CNC turning knowledge

CNC Lathe Cycle Instruction: Applications and Techniques

A working guide to canned turning cycles on FANUC-style controls. It covers G71, G72, G73, G74, G76 and G70, when each one fits, and the setup numbers that keep a cycle from scrapping a part. Written for programmers and engineers who need to pick a cycle and prove it on the first run.

Get Instant Quote Talk to an Engineer

FANUC-style G-codesG71 / G72 / G73G74 / G76 / G70Setup values and checks

CNC lathe cycle instruction applications and techniques on a turning center

On this page

Key takeaways

Pick the cycle from the shapeTurning down a diameter uses G71. Facing a shoulder uses G72. Contour copies use G73.

Peck values decide insert lifeA depth of cut between 0.5 mm and 3 mm per pass keeps most steel inserts alive.

Leave 0.2–0.4 mm for G70The finishing cycle needs stock to cut. Zero allowance means rubbing, not cutting.

Write the profile firstCycles follow a defined contour. The contour block order matters more than the cycle call.

How the cycles differ

What a CNC lathe cycle instruction actually does

A cycle instruction is a canned routine. You describe the final profile once, then the control works out the repeated passes. The tool follows the same path a dozen times at different diameters until the stock is gone. On FANUC-style controls the common set is G71 for turning, G72 for facing, G73 for pattern repeating, G74 for peck drilling, G76 for threading and G70 for the finish pass.

The alternative is writing every pass by hand. That works on a simple shoulder, where three or four blocks do the job. It stops working when the profile has a radius, a groove and a taper in sequence. Cycle calls cut the program length and remove the arithmetic error that creeps in when someone calculates passes at the machine.

Two parameters control almost everything. The depth of cut per pass sets how hard the insert works. The finishing allowance sets how much material the last pass removes. Get those two wrong and the cycle either rubs the surface or overloads the tool.

1
Cycle callOne block with the pattern type, depth and allowance.
2
Profile blockThe contour the control repeats from start point to end point.
3
Return blockMarks the end of the profile and returns the tool.

G71 and G72

Turning and facing cycles: G71 and G72

G71 removes stock along the Z axis. Use it for shafts, bushings and any part where the diameter drops in steps. The first block carries the depth of cut, the finishing allowance and the profile start and end points. A typical first block on 4140 steel runs a 2 mm depth of cut with a 0.3 mm finishing allowance in X and 0.1 mm in Z.

G72 does the same job along the X axis, so it faces a shoulder or a disc down to length. The parameter order looks familiar but the axes swap. Mixing them up is the most common cycle error we see. The tool plunges where it should feed and the insert chips on the first pass.

Both cycles support a Type I and Type II profile. Type I allows a contour that moves in one direction in X. Type II allows a contour that moves both up and down in X, which is what a part with an undercut needs. Older controls default to Type I. Check the manual before you program a recess into the profile.

1
G71 fitsStepped shafts, bushings, long diameter reductions.
2
G72 fitsDiscs, flanges, shoulders faced to a length.
3
Watch the signA positive allowance leaves stock; a negative one cuts past the profile.

G73, G74, G76

Pattern, drilling and threading cycles

G73 repeats a defined pattern at a series of offsets. It suits castings, forgings and near-net blanks where the stock is not a simple cylinder. You set the number of passes and the total offset, then the control shifts the pattern each time. On a 6061 casting with 4 mm of uneven stock, five passes at 0.8 mm each clean it up without a single air cut.

G74 pecks along Z, which makes it the drilling and deep-bore cycle. Each peck retracts to clear chips. The retract amount matters in aluminum, where a long string can wrap the tool. A 0.5 mm retract at 1,200 rpm clears a 12 mm hole without chatter. In stainless, peck depth drops to 2–3 mm per bite to keep heat out of the drill tip.

G76 cuts a thread in a controlled series of passes, each one smaller than the last. The first block sets the thread height, the first pass depth and the included angle. A 60° included angle for metric and unified threads, 55° for Whitworth. The cycle handles the infeed so the tool does not cut on both flanks at once, which is what breaks a threading insert on the first pass.

1
G73 fitsCastings, forgings, stock that is not round.
2
G74 fitsDeep holes, chip clearing, high-pressure coolant.
3
G76 fitsAny thread with a controlled infeed, internal or external.

The finish pass

G70 and the numbers that decide surface finish

G70 reads the same profile as G71 or G72 and takes one continuous pass. It cuts the allowance left by the roughing cycle. Set that allowance too small and the insert rubs instead of cutting. Set it too large and the finish pass overloads a light tool. Between 0.2 mm and 0.4 mm covers most work; tight-tolerance parts on a rigid machine can run 0.15 mm.

