Sinumerik 840D cycles: drilling, milling and turning

Sinumerik 840D standard cycles with parameter lists: CYCLE81 to CYCLE89, MCALL with HOLES1/HOLES2, pockets, face milling, CYCLE800, CYCLE832, CYCLE95 and CYCLE97.

Sinumerik cycles are subprograms that are called with a parameter list, for example CYCLE83(…). The input screens of the control write the call with all parameters, but the call can also be typed by hand. The parameter order is fixed: an unused parameter keeps its comma, and parameters at the end of the list can be dropped.

The lists on this page are the classic parameter lists of the 840D. On an 840D sl with SINUMERIK Operate the cycle names are the same, but most cycles have additional parameters at the end of the list. A program written with the short list still runs, the missing parameters take their default values.

Conditions for every cycle

The working plane (G17, G18, G19) is selected before the call. Drilling cycles drill in the axis perpendicular to the plane, milling cycles feed in along that axis.

Tool, offset (D), spindle speed, direction of rotation and feed are programmed before the call unless the cycle has its own parameter for them. G commands and the programmable frame that were active before the call are still active afterwards.

Common parameters

If both DP and DPR are given, the cycle takes the depth from DPR. A relative depth with RTP equal to RFP, or with the retraction plane below the reference plane, stops the cycle with alarm 61101.

Drilling cycles

CYCLE81 to CYCLE84 and CYCLE86 to CYCLE89 use the feed programmed before the call. SDIR in the boring cycles is the direction of rotation inside the cycle (3 for M3, 4 for M4).

CYCLE83 deep-hole drilling

CYCLE84 rigid tapping

MPIT and PIT are alternatives, only one of them is filled in.

CYCLE840 is used with a compensating chuck. SDR sets the direction for retraction (0 reverses automatically). ENC selects tapping with or without spindle encoder: 0 with encoder, 1 without encoder and feed programmed before the call, 11 without encoder and feed calculated by the cycle, 20 with encoder and dwell.

Modal call with MCALL

With MCALL in front of the cycle name, the cycle runs automatically after every following block with path motion. The MCALL block itself does not drill. MCALL without a name switches the modal call off, and so does a new MCALL with another subprogram. A subprogram called modally cannot contain another modal call.

G17 G90 G54
T5 M6
D1 S1600 M3 F140
G0 X0 Y0 Z50
MCALL CYCLE83(50, 0, 2, -30, , -8, , 3, 0, 0, 1, 1)
X20 Y10
X50
X80 Y30
MCALL
G0 Z100

The cycle drills at X20 Y10, X50 Y10 and X80 Y30. The first infeed goes to Z−8, each further infeed is 3 mm shorter, and the drill retracts fully after each infeed (VARI = 1).

Hole pattern cycles

Pattern cycles only describe positions. They are combined with a drilling cycle that is called modally with MCALL before the pattern. Without an active modal drilling cycle, the control reports alarm 62100. The alarm can be acknowledged, and the pattern then only positions.

If INDA is left out, HOLES2 spreads the holes evenly over the full circle.

G17 G90 G54
T12 M6
D1 S900 M3
G0 X0 Y0 Z50
MCALL CYCLE84(50, 0, 2, -18, , 0, 3, , 1.5, 0, 400, 800)
HOLES2(0, 0, 40, 15, 60, 6)
MCALL
G0 Z100

Six M10 threads on a circle with radius 40 mm. The first hole sits at 15°, the following ones every 60°. The spindle taps at 400 rpm and retracts at 800 rpm.

