Mazak fixed cycles: drilling, tapping, boring and turning

Mazak EIA/ISO fixed cycles: block structure, address meanings, drilling, tapping and boring cycles, hole patterns, and turning cycles on Integrex machines.

Mazak fixed cycles carry out positioning, drilling, tapping or boring with a single block. The G-numbers match the usual ISO assignment for the common cases (G81, G83, G84), but the boring cycles G75 to G79 and several addresses work differently from other controls. Programs moved from another machine should be checked cycle by cycle.

Block structure

G□□ X_ Y_ Z_ Q_ R_ P_ D_ K_ I_ J_(B_) E_ H_ F_ L_

The block has four parts: the cycle code, the hole position (X, Y), the machining data and the repeat count L. The hole position and L apply only to the current block. The machining data are modal and stay active for the following hole positions until the cycle is cancelled.

The initial point is the Z position at the moment the cycle is called. G98 returns the tool to this level after each hole, G99 to the R-point level. Both are modal, G98 is active after power-on.

With incremental hole positions, L repeats the cycle at equal spacing. With absolute positions, L repeats it at the same place. L0 stores the machining data without drilling. A cycle block without any hole position also only stores the data.

G80 cancels the cycle mode, and so does any code of group 01 (G00, G01, G02, G03, G02.1, G03.1). M00 or M01 in cycle mode stops the program after positioning and suppresses the cycle for that block.

Overview

Addresses in brackets can be omitted. X and Y can also be omitted when the tool already stands on the hole.

Drilling cycles

G81 feeds to Z and returns in rapid traverse. It has no dwell and no pecking.

G82 adds a dwell P at the hole bottom. D shifts the start of the cutting feed below the R-point.

G73 drills in pecks of depth Q and retracts by the distance D after each peck to break the chip. Without D, or with D0, the return distance comes from parameter F12. K sets the distance from the R-point to the start of cutting feed.

G83 retracts to the R-point after every peck of depth Q. The tool then returns in rapid traverse down to a clearance D above the previous depth. Without D the clearance comes from parameter F13. Q0 in G73 or G83 triggers alarm 809.

G73, G82 and G83 can reduce the feed near the hole bottom, for example at a breakthrough. When the start of a pass lies within the distance I before the bottom, the control cuts with F × J / 100. If I or J is missing, the feed stays unchanged.

G82.2 is an optional pecking cycle in which Q sets a threshold value. D and K have the same meaning as in G83.

G90 G54 G00 X0 Y0
G43 H5 Z50.
S1800 M03
G98 G83 X20. Y0 R2. Z-32. Q5. F160 I4. J50
X-20.
G80

The last 4 mm of each hole are drilled at 50 % feed (80 mm/min).

Tapping cycles

G84 taps right-hand threads, G74 left-hand threads. P is always a dwell in seconds. J (or B) sets when the spindle reverses:

Without J, or with J0, the control uses 2.

H selects the tapping method. H0 runs an asynchronous cycle. A value of H1 or higher runs a synchronous cycle and sets the return speed as a percentage of the cutting feed. Without H the control runs synchronously, which leads to alarm 952 on machines without the synchronous tapping option. On such machines, H0 has to be written explicitly.

G84.2 and G84.3 always tap synchronously. Their return speed override comes from parameter K90. In synchronous tapping F is the thread pitch.

Q splits a synchronous tap into pecks. I0 selects the deep-hole tapping cycle, which retracts to the R-point after each peck. I1 selects the high-speed deep-hole cycle, which only lifts by the distance in parameter F10. Bit 3 of parameter F155 decides which variant runs when I is missing. Q and I have no effect on asynchronous tapping.

G90 G54 G00 X30. Y20.
G43 H8 Z50.
S600 M03
G99 G84.2 R5. Z-18. F1.5     (M10x1.5, synchronous)
X60.
G80

Boring cycles

The boring cycles differ mainly in what happens at the hole bottom and how the tool leaves the bore. The direction of the shift Q is set by bits 3 and 4 of parameter I14.

In G91 mode, G77 and G87 take the machining direction from the sign of Z. The sign of R is ignored.

Chamfering cutter cycles

G71.1 (clockwise) and G72.1 (counterclockwise) chamfer a bore with a chamfering cutter on a circular path. P sets the overlap length of the arc, D a distance from the R-point. Q must be given and must not be 0, otherwise alarm 861 appears.

Hole patterns

The pattern cycles G34.1, G35, G36 and G37.1 place a previously programmed fixed cycle on several positions. The cycle is first written without a hole position, so the control only stores it. The pattern block then moves to each position in rapid traverse and runs the stored cycle. The pattern data are cleared after the block. Without an active cycle, the pattern block only positions.

After the pattern, the tool stands on the last hole. The next move is easier to program in absolute coordinates. In G35 and G37.1, a missing K (or P in G37.1) or a value of 0 raises alarm 809 or 807.

G90 G54 G00 X0 Y0
G43 H3 Z50.
S2200 M03
G98 G81 R2. Z-4. F180       (stored only, no hole position)
G34.1 X0 Y0 I45. J15. K6    (6 holes on Ø90, first hole at 15°)
G80
G00 X120. Y0

Turning cycles on Integrex machines

Integrex multitasking machines add turning cycles. The codes below use the G-code series M. In series T the same cycles use the numbers in brackets, see G-codes.

Simple turning cycles

R defines a taper.

Compound cycles

In G271, G272 and G270, P and Q are the first and last sequence numbers of the finishing contour. A is a Mazak addition: it names a separate program that holds the contour. Without A, the contour is read from the running program. The roughing passes use the F, S and T values in or before the cycle block. F and S inside the contour only apply to finishing with G270.

The first G271 block (depth and escape distance) can be left out. The control then takes both values from parameters SU103 and SU102. Both blocks use address U: if P and Q are in the same block, U is the finishing allowance in X, otherwise it is the depth of cut.

G273 suits cast or forged blanks. U and W set the escape distance and direction in X (radius) and Z, R the number of roughing passes.

In G276, the six-digit P value packs three settings: mm finishing passes (01 to 99), rr thread run-out in tenths of the lead (00 to 99), and aa tool angle (80, 60, 55, 30, 29 or 0). P021260 means two finishing passes, a run-out of 1.2 × lead and a 60° thread. In the second block, R is the radius difference for taper threads (0 for straight threads), P the thread height (radius), Q the first depth of cut (radius), and F the lead.

Drilling with the rotating tool on the face and outside diameter

Format for face cycles: G283 X C Z R Q P F K M. Outside cycles swap the roles of X and Z. M carries the C-axis clamp code: the control clamps the C-axis before drilling and outputs the following code (M + 1) to unclamp it afterwards.