CNC Turning and Swiss-Type Machining: Threads, Tapers, Chatter, and the Sliding Headstock

A lathe is a kinematic machine, not a round mill: spindle speed goes as 1000·v_c/πD, so a facing pass to X0 commands infinite rpm, and Ra = f²/32r means halving feed quarters the roughness while doubling the nose radius halves it. This guide works the arithmetic behind every turned quote — Kienzle forces giving 974 N and 2.27 kW on a Ø16 316L bar, a Taylor exponent of 0.25 that turns 20% more speed into a 52% tool-life loss, ISO 68-1 thread depth of 0.61343P with a 9-pass G76 constant-area schedule, boring-bar deflection scaling as L³/D⁴ (61 µm in steel vs 21 µm in carbide at 5:1), guide-bushing clearances of 0.005–0.020 mm, and a ₹77.50 part cost that breaks even against a 3-setup conventional route at 64 pieces.

·

CNC Turning and Swiss-Type Machining: Threads, Tapers, Chatter, and the Sliding Headstock

Milling gets the attention. Turning makes the parts that hold everything together — shafts, pins, bushings, fittings, valve bodies, connector shells, surgical screws, hydraulic spools. On a marketplace, turned parts are one of the highest-volume quote categories, and the quotes are frequently wrong by 40% because the estimator treats turning as "milling but round."

It isn't. Turning is a kinematic process with a single dominant cutting edge in continuous engagement. There is no interrupted cut to average out errors, no multi-tooth averaging, no tool-path freedom. Every defect — chatter, taper, thread lead error, a 3 µm diameter drift over 500 parts — comes from the interaction of three things: the stiffness of a cantilever, the geometry of a nose radius, and the synchronization of spindle and slide.

This guide works through that interaction quantitatively: cutting forces from Kienzle, tool life from Taylor, surface finish from nose-radius geometry, thread depth from ISO 68-1, boring-bar deflection from beam theory, and the sliding-headstock architecture that lets a Swiss machine hold tolerances on parts that would whip themselves out of the chuck on a conventional lathe.

1. The kinematics: constant surface speed is not a convenience feature

A lathe's defining variable is not feed in mm/min. It is feed per revolution, because the surface is generated once per spindle rotation. Cutting speed is a peripheral quantity:

with D in mm. Feed rate in linear terms is then v_f = f\,n mm/min, and material removal rate for a straight turn is:

with v_c in m/min, depth of cut a_p and feed f in mm. Note what this says: MRR is linear in all three variables, but tool life is violently nonlinear in v_c alone (Section 3). That asymmetry is the entire economic argument for high-feed turning — take the metal off with feed and depth, not with speed.

The consequence of n = 1000v_c/(\pi D) is that a constant cutting speed requires the spindle to speed up as the tool moves toward the centerline. Facing a Ø60 mm bar at v_c = 200 m/min demands 1,061 rpm at the outside diameter and 6,366 rpm at Ø10. At the centerline the required speed diverges:

This is why every production program runs in G96 (constant surface speed) with a G50 clamp — G50 S3500 sets a hard ceiling so the chuck, jaws and bar feeder are never asked to exceed their rated speed. Programming G96 without a G50 clamp is one of the few ways to genuinely destroy a lathe: the control will chase the surface speed to the machine's absolute maximum parameter, and a 3-jaw chuck at 6,000 rpm with an unbalanced part is a fragmentation event, not a crash.

For threading, tapping and parting off, use G97 (constant rpm) instead. Thread pitch is defined per revolution, so a spindle that changes speed mid-pass while the Z-axis is interpolating at feed-per-rev produces a lead error the control cannot compensate. The same applies to bar feeders: sudden rpm changes load the bar-feed servo and can stall a heavy bar.

