Siemens SINUMERIK 840D Programming Manual page 294

4
Turning Cycles
4.5 Stock removal cycle – CYCLE95
Finishing:
• The calculated cycle starting point is approached in both
axes simultaneously with G0 and tool nose radius
compensation is selected.
• Both axes then continue to move; with G0 up to an amount
final machining allowance + tool nose radius +
1 mm safety distance ahead of the contour starting point,
and from there with G1 to the contour starting point.
• Finish cutting along the contour with G1/G2/G3 and
FF3.
• Retraction to starting point with both axes and G0.
Description of parameters
NPP (name)
Enter the name of the contour subroutine under this
parameter. This contour subroutine must not be a
subroutine with a parameter list.
Please use the name conventions described in the
Programming Guide when naming the contour
subroutine.
In SW 5.2 and higher, the machining contour can also
be a section of the calling routine or from any other
program. The section is identified by start or end labels
or by block numbers. In this case, the program name
and labels/block number are identified by an ":".
Examples:
NPP="CONTOUR_1"
NPP="START:END"
NPP="/_N_SPF_DIR/_N_CONTOUR_1_SPF:N130:
N210"
If the section is defined by block numbers, it must be
noted that these block numbers for the section in NPP
must be correspondingly adjusted if the program is
modified and subsequently renumbered.
4-294
X
FALX
The machining contour is the complete
program "Contour_1".
The machining contour is defined as the
section starting from the block labeled
START to the block labeled END in the
calling routine.
The machining contour is defined in blocks
N130 to N210 in program CONTOUR_1.
Write the full program name together with
path and extension, refer to CALL
description in the References: /PGA/
Programming Guide Advanced.
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
4
03.96
10.00
NPP
FALZ
Z
© Siemens AG, 2002. All rights reserved