CNC Lathe Training Lesson 4: Cutting Speed, Feed, Depth of Cut and Machining Plan

On a CNC lathe, how you run a tool matters as much as choosing the right one. With unsuitable cutting values, even a high-quality insert wears, breaks or spoils the surface quickly. The basic cutting conditions are: cutting speed, spindle speed, feed, depth of cut, cutting width, coolant and rigidity. These values are not independent: raising the feed changes tool load and surface; increasing depth of cut raises cutting force; when the diameter changes, the spindle speed must change to keep the same cutting speed.

So the S180 and F0.20 seen in a program are not random numbers: the S value defines cutting speed or spindle speed depending on the mode, and the F value defines feed. In setting them, the programmer weighs material, insert, roughing/finishing, diameter, machine power, rigidity, workholding, required surface and chip control together. In this lesson we cover what cutting speed and feed are, the spindle-speed calculation, the G96/G97 difference, the maximum-speed limit with G50, the logic of depth of cut, and how a part’s machining plan is built.

xF0x9Fx93xB7 IMAGE AREA — Cutting speed (Vc), spindle speed (n) and feed (f) concepts in one visual
Suggested alt text: “CNC lathe cutting speed, spindle speed and feed concepts”

1. Why Do Cutting Conditions Matter?

In turning, the insert removes material from the rotating part; cutting force, pressure, friction, heat and vibration arise on the tool. If values are wrong, the tool wears/breaks quickly, the part goes out of size, the surface degrades, long uncontrolled chips and vibration form, the spindle is overloaded and cost rises. Choosing values too low is not always safe either: at very low feed the tool rubs instead of cutting; at very low cutting speed some materials build up on the edge; at very small depth of cut the chip breaker cannot work effectively. The right aim is not the highest value but a stable, efficient cutting condition for tool, part and machine. In choosing cutting speed, material, tool, machine condition, chip amount, power and feed are weighed together.

2. What Is Cutting Speed (Vc)?

Cutting speed is the peripheral distance of the part surface passing in front of the tool per minute; shown as Vc, usually in m/min. For example Vc = 180 m/min means the part surface travels 180 metres per minute at the contact point. Cutting speed and spindle speed are not the same: cutting speed is the peripheral speed at the contact point, while spindle speed is how many times the part turns per minute. At the same spindle speed, a larger-diameter part’s surface travels farther, so cutting speed is higher at a larger diameter.

Diameter, Spindle Speed and Cutting Speed

The part’s circumference is π × D (D = diameter, mm). If the part turns n times per minute, the surface travels π × D × n; to convert to metres, divide by 1000:

V_c = (π × D × n) ÷ 1000  |  n = (1000 × V_c) ÷ (π × D)

Here V_c is cutting speed (m/min), D the machined diameter (mm), n the spindle speed (rpm). Once cutting speed is chosen, spindle speed and feed are calculated from it.

3. Spindle-Speed Calculation and the Diameter–Speed Relationship

Example: a 60 mm steel part is machined at 180 m/min. n = (1000 × 180) ÷ (3.1416 × 60) = 180000 ÷ 188.5 ≈ 955 rpm. In practice a close, safe value is chosen (950 or 900 rpm). But if G96 constant cutting speed is used, the control calculates the speed itself from the machined diameter.

To keep the same cutting speed (180 m/min), as the diameter shrinks the required speed rises:

This relationship matters especially in facing, stepping, taper and profile work.

xF0x9Fx93xB7 IMAGE AREA — Vc formula and the rise of spindle speed as diameter shrinks
Suggested alt text: “CNC lathe diameter-speed-cutting speed relationship chart”

4. Spindle Speed and the S Address

Spindle speed is the number of spindle turns per minute (rpm) and is given by the S address. But S1000 alone does not always mean the same thing; its meaning depends on the active G code. With G97 active, S1000 = 1000 rpm; with G96 active, S180 = 180 m/min cutting speed. So the S value must always be read together with the active G96/G97 (and G50) state.