2. Cutting forces: the Kienzle model and what your spindle is actually doing

The specific cutting force model expresses force per unit chip area as a power law in chip thickness:

where k_{c1.1} is the specific cutting force at 1 mm chip thickness (N/mm²), m_c is the material exponent (0.18–0.35), and \kappa_r is the approach (lead) angle. Cutting power and spindle torque follow:

Worked example — 316L stainless, Ø16 mm bar, v_c = 140 m/min, f = 0.2 mm/rev, a_p = 1.5 mm, \kappa_r = 95°, k_{c1.1} = 2100 N/mm², m_c = 0.27:

Two things worth internalizing. First, 2.27 kW on a 5.5 kW spindle looks comfortable — until you realize the Kienzle estimate excludes wear (×1.2–1.3), and that stainless work-hardens, so k_{c1.1} in the cut zone is 10–20% above the handbook value. Real edge loading is closer to 3 kW. Second, note that h depends on feed, not depth of cut, while b depends on depth of cut. Because k_c \propto h^{-m_c}, thin chips are disproportionately expensive per unit volume. A 0.05 mm/rev finishing pass in 316L has k_c roughly 1.7× the value at 0.2 mm/rev. This is why "sneaking up" on a dimension with a feather pass produces poor finish, rapid wear, and a size that still isn't right.

Typical k_{c1.1} / m_c pairs worth keeping in an estimator's spreadsheet:

3. Tool life: why 20% more speed costs you half your inserts

Taylor's equation, extended for feed and depth:

For coated carbide on steel, n \approx 0.2–0.3; uncoated carbide 0.2–0.25; HSS 0.08–0.2; ceramics 0.4–0.6. Take n = 0.25, C = 300 m/min as an illustrative carbide/steel pair:

A 20% speed increase (140 → 168 m/min) cuts tool life to 48% of its original value; a 50% increase cuts it to 20%. Because T \propto V^{-1/n}, the sensitivity is set entirely by the exponent:

At n = 0.25, the exponent 1/n = 4 — life falls with the fourth power of the speed ratio. This is the single most common error in job-shop process planning: an operator bumps the override to 120% to clear a backlog, and the tooling budget triples silently over the next two weeks.

The economic optimum is not maximum tool life, either. Minimum-cost speed balances machining time against tool change time and insert cost:

with t_c the tool change time, C_t the insert cost per edge, C_o the fully burdened machine rate. On a ₹850/hr lathe with a ₹380 insert edge and 1.5 min change time, the optimum sits well above the "safe" vendor speed — roughly where 15–25 minutes of life is achieved, not 60. High-speed steel thinking ("make the tool last the shift") is expensive on carbide.

4. The nose radius is the most consequential number on the insert

A round-nose tool leaves a scallop per revolution. Pure geometry gives the theoretical arithmetic mean roughness and peak-to-valley height:

with f in mm/rev and r_\varepsilon in mm; multiply by 1000 for µm.

Feed (mm/rev) · Nose radius (mm) · R_{a,th} (µm) · R_{z,th} (µm)

0.20 · 0.4 · 3.13 · 12.5

0.15 · 0.4 · 1.76 · 7.0

0.10 · 0.8 · 0.39 · 1.6

0.25 · 1.2 · 1.63 · 6.5

0.08 · 0.4 · 0.50 · 2.0

Feed enters squared; radius enters linearly. Halving feed quarters the theoretical roughness; doubling the radius halves it. Inverting the equation gives the maximum feed for a specified finish:

Measured R_a is typically 1.5–3× the theoretical value because of vibration, flank wear, built-up edge, and side flow of material around the nose. If a drawing calls R_a 0.8 µm, design for a theoretical 0.4 µm and measure the first article with a calibrated profilometer — not with a fingernail.

4.1 Tool nose radius compensation, and the taper that isn't there

The insert is not a point. It is an arc of radius r_\varepsilon, and the control must offset the tool center so the arc tangent to the programmed path does the cutting, not the theoretical sharp corner. On a straight Z-axis turn, ignoring this costs nothing in diameter. On a taper or an arc it produces a size error of:

for a taper of included angle \theta — and the error direction flips between +X and −X cutting. A 0.8 mm nose radius on a 45° chamfer produces roughly 0.33 mm of unprogrammed offset per side. This is why G41/G42 (cutter/nose radius compensation) must be active for every taper, chamfer and radius, with the tool's nose orientation (T-word, 0–9) correctly declared. A program that turns, faces and threads correctly but produces an oversized chamfer is almost always a missing or mis-set TNRC.

4.2 Tool center height

The insert must sit on the spindle centerline within about ±0.05 mm at Ø20. Off-center high or low changes the effective rake angle. Low by 0.2 mm on a 0.4 mm nose radius turns the effective rake negative enough to rub rather than cut, generating heat and a polished, work-hardened surface — which then destroys the next insert too. On a CNC lathe, tool height is set by the holder geometry, not by shimming; check holder parallelism when a single station fails repeatedly while others run clean.