Feed rate drives finish more than any other value. On aluminum, 0.15 mm/rev with a sharp uncoated insert holds Ra 0.8–1.6 μm. On 316L stainless, drop to 0.08–0.12 mm/rev and expect the same range with a coated insert. Pushing feed to save cycle time shows up immediately as a torn surface on the print.

Insert nose radius sets the floor. A 0.4 mm radius cuts cleaner on small diameters and light passes. A 0.8 mm radius handles interrupted cuts better but needs a heavier feed to avoid chatter. Match the radius to the smallest radius in the profile, not to the largest.

1
Allowance0.2–0.4 mm per side for most turning.
2
Feed0.08–0.15 mm/rev depending on material and insert.
3
Nose radiusKeep it equal to or smaller than the smallest profile radius.

At the machine

Step by step: writing and proving a cycle

Follow the order. Skipping a step is how a cycle scraps the first part.

1
Read the profile from the drawingList every diameter, length and radius in cutting order. Note the smallest internal radius, since that caps the insert nose radius you can use.
2
Choose the cycle by shapeDiameter reduction: G71. Faced length: G72. Uneven stock: G73. Holes: G74. Threads: G76. Write the choice at the top of the program.
3
Write the profile blockStart above the blank, feed to the first diameter, then move through each element in order. End at a point that lets the tool retract without dragging.
4
Set the depth of cut0.5–2 mm per pass for steel, up to 3 mm for aluminum on a rigid machine. Never exceed the insert maker's maximum depth for the corner radius.
5
Set the finishing allowance0.2–0.4 mm on X and Z for the G70 pass. Write the value with the correct sign or the cycle cuts into the profile.
6
Dry run above the partShift the work offset 50 mm in Z and run the cycle at rapid override. Watch the tool path on the screen and confirm every pass clears the blank.
7
Cut one part and measureCheck the first diameter, the length and one radius. Adjust the wear offset, not the program, before the second part.
8
Log the proven valuesRecord depth, allowance and feed in the setup sheet. The next run starts from a known point instead of a guess.

Cycle selection

Which cycle instruction to use

Match the stock condition and the feature to the cycle.

Cycle	Use when	Typical depth	Watch for
G71	Diameter drops in steps	0.5–2 mm/pass	Profile sign errors
G72	Facing to a length	0.5–2 mm/pass	X and Z swapped
G73	Casting or forging stock	0.5–1 mm/pass	Air cuts on light stock
G74	Drilling or deep boring	2–5 mm/peck	Chip wrapping the drill
G76	Internal or external threads	Decreasing passes	Wrong included angle
G70	Finishing after G71/G72	0.2–0.4 mm total	Too little allowance

Pick the cycle from the stock, not the drawing

The drawing shows the final shape. The cycle has to remove what is actually on the blank. Match the cycle to the stock condition and the profile usually proves on the first part.

Get Instant Quote Talk to an Engineer

FAQs

Common questions

Can I run G70 without a roughing cycle first?

Yes, if the blank is already close to size. G70 only follows the profile, so it removes whatever stock sits outside that line.

On a raw bar with several millimeters to remove, the finishing pass overloads the insert. Rough first with G71 or G72, then finish.

Why does my G71 cycle cut air on the first passes?

The profile start point usually sits inside the blank, so the control has nothing to remove until it reaches the larger diameter.

Move the start point outside the stock, or switch to G73 if the blank is a casting with uneven material.

What depth of cut should I use in stainless?

Keep it lighter than carbon steel. A 1–1.5 mm depth per pass with a coated insert controls work hardening better than a heavy bite.

Below 0.5 mm the tool tends to rub, which hardens the surface and shortens insert life on the next pass.

Do cycle instructions work the same on every control?

The concept is the same but the block format differs. FANUC, Siemens and Mitsubishi all use two-block cycle calls with different parameter order.

Check the control manual before copying a program between machines. A swapped parameter can scrap the part on the first pass.

How do I stop chatter during a finishing pass?

Reduce the nose radius, shorten the tool overhang and check that the part is held rigidly. A 0.4 mm radius on a short holder usually clears it.

If chatter persists, lower the feed slightly and increase spindle speed rather than adding depth.

How long does it take to prove a new cycle program?

On a simple turned part, a dry run and one measured part take under an hour. Complex profiles with threads and grooves take longer because each feature is checked separately.

We quote and return a DFM analysis within 12 hours for parts sent to us, and production can start within 24 hours once the program is approved.