Siemens sinumerik 840d Programming Manual page 466

User Stock Removal Programs
14
14.2 Contour preparation: CONTPRON
840D 840D
NCU 571 NCU 572
NCU 573
Additional notes
Preconditions for the call
Before CONTPRON is called
• a starting point must be approached which
permits collision-free machining,
• tool edge radius compensation with G40 must be
deactivated.
Permitted traversing commands, coordinate
system
Only G commands G0 to G3 are permitted for
contour programming in addition to rounding and
chamfer.
SW 4.4 and higher supports circular-path
programming via CIP and CT.
The functions Spline, Polynomial, thread produce
errors.
It is not permitted to change the coordinate system by
activating a frame between CONTPRON and
EXECUTE. The same applies to a change between
G70 and G71/ G700 and G710.
Changing the geometry axes with GEOAX while
preparing the contour table produced an alarm.
Terminate contour preparation
When you call the predefined subroutine EXECUTE
(variable), contour preparation is terminated and the
system switches back to normal execution when the
contour has been described. The variable then
indicates:
1 = error
0 = no error (the contour is error free).
Relief cut elements
The contour description for the individual relief cut
elements can be performed either in a subroutine or
in individual blocks.
Stock removal irrespective of the programmed
contour direction (SW 4.4 and higher)
In SW 4.4 and higher, contour preparation has been
expanded. Now when CONTPRON is called, the
contour table is available irrespective of the
programmed direction.
14-466
FM-NC 810D 840Di
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Advanced (PGA) – 04.00 Edition
12.98
14
 Siemens AG 2000. All rights reserved