5. Threading is a kinematic constraint, not a shape

A thread is a helix that must be generated with the tool advancing exactly one pitch per spindle revolution. The geometry is fixed by ISO 68-1 (60° metric) and ISO 68 (UN):

External thread radial depth (basic profile):

Basic minor diameter of an external metric thread:

Internal thread depth:

For M10 × 1.5: H = 1.299 mm, h_3 = 0.920 mm, d_1 = 8.376 mm. The tool does not cut to d_1 with a sharp point — crest truncation means the programmed depth is 0.61343P while the finished minor diameter lands at d_1. Mixing these up produces threads that gauge loose on the wire but strip under load.

5.1 G76: constant-area infeed and the pass schedule

A naive radial infeed (plunge straight in) increases chip area quadratically with depth. By the time the tool reaches full thread depth on a coarse pitch, it is removing several times the area of the first pass, which is exactly when chatter and insert breakage occur. The standard fix is constant-area (flank) infeed, where cumulative depth after pass i is:

so each pass removes roughly equal area. Total passes for a first-cut depth \Delta_1:

For M10 × 1.5 with h = 0.920 mm and \Delta_1 = 0.30 mm, N = 9.4 → 9–10 passes. Cumulative depths: 0.920, 0.651, 0.531, 0.460, 0.412, 0.376, 0.348, 0.325 mm — note how quickly the increments collapse. The minimum-depth parameter (Q in Fanuc's two-line G76, typically 0.025–0.05 mm) prevents the cycle from grinding out dozens of 2 µm passes near the root, which work-hardens stainless and burns the tip.

Fanuc two-line form:

G76 P011060 Q0050 R0.05
G76 X8.376 Z-14.0 P920 Q300 F1.5

First line: 01 finish passes, 10 chamfer (1.0 × lead), 60 included angle; Q minimum depth; R finish allowance. Second line: X minor diameter, Z end point, P thread height in µm (radial), Q first cut in µm, F pitch. The chamfer pull-out matters more than people think — a 45° chamfer at the thread exit prevents the insert from breaking out sideways and produces a usable lead-in for a nut.

5.2 Where single-point threading loses

Single-point G76 is correct for: large diameters, precision classes (6g/6H and tighter), threads that must be concentric to a datum within 0.02 mm, and any thread with a relief or shoulder within one pitch of the end.

It is the wrong tool for: small-diameter threads in soft or gummy material (the part deflects under radial force and the thread comes out lobed), high-volume parts where a die head or thread roll is 10× faster, and thin-wall tubes where any radial force ovalizes the bore. Thread milling on a mill-turn or 4-axis lathe beats single-pointing whenever the thread is near a shoulder, in a difficult material, or on a large diameter where the part cannot be spun fast enough — the cutter is small, the force is low, and a broken tool is recoverable.

Thread rolling is the process most people forget. It cold-forms the thread instead of cutting it, producing a continuous grain flow at the root and a fatigue strength improvement of 30–100% over cut threads. If the drawing specifies a rolled thread (common on automotive studs and aerospace fasteners), cutting it produces a part that passes dimensional inspection and fails fatigue.

6. Boring: the cantilever problem, in numbers

Internal turning is a cantilever beam with a cutting force at the free end. Static deflection:

so \delta \propto L^3/D^4. Doubling overhang multiplies deflection by eight; doubling bar diameter divides it by sixteen. Nothing else in turning has that sensitivity.

Computed for a 300 N radial load:

Bar · Overhang · L/D · Deflection

Steel, Ø20 · 100 mm · 5:1 · 60.6 µm

Carbide, Ø20 · 100 mm · 5:1 · 21.2 µm

Carbide, Ø25 · 150 mm · 6:1 · 39.1 µm

Carbide, Ø32 · 224 mm · 7:1 · 60.7 µm

Solid carbide delivers roughly 3× the stiffness of steel (E \approx 580–620 GPa vs 210 GPa), which is why it becomes the default above 4:1. Tungsten heavy alloy (E \approx 360 GPa, density ~17 g/cm³) sits in the middle and has the useful side effect of lowering the bar's natural frequency out of the chatter band. Practical ceilings under finishing loads: steel ~4:1, heavy metal ~5:1, solid carbide ~6:1, tuned mass-damped bars 8:1–14:1.

