversed as a positioning axis
• Selection of tool radius compensation with
G41/G42
alarm 10931 "Incorrect machining contour" is
activated and aborts the cycle.
Contour direction
With SW 4.4 and later, the direction in which the
stock removal contour can be programmed is freely
selectable. The machining direction is automatically
defined in the cycle. With complete machining
operations, the contour is finished in the same
direction in which rough cutting took place.
If only finishing is selected, the contour is always
traversed in the programmed direction.
The first and last programmed contour points are the
criteria for selecting the machining direction. For this
reason, both coordinates must always be
programmed in the first block of the contour
subroutine.
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
4.5 Stock removal cycle – CYCLE95
X
Extended
straight line
End point
Turning Cycles
4
Starting
point
Z
4-235