5. G97 — Constant Spindle Speed

G97 is constant spindle-speed mode. For example G97 S1200 M03: selects constant-speed mode, defines the spindle at 1200 rpm, turns it clockwise. In this mode the speed does not change even if the tool moves to different diameters (1200 rpm at Ø60, Ø40, Ø20); but the cutting speed changes with diameter. G97 is used especially for drilling, tapping, threading, parting, operations needing a set speed, or a controlled low speed on first approach.

6. G96 — Constant Cutting Speed

G96 enables constant cutting speed (constant surface speed) control. For example G96 S180 M03 selects 180 m/min. With G96 active, the CNC tracks the tool’s X diameter and changes the spindle speed automatically: at a large diameter the speed drops, as the tool nears a small diameter the speed rises; thus surface speed stays roughly constant. G97 cancels this control.

Why used? If a part is machined from Ø100 to Ø30 with constant speed, the cutting speed is too high at the large diameter and too low at the small one, which spoils tool wear and surface. With G96 the insert works in a more balanced condition at different diameters; it is very useful in OD and facing. In facing, as the tool moves X100→X0 the speed keeps rising as the diameter shrinks; theoretically near X0 the required speed goes to infinity, which is neither possible nor safe on a real machine. So with G96 a maximum-speed limit must always be set.

xF0x9Fx93xB7 IMAGE AREA — G96 constant cutting speed (speed varies with diameter) vs G97 constant speed comparison
Suggested alt text: “CNC lathe G96 constant cutting speed vs G97 constant speed”

7. G50 — Maximum Spindle-Speed Limit

When G96 is used, the speed rising as the diameter shrinks must not exceed the chuck’s safe speed limit, the part’s clamping capacity, the machine’s maximum speed or the part’s mechanical strength. So a limit like G50 S2500 is usually set: “the spindle speed must never exceed 2500 rpm.”

G50 S2500 ;
G96 S180 M03 ;

In this program the CNC tries to keep 180 m/min; if the calculated speed exceeds 2500, the spindle is limited to 2500 rpm. Maximum speed is chosen not only by the machine’s top speed but by considering the chuck’s permitted speed, part diameter/overhang, clamping pressure, eccentric mass and whirling in long parts. For example a machine may reach 4000 rpm, but turning a large-diameter, long-overhang part at 4000 may not be safe. So the G50 value is set by the speed at which the clamped part can safely turn, not by what the machine can reach.

8. G96 vs. G97

G96 and the X coordinate: with G96 active, the CNC computes the required speed from the tool’s X coordinate. If the workpiece zero, tool geometry or X offset is wrong, the control perceives the diameter incorrectly and computes the wrong speed. So G96 is not just a speed command; its correct operation depends on the workpiece coordinate, the tool offset and the real X position.

9. Factors Affecting Cutting Speed

• Workpiece material: higher speed in soft/easy materials, lower in hard/difficult ones. Not only hardness but thermal conductivity, sticking tendency, work hardening and abrasiveness matter (e.g. stainless steel needs special conditions due to work hardening and low thermal conductivity even if not very hard).
• Cutting-tool material: HSS low, carbide high, ceramic/CBN very high in suitable applications, PCD high in non-ferrous.
• Roughing/finishing: in roughing, depth of cut and feed are high so cutting speed is often lower; in finishing, with suitable rigidity a higher speed can be used.
• Continuous/interrupted cutting: on an interrupted surface (hole, groove, casting skin) the tip is impacted each turn; a tougher tip, stronger edge and lower speed are needed.
• Machine/workholding rigidity: worn slides, a weak holder, long overhang, low chuck force and a thin part limit cutting speed.
• Coolant: coolant cools the cutting zone, flushes chips and extends tool life; but interrupted cooling can thermally crack some ceramic inserts. Use is set by the manufacturer’s recommendation.

10. Feed (F), G99 and G98

Feed is the tool’s cutting motion relative to the part. The most common unit in turning is mm/rev: F0.20 means the tool advances 0.20 mm per part revolution. Feed directly affects machining time, surface quality, chip thickness, cutting force, tool life and chip breaking.