Chatter onset is a stiffness-to-mass problem, not a strength problem. The first bending natural frequency of the bar is:

For a Ø20 carbide bar at 100 mm overhang (\rho \approx 15{,}000 kg/m³) this evaluates to 276 Hz. Any forcing frequency near that — a tooth-pass frequency, a spindle harmonic, a bar-feeder pulse — will regenerate vibration. The practical countermeasures, in order of effectiveness: shorten the overhang, increase bar diameter, switch to a damped bar, reduce depth of cut, then shift spindle speed 10–20% to move off resonance. Note the ordering: speed changes are last because they cost cycle time and only move you off one lobe of the stability map, while the next harmonic is often still inside the unstable region.

A useful diagnostic: if the bore tapers (larger at the mouth, smaller at depth) the bar is deflecting away from the cut — reduce depth of cut and check insert sharpness. If the bore is bell-mouthed or lobed with a repeatable pitch, it's chatter. If the diameter is correct at the start of a batch and drifts over 50 parts, it's thermal growth, and the fix is a warm-up cycle and a mid-batch offset, not a new bar.

7. Parting off: the operation that breaks the most tools

Parting is a self-induced vibration problem. The tool is a thin blade at maximum overhang, cutting a full-width chip, with decreasing stiffness as it approaches the centerline. Rules that actually hold:

Chip control is the other half. In turning, the chip must break within 20–50 mm of the edge. The relevant parameter is the chip thickness ratio and the insert's chipbreaker groove width, matched to feed: a chipbreaker rated for 0.15–0.35 mm/rev will not break a chip at 0.08 mm/rev, no matter the speed. If chips are stringy, the feed is too low for the groove — that's the fix, not more coolant.

8. The Swiss-type lathe: inverting the kinematics

Everything above assumes the workpiece is held and the tool moves. A Swiss-type (sliding-headstock) machine reverses it: the bar stock moves in Z through a stationary guide bushing, and the tools move only radially. The cut always occurs within 0.5–3 mm of the bushing face, so the unsupported length of the workpiece is effectively zero regardless of part length.

The effect on the deflection equation is total. A conventional lathe holding a Ø6 mm bar out 60 mm has an L/D of 10:1 and will deflect visibly under a 200 N cut. The same bar on a Swiss machine is supported 1 mm from the tool, and the finished 60 mm of part hangs behind the cut, not in front of it. This is why Swiss shops routinely quote 20:1 to 30:1 length-to-diameter parts that a chucker cannot hold at all.

8.1 Guide bushing clearance is the whole game

The bushing is a precision sleeve, usually micro-grain tungsten carbide, honed to R_a \le 0.1 µm. Its bore must match the bar within a window narrow enough that it feels like a manufacturing impossibility:

Material · Bar Ø range · Total diametral clearance

Free-machining steel (12L14) · 3–25 mm · 0.005–0.010 mm (0.0002"–0.0004")

Stainless 303/304 · 3–25 mm · 0.008–0.013 mm (0.0003"–0.0005")

Aluminium 6061-T6 · 3–32 mm · 0.013–0.020 mm (0.0005"–0.0008")

PEEK / Delrin · 3–25 mm · 0.025–0.050 mm (0.0010"–0.0020")

Too tight and the bar galls, seizes, and stalls the feed — potentially snapping the spindle belt. Too loose and the bar orbits inside the bushing: diameters wander part-to-part, long features cut tapered, finish goes rough, and micro-drills snap. The failure is quiet — it doesn't alarm, it just produces a tray of parts that fail incoming inspection.

Because the bushing rides the bar, bar stock tolerance sets the accuracy ceiling of the whole process. Swiss work wants centerless-ground stock, commonly held to +0/−0.013 mm on small diameters. Metric ground bar is quoted h9 or h10 — and h9 on a 12 mm bar permits 0.043 mm of minus tolerance, which is 1.7 thou, far more than the bushing window. Straightness matters too: 0.5 mm/m is the usual ceiling before the bar feeder complains. This is a real cost line in a Swiss quote; specifying "12 mm 316L" without a tolerance class on a Swiss part is a specification error, not a purchasing shortcut.