Milling cycles

POCKET3 rectangular pocket

POCKET3(_RTP, _RFP, _SDIS, _DP, _LENG, _WID, _CRAD, _PA, _PO, _STA, _MID, _FAL, _FALD, _FFP1, _FFD, _CDIR, _VARI, _MIDA, _AP1, _AP2, _AD, _RAD1, _DP1)

G17 G90 G54
T8 M6
D1 S3000 M3
G0 X0 Y0 Z20
POCKET3(20, 0, 2, -12, 80, 50, 6, 60, 40, 0, 4, 0.3, 0.2, 600, 200, 0, 21, 6, , , , 4, 2)

Roughs a pocket 80 × 50 mm with 6 mm corner radius and 12 mm depth, centered on X60 Y40. Infeed 4 mm per pass on a helix with 4 mm radius and 2 mm pitch, stepover 6 mm, 0.3 mm left on the walls and 0.2 mm on the floor.

POCKET4 (circular pocket) uses the same scheme with _PRAD for the radius and _PA/_PO as center. Its _VARI has a thousands digit: 0 machines plane by plane, 1 mills the whole depth on a helix.

CYCLE71 face milling

CYCLE71(_RTP, _RFP, _SDIS, _DP, _PA, _PO, _LENG, _WID, _STA, _MID, _MIDA, _FDP, _FALD, _FFP1, _VARI, _FDP1)

_PA/_PO is the start corner, _LENG and _WID the incremental size of the area (the sign selects the corner). _FDP is the run-out in cutting direction, _FDP1 the overrun in stepover direction. _VARI: units digit 1 roughing, 2 finishing. Tens digit 1 or 2 mills parallel to the first or second axis in one direction, 3 or 4 parallel to the first or second axis with alternating direction.

CYCLE800 swivel

CYCLE800(_FR, _TC, _ST, _MODE, _X0, _Y0, _Z0, _A, _B, _C, _X1, _Y1, _Z1, _DIR)

CYCLE800 rotates the working plane on machines with swivel head or swivel table. The kinematics are stored in a swivel data set, which the machine builder sets up.

CYCLE832 high-speed settings

CYCLE832(_TOL, _TOLM)

CYCLE832 sets the contour tolerance and the matching smoothing, compressor and dynamics settings for free-form machining. _TOL is the tolerance of the machining axes in mm (or degrees for rotary axes). _TOLM selects the machining type: roughing, semi-finishing, finishing, or 0 to return to the default settings. The machine builder can adapt what each type switches on.

CYCLE832(0.1, 1003)       (Roughing, tolerance 0.1 mm)
CORE_ROUGH
CYCLE832(0.005, 102001)   (Finishing, tolerance 0.005 mm)
CORE_FINISH
CYCLE832(0, 0)            (Default settings)

Turning cycles

CYCLE95 stock removal

CYCLE95(NPP, MID, FALZ, FALX, FAL, FF1, FF2, FF3, VARI, DT, DAM, _VRT)

Adding 200 (201 to 212) switches off the cleanup cut along the contour after each roughing pass. Residual corners can then remain, depending on tool radius and infeed. In longitudinal machining the infeed is in the facing axis, in facing it is in the longitudinal axis. Outside machining feeds in negative direction, inside machining in positive direction.

G18 G90 G54 G95
T1 D1 S1200 M4
G0 X80 Z5
CYCLE95("SHAFT_CONTOUR", 2, 0.1, 0.2, , 0.3, 0.15, 0.08, 9, , , 1)
G0 X150 Z100

Roughs and finishes the outside contour from the subprogram SHAFT_CONTOUR longitudinally, with 2 mm infeed and allowances of 0.1 mm in Z and 0.2 mm in X.

CYCLE97 thread cutting

CYCLE97(PIT, MPIT, SPL, FPL, DM1, DM2, APP, ROP, TDEP, FAL, IANG, NSP, NRC, NID, VARI, NUMT, _VRT)

G18 G90 G54 G95
T3 D1 S800 M4
G0 X40 Z10
CYCLE97( , 30, 0, -28, 30, 30, 6, 2, 2.15, 0.05, 29, 0, 6, 1, 3, 1, 1)
G0 X100 Z100

External thread M30 (pitch 3.5 mm taken from MPIT) over 28 mm length, 6 roughing cuts at constant chip cross-section, 0.05 mm finishing allowance and one spring pass.