Roughing & Finishing Cycles

G71 and G70 automate the bulk of lathe work. Instead of writing every roughing pass by hand, you define the finished contour once and let the controller generate the passes. This page explains the G71 format, P/Q contour rules, finish allowance, and a complete stepped-shaft example.

Concept

G71 is the stock removal turning cycle. It repeatedly cuts the raw stock down to near the finished contour, leaving a small amount of material (the finish allowance) for a final clean pass. G70 is the finishing cycle: it follows the same contour at finishing speed and feed, producing the final dimensions.

The P and Q block numbers define the finished shape. You write the contour geometry between N10 and N20 just as you would machine it in one pass — G01 lines with X and Z coordinates. G71 reads those blocks and automatically generates all the roughing passes needed to reach them. This separates geometry (what the part looks like) from process (how many passes, how deep each one is).

Why It Matters

Consider a straight cylindrical part starting at Ø50 and finishing to Ø30 over 40 mm. At 2 mm radial depth per pass, that is (50−30)/2 = 10 mm radial stock / 2 mm = about 5 roughing passes. Writing each pass as separate G01 blocks means 10+ motion blocks, and changing the depth per pass means rewriting all of them. G71 does it in one line plus the contour definition. Changing the depth from D1.0 to D1.5 changes one number — the controller recalculates the passes. The stepped example below does not cut 40 mm on every pass; see the trace note.

How It Works

Haas Single-Line G71 Format

G71 P10 Q20 D1.0 U0.4 W0.1 F0.2

After G71 finishes roughing, the part is U0.4 oversize in X and W0.1 oversize in Z. Then G70 P10 Q20 takes one clean pass at the finishing speed and feed (set with S and F before G70).

P/Q Contour Rules (Type I vs Type II)

• First block after P — if it contains X only, this is Type I; if it contains X and Z (Z may equal the current position), it is Type II. Type II does not alarm just because Z is present.
• X monotonic in Type I — the contour X must move in one direction; it does not have to be decreasing for OD (the example below goes X30→X36, increasing). Type II allows X reversal for certain profiles.
• Z monotonic — for either type, the Z direction along the contour must not reverse.
• No grooving or threading in the G71 contour — G71 is for turning contours; grooves and threads are separate operations. G73 pattern-repeating suits near-net-shape stock, not every grooved part.
• Use G18 — turning works in the XZ plane.

Example

Worked example: Stepped shaft. Start at Ø50 raw. Finished: Ø30 from Z0 to Z-20, then Ø36 from Z-20 to Z-40. Rough at D1.0 (1 mm radial per pass), U0.4 diameter finish allowance, W0.1 Z allowance. Rough S1000 F0.2; finish S1500 F0.1.

O0020 (G71/G70 EXAMPLE)
G21 G18 G97 G99 G40
G54
T0101                    (OD turning tool)
S1000 M03
G00 X52. Z2.             (approach: above stock, off face)
G71 P10 Q20 D1.0 U0.4 W0.1 F0.2
N10 G00 X30.             (first block: X only, start of contour)
G01 Z0 F0.1
Z-20.                    (turn O30 to Z-20)
X36.                     (step out to O36)
Z-40.                    (turn O36 to Z-40)
N20 X52.                 (last contour block, pull away)
S1500 M03                (finish speed)
G70 P10 Q20              (one finish pass)
G00 X100. Z100.
M30

Trace: G71 reads N10–N20 and generates roughing passes from Ø52 down to near Ø30/Ø36, leaving 0.4 mm on diameter and 0.1 mm on Z. Then G70 at S1500 takes one clean pass along the same contour to the exact finished dimensions. The N10 block is X30 only (no Z), which satisfies the first-block rule.

Choosing D, U, and W

D is the radial depth per roughing pass. It is limited by insert grade, machine rigidity, and chip load; typical steel roughing takes 1–3 mm radial. U and W are the finish allowances left on diameter and Z. U0.4 means 0.4 mm on diameter (0.2 mm radial); a finish pass of 0.2 mm radial is light enough for a clean surface but not so light that the tool rubs. W0.1 leaves a small face step for the finish pass to clean up. Too small a U risks rubbing and poor finish; too large wastes finish-pass time.

G72, G73, and G70 in Context

G72 is the face-turning cycle for parts where Z is short but the diameter changes a lot. G73 (pattern repeating) cuts the same contour repeatedly for parts with already near-net shape or irregular profiles, including grooves. G70 always runs after G71/G72/G73 to clean up. Do not put grooving, threading, or part-off inside the G71 contour; those are separate operations with their own tools and cycles.

Verifying the Cycle Before Running

After writing G71, dry-run with feed override low and watch: is the first P block Type I (X only) or Type II (X plus Z)? Do rough passes stay on the stock side? Does the tool pull away before indexing? An alarm usually means X reverses in Type I, Z reverses, or the tool starts inside the finished profile. Identify the type first, then check the matching rule.