• G99 — feed per revolution (mm/rev): mostly preferred in turning. E.g. G99 ; G01 Z-40 F0.25 ; → the tool advances 0.25 mm per part revolution. Advantage: even if the speed changes with diameter under G96, the chip thickness per revolution stays constant.
• G98 — feed per minute (mm/min): time-based. E.g. G98 ; G01 Z-40 F150 ; → the tool advances 150 mm/min. Used in drilling, milling and driven-tool applications; in standard turning, feed per revolution is more meaningful.

Relationship: feed per minute V_f = f × n. For example f = 0.20 mm/rev and n = 1000 rpm gives V_f = 200 mm/min; at 1500 rpm, V_f = 300 mm/min. In G99 mode, though the F value stays the same, the tool’s real per-minute motion rises as the speed increases.

xF0x9Fx93xB7 IMAGE AREA — Relationship of feed to surface marks and nose radius
Suggested alt text: “CNC lathe feed, nose radius and surface roughness”

11. Feed, Surface Quality and Nose Radius

As feed increases, the spacing between tool marks grows: low feed leaves finer marks, high feed more pronounced marks. But very low feed is not always a good surface either: if the feed is smaller than the cutting-edge roundness, the tool rubs instead of cutting, the surface smears, and heat and sticking rise. The right feed must suit the nose radius, chip breaker, material and depth of cut.

Theoretical surface roughness is roughly evaluated by:

R_a ≈ f² ÷ (32 × r_ε)

Here f is feed (mm/rev), r_ε the nose radius (mm). This formula is for ideal geometric conditions; the real surface is also affected by vibration, wear, sticking, machine backlash and cutting speed. At the same feed, a 0.8 mm nose radius leaves a theoretically smoother surface than a 0.4 mm one; but a large radius increases cutting force and can vibrate a thin/long part.

Factors Affecting Feed

Roughing uses higher feed + large depth of cut; finishing lower feed + small depth. Higher feed in soft materials, lower in hard; but in aluminium a very low feed can give a poor result due to sticking. Carbide/coated inserts run at higher feeds than HSS. High feed on a long/thin part causes bending, vibration and taper; a long part needs lower feed. If machine power, torque, turret rigidity and chuck capacity are insufficient, high feed cannot be used.

xF0x9Fx93xB7 IMAGE AREA — Depth of cut (ap) and pass distribution diagram (Ø60→Ø40, 10 mm radial)
Suggested alt text: “CNC lathe depth of cut and pass distribution diagram”

12. Depth of Cut (ap) and Passes

Depth of cut is how far the tool plunges radially into the part; shown as ap. In OD turning: ap = (D_start − D_final) ÷ 2. For example machining a part from Ø60 to Ø52 gives a diameter difference of 8 mm and a radial depth of 8 ÷ 2 = 4 mm; the program says X52. In the shop “4 mm pass” sometimes means radial, sometimes “drop 4 mm on diameter”; to avoid confusion, radial pass and pass on diameter should be stated explicitly.

Pass distribution: to reduce Ø60 to Ø40, the total radial stock is (60−40)÷2 = 10 mm. At 2 mm radial per pass, 10÷2 = 5 roughing passes are needed (Ø56, Ø52, Ø48, Ø44, Ø40). But if a finishing allowance is left, roughing does not go to the final diameter. Finishing allowance: if the final diameter is Ø40 and 0.4 mm is left on the diameter, the rough diameter is Ø40.4; radial allowance (40.4−40)÷2 = 0.2 mm. So 0.4 mm on diameter = 0.2 mm radial. In cycles like G71, whether the X finishing allowance is read as diameter or radius must be verified per control system (in some cycles U values are in radius).

Factors Affecting Depth of Cut

The insert maker gives a minimum, recommended and maximum depth of cut for each geometry; at too small a depth the tool rubs, at too large a depth the tip breaks. Depth of cut must suit the nose radius and cutting-edge length; machine power, part rigidity and tool overhang must be considered. A long/thin part bends under a large pass; the diameter comes out tapered and vibration occurs. On boring bars, pass, feed and overhang are evaluated together.

