0 votes
27 views
in cnc programming by (9.4k points)

In this article, we describe how to use Siemens CYCLE75 code on CNC machines with all details and examples.

Cycle CYCLE75 transfers the island contours to pocket milling cycle CYCLE73. The cycle is called once per island contour. It does not need to be called if no island contours are programmed.
The transferred parameter values are written to the temporary file opened by CYCLE74.

Note :

Pocket milling with islands is an option that requires SW6 in both the NCK and HMI Advanced.

Format

CYCLE75 (_KNAME, _LSANF, _LSEND)

_KNAME = Name of contour subroutine of island contour
_LSANF = Block number/label identifying start of contour definition


_LSEND = Block number/label identifying end of contour definition

Contour Programming

Pocket edge and island contours must always be closed, i.e., the start and end points are
identical.
The starting point, i.e., the first point in every contour, must always be programmed with G0. All other contour elements are programmed via G1 to G3.
When programming the contour, the last contour element must not contain a radius or
champfer.
The tool may not be located at a starting position of the programmed contour element before CYCLE73 is invoked.
The necessary programs must always be stored in one directory only (workpiece or parts program). It is permissible to use the global subroutine memory for pocket edge or island contours.

Workpiece-related geometric dimensional data may be programmed in either metric or imperial dimensions. Switching between these units of measurement within individual contour programs 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.
Only the geometries in the plane are taken into account when calculating the machining
program for the pocket.
If other axes or functions (T.., D.., S.. M.. etc.) are programmed in the contour sections,
these are skipped when the contour is preprocessed in the cycle.


All technical 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.
It is not possible to repeat island contours by offsets implemented by suitable control
commands (e.g., zero offset, frames, etc.). Every island to be repeated always has to be


programmed again with the offsets calculated in the coordinates.

Example

Example of contour programming for pocket milling

Siemens CNC Milling CYCLE75 Program Example

%_N_SAMPLE1_MPF
;$PATH=/_N_MPF_DIR
; Example_1: Pocket with islands
;
$TC_DP1[5,1]=120 $TC_DP3[5,1]=111 $TC_DP6[5,1]=6 ;Tool offset cutter T5 D1
$TC_DP1[2,2]=120 $TC_DP3[2,2]=130 $TC_DP6[2,2]=5
N100 G17 G40 G90 ;Initial conditions G code
N110 T5 D1 ;Load milling tool
N120 M6
N130 S500 M3 F2000 M8
GOTOF _MACHINE
;
N510 _EDGE:G0 G64 X25 Y30 F2000 ;Define edge contour
N520 G1 X118 RND=5
N530 Y96 RND=5
N540 X40 RND=5
N545 X20 Y75 RND=5
N550 Y35
N560 _ENDEDGE:G3 X25 Y30 CR=5
;
N570 _ISLAND1:G0 X34 Y58 ;Define bottom island
N580 G1 X64
N590 _ENDISLAND1:G2 X34 Y58 CR=15
;
N600 _ISLAND2:G0 X79 Y73 ;Define top island
N610 G1 X99
N620 _ENDISLAND2:G3 X79 Y73 CR=10
;
_MACHINE:
;Programming of contours
SAMPLE_CONT:
CYCLE74 (“Example1″,”_EDGE”,”_FINAL_EDGE”) ;Transfer edge contour
CYCLE75 (“Example1″,”_ISLAND1″,”_FINAL_ISLAND1”) ;Transfer island contour 1


CYCLE75 (“Example1″,”_ISLAND2″,”_FINAL_ISLAND2”) ;Transfer island contour 2
ENDLABEL:
M30

Your answer

Your name to display (optional):
Privacy: Your email address will only be used for sending these notifications.
Anti-spam verification:
To avoid this verification in future, please log in or register.
...