G72 Face Roughing Cycle Simulator and NC Code Generator

With this free G72 face roughing simulator and NC code generator you can enter the stock, final profile, pass depth and finish allowances, watch the live toolpath simulation and instantly generate FANUC 0i-TC compatible G-code (G72 + G70). For the theory see our G72 Face Rough Turning Cycle guide, and for standard thread calculation the Thread Calculator. For roughing castings and forgings also try our G73 Pattern Repeating Simulator. For longitudinal roughing also try our G71 Rough Turning Simulator.

What is G72 and when should you use it?

G72 is the stock removal in facing cycle on FANUC lathes. The tool cuts along the X axis (in the facing direction) and steps along Z after each pass to reach the next slice. In other words, the cutting direction is radial and the pass increment is axial.

The cycle pays off in particular on:

• Short, large-diameter parts — flanges, covers, discs, pulley bodies and similar workpieces whose length is smaller than their diameter.
• Jobs with deep stock on the face — when the profile changes mainly along the length rather than the diameter.
• Limited rigidity situations — slicing a long part from the face can reduce chatter compared with longitudinal roughing.

G71 or G72? A decision table

This is the most commonly confused point on the shop floor. The two cycles do the same job in different directions.

A practical rule: if the part is longer than its diameter use G71, if it is shorter use G72 — you will normally finish in fewer passes and less time. For the final decision, look at which direction carries the thicker stock.

Block structure and parameters

On FANUC 0i-T and similar controls, G72 is defined over two lines:

G72 W(Δd) R(e) ;
G72 P(ns) Q(nf) U(Δu) W(Δw) F__ S__ T__ ;

The most critical detail: the letter W means different things on the two lines. On the first line it is the depth of cut; on the second it is the finishing allowance. Mixing them up makes the machine try to take the entire stock in a single pass.

The sign of the U and W allowances

The sign of the finishing allowances decides which side the tool leaves the stock on, and a wrong sign means scrap.

• External machining: U positive (e.g. U0.5) — 0.25 mm on radius stays outside the profile.
• Internal machining (bore): U negative (e.g. U-0.5) — the allowance stays inside the bore.
• W is usually positive, leaving stock in the Z+ direction on the face. If the face is already at final size, command W0.

Remember: U is a diameter value. When you write U0.5, the real allowance left on the surface is 0.25 mm.

Type I versus Type II

Type I requires the profile to be monotonic: the diameter must keep increasing or keep decreasing. If there is a pocket, groove or reversal in between, the control raises an alarm.

Type II allows a limited number of pockets in the profile. However, Type II is not present on every control — it is an optional feature and will not work if it was not specified when the machine was purchased. If you are not sure whether your control has it, designing the profile to obey the Type I rule is the safest route.

How the control tells Type I from Type II depends on the content of the block addressed by P: if that block contains Z motion only it is read as Type I; if it contains both Z and X it is read as Type II.

Worked example: face roughing a Ø120 flange

Stock Ø125 × 30 mm; target profile: Ø120 outside diameter with a step down to Ø80 at 12 mm depth from the face. Material 1040 steel, coated carbide.

O0072 ;
G21 G18 G40 G99 ;
G50 S2200 ;
T0101 M08 ;
G96 S180 M03 ;
G0 X130. Z2. ;

G72 W2. R0.8 ;
G72 P100 Q160 U0.4 W0.1 F0.25 ;
N100 G0 Z-12. ;          ( ns block: Z MOTION ONLY )
N110 G1 X80. F0.15 ;
N120 Z-6. ;
N130 X100. ;
N140 Z-2. ;
N150 X120. ;
N160 Z0. ;               ( nf block )

G70 P100 Q160 F0.12 ;    ( finishing pass )
G0 X200. Z100. M09 ;
M30 ;

Pass count: 12 mm total depth ÷ 2 mm per pass ≈ 6 roughing passes plus one finishing pass. At 180 m/min cutting speed the spindle starts at 1000/(π×0.12) ≈ 478 rpm on Ø120; as the diameter shrinks, G96 raises the speed, which is why the G50 S2200 clamp is there.

Typical alarms and how to clear them

Alarm numbers can differ slightly between FANUC control series; always take your own machine’s alarm list as the reference.

Six common mistakes

1. Putting X motion in the ns block. In Type I that block must contain Z only; adding X makes the control assume Type II and most machines alarm out.
2. Confusing the two W values. The first is depth of cut, the second is finishing allowance.
3. Treating U as a radius value and leaving twice the intended allowance. U is on diameter.
4. Using G96 without a G50 clamp. In facing the diameter shrinks, the speed climbs fast and can exceed the chuck’s safe rpm.
5. Changing F between profile blocks. In the roughing cycle the feed comes from the F on the G72 line; F values inside the profile only apply during the G70 finishing pass.
6. Not compensating for the nose radius. Without G41/G42 in finishing, dimensional error on curved surfaces is unavoidable.

Frequently asked questions

Is G70 mandatory after G72?

Not mandatory, but it is the natural next step. G72 only removes the roughing stock and leaves the U/W allowances. G70 P Q cleans the same profile in a single pass. If you finish with a separate tool, calling G70 after the tool change is enough.

How deep can each pass be?

The limit is set by machine power, holder rigidity and insert geometry. On a mid-size lathe in steel, 2–3 mm is common. Check the required torque with the Spindle Torque Calculator and the speed and feed with the Speed and Feed Calculator.

Can G72 be used on an internal diameter?

Yes. The profile is defined on the bore and U is given as negative. Because boring bar rigidity is limited, reduce the depth of cut and make sure chips evacuate — through-tool high-pressure coolant helps a great deal.