Contour Programming - Siemens SINUMERIK 840D Programming Manual

03.96
08.99
3
3.15 Pocket milling with islands - CYCLE73, CYCLE74, CYCLE75

3.15.3 Contour programming

Pocket edge and island contours must always be closed,
i.e. the start and end points are identical.
The start point, i.e. first point on a contour must always be
programmed with G0, and all other contour elements via
G1 to G3.
When the contour is programmed, the last contour element
(block with label or block number at end of contour) must
not contain a radius or chamfer.
The tool must not be positioned on a starting position of the
programmed contour elements before CYCLE73 is called.
The necessary programs must always be stored in one
directory (workpiece or part program). It is permissible to
use the subroutine memory for pocket edge or island
contours.
Workpiece-related geometric dimensional data may be
programmed in either metric or inches. Switching between
these units of measurement within individual contour
programs will causes errors in the machining program.
When G90/G91 are programmed alternately in contour
programs, care must be taken to program the correct
dimensional command at the start of the program in the
sequence of contour programs to be executed.
When the pocket machining program is calculated, only the
geometries in the plane are taken into account.
If other axes or functions (T.., D.., S.. M.. etc.) are
programmed in contour sections, they are skipped when
the contour is prepared internally in the cycle.
All machine-specific program commands (e.g. tool call,
speed, M command) must be programmed before the
cycle commences. Feedrates must be set as parameters in
CYCLE73.
The tool radius must be greater than zero.
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
Milling Cycles
3
3-185