13. Cutting Force, Chip Section and Material Removal

Cutting force rises as depth of cut, feed and cutting speed increase, but their effects differ. Increasing depth of cut enlarges the section and raises force significantly; increasing feed thickens the chip, makes surface marks more visible and shortens time; increasing cutting speed raises temperature and speeds wear but can improve the surface in a suitable range. Theoretical chip section A = ap × f (e.g. 2 mm × 0.25 = 0.5 mm²); material-removal rate is roughly Q = Vc × ap × f. These relationships show why a large pass with high feed cannot be used at once on every machine. Continuously raising all three for productivity is wrong; the limit is set by tool, machine, part, workholding and surface requirement.

14. Roughing and Finishing Cutting Values

In roughing the aim is to remove excess material stably and fast: medium/low cutting speed, medium/high feed, large depth of cut, strong insert and chip breaker. In finishing the aim is final size and surface quality: low feed, small depth, sharp/suitable geometry. The values below are educational starting examples only; real values come from the manufacturer catalogue per material, insert grade, chip breaker, holder, machine power and workholding.

Example pass plan: raw Ø60, final Ø40, 0.4 mm finishing allowance on diameter → rough final diameter Ø40.4; radial stock for roughing (60−40.4)÷2 = 9.8 mm. At ~2 mm radial per pass: Ø56, Ø52, Ø48, Ø44, Ø40.4; then finishing to Ø40. To avoid a too-small last roughing pass, the passes can be distributed evenly: 9.8 mm over four passes = 9.8÷4 = 2.45 mm radial (~4.9 mm on diameter), roughly Ø55.1, Ø50.2, Ø45.3, Ø40.4. CNC cycles can distribute passes automatically, but the programmer must correctly set the total stock, finishing allowance and target pass.

15. Cutting Values in Special Operations

• Facing: the excess is removed in Z (e.g. 3 mm excess over three passes Z2, Z1, Z0). Centre height and the G96 maximum-speed limit are especially important.
• Internal: the system is less rigid; lower depth of cut and feed, a steady cutting speed, and the shortest bar overhang. OD catalogue values cannot be used directly.
• Grooving: because the whole edge cuts at once, the cutting force is high; a lower speed than OD, feed set to tool width, perpendicular/rigid mounting and chip evacuation matter.
• Parting: as the tool feeds toward the centre with G96 active, the speed can rise fast; use a suitable G50 limit or switch to G97 constant speed if needed; watch for the part dropping and chip jamming.
• Drilling: cutting speed by drill diameter: n = (1000 × Vc) ÷ (π × D). E.g. Ø12 drill, Vc = 25 m/min → n ≈ 663 rpm (~650 chosen). G97 constant speed is mostly used.
• Threading: the F value is mostly the thread pitch (F2.0 = 2 mm per revolution). Feed override is not changed like normal turning during threading; spindle and Z run synchronously. G97 is mostly used.

16. Reading Catalogue Values and Their Limits

An insert catalogue gives the material group, insert grade, chip breaker, cutting-speed/feed/depth-of-cut ranges, rough/medium/finish and coolant info (e.g. Vc: 160–240, f: 0.18–0.35, ap: 1.0–4.0). At the start you begin near the middle of the range, not at the top; watching chip, spindle load, surface and wear, you raise/lower under control (e.g. Vc = 190, f = 0.25, ap = 2). Catalogue values assume ideal conditions; in the real shop the machine may be old, the tool long, the part thin, the chuck force weak, coolant insufficient or the material hardness variable. So a catalogue value is not an exact value but a technical starting range. A single cutting speed found online should not be applied to all inserts.

What Happens at Low/High Values?

Too low: at very low cutting speed, built-up edge and a poor surface; at very low feed, rubbing, unbroken chips, rising heat; at very small depth, working below the edge roundness and rubbing. Too high: at very high cutting speed, excessive heat and fast wear, coating damage, dangerous speed; at very high feed, poor surface, part bending, tool breakage; at very large depth, spindle overload, tool deflection, tip breakage and the part slipping in the chuck.