Fixed bushings (bar rotates inside a stationary carbide sleeve) give the best concentricity and are used for precision work; rotary bushings spin with the bar, eliminate sliding friction, tolerate h9/h10 stock, and suit diameters above ~16 mm. Bushingless mode — running the sliding headstock without the bushing — trades rigidity for faster setup and better concentricity on short, low-L/D parts, and is increasingly common on newer machines.

8.2 Segmented machining and the Z-axis sign convention

A Swiss part cannot be machined in one continuous pass, because the finished section would have to leave the bushing to let the tool reach further along the bar. Instead the part is machined in segments shorter than the bushing land length, each supported as it is cut.

That inverts the Z-axis convention that every lathe programmer has in muscle memory. On a conventional lathe, Z0 is the faced end and material lies in −Z, so a deeper feature is a more negative Z. On a Swiss machine, the bar extends toward the tool in +Z, so a longer part is a more positive Z, and a deeper drill is a minus offset on the headstock. A post-processor or hand-written program carrying the wrong convention produces parts that are dimensionally plausible but wrong by the feature length — and it won't crash, so it survives until inspection.

8.3 What the extra axes buy, and what they cost

A production Swiss machine carries 7–13+ axes: main and sub spindle, two or three tool platens, live tooling with B-axis, and a pickoff. That enables:

The cost is setup complexity: a Swiss job typically needs 12–36 months of operator development to run unsupervised, and the scrap cost during that learning curve is 5–10× a conventional lathe's. Guide-bushing damage and sub-spindle synchronization faults are the dominant failure modes, not crashes.

Material yield is the hidden tax. The bar must pass entirely through the bushing, so the remnant — typically 80–150 mm — is unusable. On a 3 m bar feeding 42 mm parts, 64 parts consume 2,688 mm and the 100 mm remnant is 3.3% scrap, plus the saw kerf between parts.

9. Capability comparison

Metric · Conventional 2-axis CNC lathe · Swiss-type (7–13 axis)

Workholding · Chuck or collet, fixed headstock · Collet + guide bushing, sliding headstock

Support at cut point · Up to ~4:1 L/D before deflection · Continuous, 0.5–3 mm from tool

Diameter tolerance · ±0.013–0.025 mm typical · ±0.003–0.005 mm (premium machines tighter)

Length tolerance · ±0.025 mm · ±0.005–0.010 mm

Concentricity · 0.010–0.020 mm · 0.003–0.008 mm

Turned surface finish · R_a 0.8–3.2 µm · R_a 0.2–0.8 µm

Practical part L/D · 3:1 chucked, 10:1 with tailstock · 20:1–30:1 routine

Setups for a threaded, cross-drilled shaft · 2–3 · 1

Setup time · 30–90 min · 2–6 h (first run)

Hourly rate (India, 2026) · ₹600–1,000 · ₹1,200–2,000

Note the rate gap: a Swiss hour costs roughly double. The economics only work because the Swiss machine collapses 2–3 setups into one cycle and produces parts that a chucker cannot make at all.

10. The cost model, with a worked example

Per-part cost decomposes into four terms that behave completely differently with quantity:

Worked example — Ø16 mm 316L bar, 42 mm part with a Ø10 × 20 mm journal, M10 × 1.5 thread, Ø6 through bore. Cutting times: roughing 3.9 s (two passes a_p 1.5), finishing 2.3 s, facing 0.9 s, threading 10.1 s (9 passes at 500 rpm), drilling 10.8 s, parting 6.2 s — 34.1 s of cutting. With 60% non-cutting overhead (rapids, tool changes, bar feed), t_c = 0.91 min.

Total ≈ ₹77.50 at N = 200; ₹104.50 at N = 50; ₹38.30 excluding material.

Two structural observations. First, material is 51% of the part cost — a 42 mm part is 39% of the bar's length, and the rest is kerf, remnant and the bore's swarf. Second, tooling is 21% and scales with cutting time, so a 20% speed increase (which halves tool life, per Section 3) can raise part cost even as cycle time falls. The break-even depends on C_{edge}/R_m; on a cheap insert and an expensive machine, run fast. On a ₹400 insert and a ₹600/hr lathe, don't.

Comparing to a 3-setup conventional route (4.2 min total at ₹850/hr = ₹59.50 machine cost per part):

That 64-part threshold is the whole strategic argument. Below it, the conventional lathe wins on setup and hourly rate. Above it — and for any part that physically cannot be chucked — the Swiss machine wins decisively.

