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

In this article, we describe how to use Siemens CYCLE73 code on CNC machines with all details and examples.

CYCLE73 is a machining cycle used for machining any contour axes with or without islands. It supports complete machining of this type of pocket and offers the following machining operations:

  • Predrilling
  • Solid machine pocket
  • Machine residual material
  • Finish edge
  • Finish base

Pocket and island contours are freely programmed in DIN code supported, for example, by
the geometry processor.
The cycle is executed once for each operation according to the programmed machining type
(_VARI). In other words, in applications requiring roughing and finishing, or an additional rough-cut residual material operation, CYCLE73 must be called a second time.

Note :

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

Solid machine pocket
When a pocket is solid machined, it is machined with the active tool down to the programmed final machining allowances. The insertion strategy for milling can be selected. The cutting operation is segmented in the pocket depth direction (tool axis) in accordance with the specified values.

Machine residual material
The cycle allows material to be removed with a smaller milling tool. The traversing motions defined by the residual material of the last milling operation and the current tool radius are output in the generated program. The residual material technology can be programmed repeatedly with a succession of decreasing tool radii.
There is no check to determine whether residual material remains in the pocket.

Edge/base finishing
Another function of the cycle is to finish the pocket base or circumnavigate the pocket and
individual islands in a finish operation.

Predrilling
Depending on the milling tool used, it may be necessary to drill before solid machining the
workpiece. The cycle automatically calculates the predrilling positions as a function of the
solid machining operation to be performed subsequently. The drilling cycle called modally

beforehand is executed at each of these positions. Predrilling can be executed in a number
of technological machining operations (e.g., 1. centering, 2. drilling).

Check Also

Format

CYCLE73 (_VARI, _BNAME, _PNAME, _TN, _RTP, _RFP, _SDIS, _DP, _DPR, _MID, _MIDA, _FAL, _FALD, _FFP1, _FFD, _CDIR, _PA, _PO, _RAD, _DP1, _DN)

_VARI = Machining type: (enter without sign)
Values:
UNITS DIGIT: Machining process
1: Roughing (solid machining) from solid material
2: Roughing of residual material
3: Finishing of edge
4: Finishing of base
5: Predrilling
TENS DIGIT: Insertion strategy
1: Perpendicular to G1
2: On helical path
3: Oscillation
HUNDREDS DIGIT: Lift-off mode
0: on retraction plane (_RTP)
1: by amount of safety clearance (_SDIS) over reference plane (_RFP)
THOUSANDS DIGIT: Start point
1: automatic
2: manual
_BNAME = Name for program of drill positions
_PNAME = Name for pocket milling machining program
_TN = Name of solid machining tool
_RTP = Retraction plane (absolute)
_RFP = Reference plane (absolute)
_SDIS = Safety clearance (to be added to the reference plane, enter without sign)
_DP = Pocket depth (absolute)
_DPR = Pocket depth (incremental)
_MID = Maximum infeed depth for one infeed (enter without sign)
_MIDA = Maximum infeed width in the plane (enter without sign)

_FAL = Final machining allowance in the plane (enter without sign)
_FALD = Final machining allowance on base (enter without sign)
_FFP1 = Feedrate for surface machining
_FFD = Feedrate for depth infeed
_CDIR =Mill direction for machining the pocket: (enter without sign)
Values: 0: Down-cut milling (corresponds to direction of spindle rotation)
1: Down-cut milling
2: with G2 (independent of spindle direction)
3: with G3
_PA = Start point in first axis (only with manual selection of start point)
_PO = Start point in second axis (only with manual selection of start point)
_RAD = Radius of center point path for insertion along helical path or max. insertion angle for oscillating insertion

_DP1 = Insertion depth per 360° revolution on insertion along helical path
_DN = Tool offset number of stock removal tool (D number)

Example

The machining task consists of milling a pocket with 2 islands from solid material, followed
by finishing in the plane X,Y.

Siemens CNC Milling CYCLE73 Program Example

%_N_SAMPLE1_MPF
;$PATH=/_N_WKS_DIR/_N_CC73BEI1_WPD
;Example_1: Pocket with islands
;Solid machine and finish
$TC_DP1[5,1]=120 $TC_DP3[5,1]=111 $TC_DP6[5,1]=4 ;Tool offset cutter T5 D1
$TC_DP1[2,1]=120 $TC_DP3[2,1]=130 $TC_DP6[2,1]=5 ;Tool offset cutter T2 D1
N100 G17 G40 G90 ;Initial conditions G code
N110 T5 D1 ;Load milling tool
N120 M6
N130 M3 F2000 S500 M8
N140 GOTOF _MACHINE
;
N510 _EDGE:G0 G64 X25 Y30 ;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
;
;Programming of contours
_MACHINE:
GOTOF ENDLABEL
SAMPLE1_CONT:
CYCLE74(,”_EDGE”,”_ENDEDGE”)
CYCLE75(,”_ISLAND1″,”_ENDISLAND1″)
CYCLE75(,”_ISLAND2″,”_ENDISLAND2″)
ENDLABEL:
;
; Programming of pocket milling
REPEAT EXAMPLE1_CONT ENDLABEL
CYCLE73(1021,”EXAMPLE1_DRILL”,”EXAMPLE1_MILL1″,”5″,10,0,1,-17.5,0,0,2,0.5,0,9000,3000,0,0,0,4,3)
;
; Milling cutter for finishing
T2 D1 M6
S3000 M3
;
; Programming of pocket finishing
REPEAT EXAMPLE1_CONT ENDLABEL
CYCLE73(1023,”EXAMPLE1_DRILL”,”EXAMPLE1_MILL3″,”5″,10,0,1,-17.5,0,0,2,0,0,9000,3000,0,0,0,4,2)
M30

Machining result:

Machining Result

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.
...