17. Reading the Spindle Load and the Chip

On many CNC lathes the spindle load is shown as a percentage (e.g. Spindle Load 45%). The load gives an idea about tool wear, high values, chip jamming, a hard zone or tip breakage; but a decision is not made by the percentage alone (the same load means different things at large/small diameter or low/high speed; short-term and continuous limits differ). A good operator also looks at the chip: short/regular chips suggest good breaking; long spiral chips suggest low feed/wrong breaker; blue/dark chips suggest high temperature (in carbide, some heat leaving with the chip is desired); chips sticking to the tip can indicate low speed/unsuitable geometry/insufficient coolant. Chip appearance alone is not a firm diagnosis but an important indicator.

xF0x9Fx93xB7 IMAGE AREA — Example part and operation sequence (clamp→face→drill→rough→finish→chamfer→groove→thread→part)
Suggested alt text: “CNC lathe machining plan and operation sequence”

18. Machining Plan and Operation Sequence

The machining plan is the production order that decides in what sequence and conditions the raw material becomes the final part in the drawing. Starting to write a program directly with G codes is wrong; the operation plan is prepared first. When studying a drawing, determine the part’s general form (shaft, bushing, flange…), the raw material (bar, tube, casting…), the critical dimensions (precision diameter/length, thread, groove, concentricity), the workholding surface and the workpiece zero (usually the face centre).

General operation sequence (varies by part): clamp raw material → machine/part check → facing (Z0 surface) → centre drill → drill if needed → OD roughing → ID roughing → OD/ID finishing → chamfers and radii → grooving → threading → final measurement check → parting → back face in a reversed setup if needed. Key logic: facing usually first (for a clean reference surface and correct Z0); parting last (since the main clamping then ends); the thread-relief groove before threading; finishing after heavy roughing and in an order that avoids damage. In thin-walled bushings, the drill and OD order is planned per deformation.

19. Example Part: Machining Plan and Cutting-Value Plan

Raw Ø50 steel bar; finished part: total length 60 mm, front step Ø30×20, middle Ø40×30, rear Ø45×10, front chamfer 2×45°, M30×2 thread on the Ø30 section, a 4 mm groove at the thread end, a Ø12×35 centre hole, to be parted from the bar. Operation plan:

Each operation’s tool, cutting speed, spindle speed, feed, pass, coolant and measuring point must be set before writing the program. Example per-tool cutting values (starting example only):

20. Machining Time and Reducing It

For a straight turning move, the approximate cutting time is t = L ÷ (f × n) (t: minutes, L: cutting length mm, f: mm/rev, n: rpm). For example L = 100 mm, f = 0.20, n = 1000 → feed per minute 200 mm/min, time 100÷200 = 0.5 min (~30 seconds). This does not include approach, retract, tool change, speed ramp-up, measurement or operator time. The right ways to reduce time are not only raising the speed: choose a suitable insert, raise feed within the catalogue range, cut unnecessary tool moves, optimise the number of roughing passes, use cycles like G71, improve rigidity and chip breaking. For productivity, feed is kept as high as possible but is limited by surface, precision, tool life and vibration.

21. Placement of Cutting Values in the Program

In a simple tool section, cutting values look like this:

G50 S2500 ;      (max speed 2500 rpm)
T0101 ;          (tool 1 + offset)
G96 S180 M03 ;   (180 m/min constant cutting speed, spindle CW)
G99 ;            (feed per revolution)
M08 ;            (coolant on)
G00 X62 Z2 ;     (rapid approach)
G01 X56 F0.28 ;  (plunge, 0.28 mm/rev)
Z-50 ;           (cut along the length)
G00 X100 Z100 ;  (safe retract)
M09 ; M05 ;      (coolant off, spindle stop)

In the same program, different tools need different conditions; S and F must be rewritten explicitly in each tool section.

22. Program Safety, First Part and Feed Override

Before running, check: is G96 or G97 active; is S cutting speed or spindle speed; is there a G50 limit; is G98 or G99 active; is F mm/min or mm/rev; during threading is F the correct pitch; is the tool within the catalogue range; is the part suited to a safe speed; are the spindle direction and depth of cut correct. A wrong mode makes a correct-looking number dangerous: e.g. F200 is 200 mm/min in G98 but, if read as 200 mm/rev in G99, produces an extremely dangerous move.