11. DFM rules for turned parts

Practical rules that reduce quote price and reject rate, roughly in order of impact:

  1. Tolerances only where the function needs them. A blanket ±0.01 mm on a drawing forces a finishing pass, a slower feed, and often a second op. Call out the two or three critical diameters; let the rest run to general tolerance (ISO 2768-m).
  2. Respect the L/D. Beyond 3:1 chucked without a tailstock, expect taper and chatter, and expect the shop to quote a centre hole and live centre. Beyond 10:1, it's a Swiss or a between-centres cylindrical grind job.
  3. Avoid internal features deeper than 4× diameter. A Ø8 bore 40 mm deep (5:1) needs a carbide bar, reduced depth of cut, and a higher price. At 8:1, only a damped bar works and the quote doubles.
  4. Provide a runout groove or undercut at thread ends. Threads to a shoulder need either a relief groove (one pitch wide, to the thread's minor diameter) or a thread mill — both add cost, but a missing relief guarantees a torn thread or a broken insert.
  5. Specify thread class, not just size. "M10" is a 6g/6H default. A 4g5g or 3A class thread requires a different insert, more passes, and gauging — quote it honestly.
  6. Keep wall sections above 0.8 mm in soft materials and 1.5 mm in stainless. Thin walls deflect under radial force from boring and parting, producing oval parts.
  7. Don't mix a ±0.005 mm bore with a ±0.05 mm OD and expect one setup to hold both; that's a machine-capability question, not a programming question.
  8. Call out the bar stock spec on Swiss parts. Ground, h9, or h11 changes the achievable tolerance and the bushing setup, and it changes the material price by 15–30%.
  9. Break edges rather than deburring later. A 0.2 × 45° chamfer on every external edge is nearly free in-cycle and eliminates a ₹8–15 manual deburr per part.
  10. Don't specify a surface finish without a functional reason. R_a 0.8 µm is achievable at 0.10 mm/rev with a 0.4 mm radius; R_a 0.4 µm needs 0.072 mm/rev, which roughly doubles cycle time. If the surface is cosmetic, call R_a 1.6–3.2 µm and save the money.

12. Failure modes, diagnosed

Symptom · Likely cause · Diagnostic · Fix

Diameter drifts over a batch · Thermal growth of spindle/turret · Measure first vs 50th part at steady state · Warm-up cycle, mid-batch offset

Bore tapers (larger at mouth) · Boring bar deflection · Compare Ø at two depths · Shorten overhang, reduce a_p, carbide bar

Regular lobing / ringing · Chatter at bar natural frequency · Count lobes, estimate f_n from bar geometry · Dampened bar, shift rpm 10–20%, reduce a_p

Rough finish on finish pass · Feed too high for nose radius · Compute R_{a,th} from f and r_\varepsilon · Lower feed or larger radius

Polished, work-hardened surface · Tool below centerline, or rubbing · Check tool height and edge wear · Reset height, fresh edge, raise feed

Thread tears / gauls · Radial infeed, or lubricant starvation · Inspect flanks for smearing · Flank infeed (A60/A58), neat oil

Thread won't gauge, wire ok · Pitch diameter error from lead · Check thread with pitch micrometer · Fix G97, check spindle encoder sync

Chips stringy and wrapping · Feed below chipbreaker range · Compare f to insert groove rating · Raise feed, or change chipbreaker groove

Part snapped at parting · Dwell / re-entry into work-hardened groove · Program shows feed stop or peck · Constant feed, controlled break-through

Guide-bushing galling (Swiss) · Clearance too tight, or bar oversized · Drag marks, feed motor load · Re-set 2–6 tenths clearance at largest bar section

13. Choosing the process

The most expensive mistake in this list is not choosing the wrong machine. It's specifying a part that needs a Swiss machine and a 4:1 tolerance stack on a drawing priced for a 2-axis lathe, then discovering the mismatch after the first article fails inspection. On a marketplace, the fix is upstream: state the tolerance, the L/D, the thread class and the bar stock spec on the RFQ, and let the quotes reflect the process that can actually hold them.

All forces, deflections and costs above are computed from the stated assumptions, not measured on a specific machine. Kienzle coefficients vary ±20% between sources and batches; Taylor constants are tool-and-workpiece specific and should be replaced with your own wear-test data before being used for production economics.

More FabFlow blog posts