Common Mistakes

• Grooves in the G71 contour — reversing X in Type I alarms or cuts wrong. Evaluate the part and tool access; G73 is for near-net-shape stock, not a universal groove solution.
• Mixing Type I/II assumptions — an X-only P block is Type I; adding Z selects Type II. Know which one you programmed; Z does not by itself cause an alarm.
• Forgetting G70 — G71 leaves U0.4 stock. Without G70, the part is 0.4 mm oversize on diameter.
• Wrong sign on U — for OD turning, U is positive (leaving material outside). For ID boring, U is negative.
• Rough and finish F on same line — the F in G71 is the roughing feed. In this example the finish feed F0.1 is set on the G01 Z0 line inside the contour, which G70 reads; confirm on your control.

Practice

1. U0.4 on diameter. What is the radial finish allowance?

2. Why can't Type I G71 machine grooves?

3. What does G70 do?

4. Raw stock Ø60, finish to Ø40, D1.0 per pass. How many roughing passes?

ID Boring with G71

The same G71 works for ID boring, but the sign of U flips: material is inside the bore, so the finish allowance is negative U (the bore grows toward the finished size). The first P block starts at the small bore diameter and X increases monotonically toward the finished ID. Boring bar deflection usually limits depth-of-cut more than the OD case.

Cycle Time Estimate

For an ideal straight cylinder with D1.0 radial depth and 10 mm total radial stock, expect about 10 roughing passes (the last leaves U0.4 diameter = 0.2 mm for finish). At F0.2 mm/rev and S1000 = 200 mm/min, a 40 mm effective cut length takes 0.2 min = 12 s. This is a classroom approximation for a straight part; on the stepped example below, passes below Ø36 only travel the first length, so not every pass cuts 40 mm. Ignore rapid and acceleration until you have a cycle-time study.

When Not to Use G71

Very short parts, chamfers only, or a single finishing pass do not need G71. Hand-code those directly. Parts with cross-holes, interrupted cuts, or hard scale benefit from a deliberate first pass rather than the automatic cycle. G71 shines when there is a long profile to rough repeatedly.

Verifying the First Article

After G70, stop and measure: diameter at the step, length to the shoulder, and surface finish. If the diameter is small, adjust the wear offset on that tool, not the program. If the step is off in Z, adjust the Z wear. The geometry offset stays; wear absorbs the small corrections.

Contour Block Trace (P–Q)

First move is Z on the O30 diameter, then X steps out to O36 at the shoulder — a stepped part, not a taper.

Target Allowance Table

U0.4 is on diameter (0.2 mm radial); W0.1 leaves axial stock on the shoulder. The exact rough pass sequence is computed by the control, not listed here.

U and W Sign by Cutting Side

On OD roughing, U leaves material on the outside, positive in diameter. On ID boring, the finish allowance sign flips because material is inside the bore. Always state which side you are cutting; do not infer the sign from the word "bore" alone. W leaves axial material on the shoulder that the finish pass will clean up.

Reading the First-Part Result

After G70, measure. If the front diameter is 30.10 instead of 30.00, and positive X wear moves the tool outward (larger diameter), reduce X wear by 0.10 in a diameter field (0.05 in a radius field) for the next part; confirm the sign convention on your control. If the shoulder lands at Z−19.8 instead of −20.0, adjust Z wear accordingly. Material already removed cannot be restored; corrections apply to subsequent parts only.

Reading a G71 Alarm on the First Block

Common causes: the P block starts with a move that reverses X inside Type I, the Z direction changes along the contour, or the tool starts inside the finished profile instead of above the stock. Walk through N10→N20 block by block and compare against the part. Do not increase D to "force" the cycle through; that hides a geometry error.

Roughing vs Finishing Feed and Speed

Roughing favors depth over surface finish; finishing favors light cuts at higher speed. The same tool may run at S1000 F0.2 rough and S1500 F0.1 finish. These are classroom starting points; the insert manufacturer's data and the machine's rigidity determine the real values.

Why U0.4 Means 0.2 mm Radial

U is on diameter. On a turned part, diameter is twice the radius, so leaving 0.4 mm on diameter leaves 0.2 mm on each side radially. G70 takes that 0.2 mm radial light finish cut. W0.1 is axial: the shoulder at Z−20 is left at Z−19.9 after roughing, and the finish pass steps it to −20.0. The allowance table shows these final positions; the internal step-down path is computed by the control.

Roughing Feed vs Finishing Feed

G71 uses the F on its own line for roughing (F0.2). G70 reads the feed from the contour blocks, where the example sets F0.1 on the G01 Z0 line. That is why the same contour can be rough-fed fast and finish-fed light without rewriting the geometry.

Checking Diameter Allowance and Shoulder Allowance Separately

After roughing, the two diameters are O30.4 and O36.4 (each 0.2 mm radial over finished), and the shoulder sits at Z−19.9 instead of −20.0. Before changing any offset, check the program target, U/W allowance, G54 datum, geometry offset, measurement, and deflection. If a diameter error remains after those checks, X wear is the correction; for a shoulder error, check Z path and datum before Z wear. P/Q describes the finished contour that G70 follows; it is not a record of every rough pass the control took.

When to Use G71 vs a Straight Roughing Pass

G71 pays off when the stock is a long cylinder and the profile has several diameters or a taper. For a single short shoulder, hand-coded G01 blocks are faster to write and easier to verify. Match the cycle to the part, not to the other way around.

Sources

• Haas G71 Stock Removal in Turning.
• Haas G70 Finishing Cycle.