The first part is not started at the catalogue maximum; the safe order: choose a medium/safe value → limit the max speed → do the first approach in single block → watch with low rapid and controlled feed override → check chip, load, sound, vibration → measure the part → correct in small steps if needed. Feed override changes the programmed feed by percentage (F0.30 + 50% ≈ 0.15 mm/rev); but in threading/synchronous tapping its behaviour can be limited or disabled – special care is needed. When a problem is seen, do not change all values at once; first check wear/mounting/vibration and change one variable by a small amount so you can tell which change improved things.

23. Common Cutting-Value Mistakes

• Applying a single value found online to all inserts (each grade and chip breaker differs).
• Reading the S value without checking G96–G97 (S180 is sometimes 180 m/min, sometimes 180 rpm).
• Using G96 without a G50 limit (dangerous speed near the centre).
• Mistaking a diameter change for a radial pass (Ø50→Ø46 is 4 mm on diameter, 2 mm radial).
• Leaving too little stock for finishing (the tool rubs).
• Lowering feed only by surface (chip breaking and tool action are disturbed).
• Applying roughing values directly to a long part (bending, vibration).
• Starting at the catalogue maximum; using the old S/F after a tool change.

24. Shop Reality: Not an Exact Value but the Right Method

In training, memorised values like “use 180 in steel, 300 in aluminium” are incomplete on their own; because two steel parts can differ in hardness, alloy, diameter, workholding and insert. The right approach: identify the material → find the tool code and catalogue → define the operation → read the catalogue range → compute diameter and speed → assess machine/workholding → choose a safe starting value → observe the result → optimise under control. CNC lathe mastery is not memorising a single number for each value; it is knowing how to reach the right value.

Lesson Summary

• Cutting speed Vc (m/min) is the peripheral speed at the contact point; n = (1000×Vc)÷(π×D). As the diameter shrinks, the speed rises for the same Vc.
• The S value is speed in G97 and cutting speed in G96. With G96, the max speed is limited by G50.
• Feed in turning is mm/rev (G99); G98 is mm/min. Vf = f×n. Surface roughness is roughly Ra ≈ f²÷(32×rε).
• Radial depth ap = (D_start−D_final)÷2; allowance on diameter = 2× radial allowance. Section A = ap×f, removal Q = Vc×ap×f.
• A catalogue value is a starting range; before writing the program, the machining plan and each operation’s cutting values are set. The right method is controlled optimisation, not memorisation.

Assessment Test

1. For a 60 mm part machined at 180 m/min, what is the approximate spindle speed? A) 318 B) 955 C) 1910 D) 5730 rpm
2. In G96 mode, what does S180 mean? A) 180 rpm B) 180 mm/min C) 180 m/min cutting speed D) 180 mm/rev
3. (True/False) With G96 constant cutting speed, since the speed rises as the diameter shrinks, the max speed must be limited with G50.
4. If a part is machined from Ø60 to Ø52, what is the radial depth of cut? A) 2 B) 4 C) 8 D) 16 mm
5. Which G code selects feed per revolution (mm/rev) in turning? A) G98 B) G99 C) G96 D) G97
6. If f = 0.20 mm/rev and n = 1000 rpm, what is the feed per minute (Vf)? A) 20 B) 100 C) 200 D) 5000 mm/min
7. Which mode is mostly used for drilling and threading? A) G96 B) G97 C) G41 D) G28

Open-Ended Questions

• Explain the difference between cutting speed and spindle speed using the diameter relationship.
• In which operations are G96 and G97 preferred, and why?
• Explain the difference between allowance on diameter and radial allowance with an example.
• Why are catalogue values not a direct guarantee?
• List the steps for converting a technical drawing into a machining plan.

Summary and Next Lesson

In this lesson we learned the logic of cutting speed, spindle speed, feed, passes and the machining plan; we saw the functions of G96, G97, G50, G98 and G99 and a part’s operation sequence. You can now combine coordinate, tool and cutting-value knowledge. In the next lesson we cover workholding, tool offsets and part zeroing (setup) and learn how to register the tools we chose and the workpiece zero into the machine.