A 1.2 m door on a powder-coated 304 stainless cabinet does not fail because the laser cut was wrong. It fails because three bends, each one drifting by half a degree, moved the latch edge further than the gasket could absorb — and the flat pattern was never going to produce the dimension on the drawing in the first place. The arithmetic that stands between your 3D model and a panel that closes is called sheet metal bend allowance, and it is the single most under-specified number on fabrication drawings we receive. It bites hardest on the parts we build most: amplifier chassis, speaker enclosures and audio studio metal enclosures, where a lid gap of 0.2 mm is visible, audible and unshippable all at once.
Reviewed by the process engineering team at Ruijin Fenghui Precision Technology, Dongguan — 23+ years of precision fabrication, 200+ CNC machines, ±0.01 mm on machined features, IATF 16949 / ISO 9001 / ISO 13485 certified. Updated 4 October 2026.
This sheet metal bending design guide is written for the person who has to sign off the drawing: what bend allowance actually measures, how the K-factor behind it is chosen (and why published charts disagree), what springback does to a programmed angle, where the minimum bend radius really comes from, how the V-die opening quietly changes every number above, and what tolerance a brake can hold once paint and anodising are added on top. Every formula is shown with a worked example in both millimetres and inches, because mixed-unit drawings are where most of these errors are born.
What sheet metal bend allowance actually measures
Bend a strip of metal and something has to give. The inside surface of the bend is compressed, the outside surface is stretched, and somewhere between them there is a layer that keeps exactly the length it had before the punch moved. That layer is the neutral axis, and the bend allowance is the length of the neutral axis measured around the arc of the bend.
Put another way: bend allowance is the amount of material you must add to the sum of the two flat legs to get the true flat-blank length. Unfold a bracket in CAD, add the two outside dimensions together, and the flat comes out too long — always too long, because bend deduction is never negative. At R = 1T it runs at roughly 1.8 mm of deduction per millimetre of thickness: 1.8 mm on 1 mm sheet, 3.5 mm on 2 mm, 5.3 mm on 3 mm. That is ten to twenty-five times the ±0.2 mm tolerance written on the same drawing.
Three related terms do the work, and confusing them is the most common source of wrong flat patterns:
Allowance is flat-pattern arithmetic; what the formed part may deviate by is a separate question, governed by ISO 2768 and DIN 6930. See our sheet metal tolerances guide.
- Bend allowance (BA) — the arc length of the neutral axis through the bend. Added to the straight legs.
- Outside setback (OSSB) — the distance from the bend line (where the two outside faces would intersect) to the tangent point where the bend arc begins.
- Bend deduction (BD) — what you subtract from the sum of the two leg dimensions:
BD = 2 × OSSB − BA.
Everything downstream — laser nesting, flat-pattern DXFs, flange-to-hole position, whether an enclosure lid fits — depends on those three numbers agreeing with the tooling that will actually form the part. Our own custom sheet metal fabrication cell runs fibre laser, press brake, weld and finish under one roof, which is precisely why we care: when the flat is wrong, the error is not discovered at the brake, it is discovered at final assembly.
The three formulas, and what each variable really means
For a bend of angle A (degrees), inside radius R, material thickness T, and K-factor K:
BA = (π / 180) × A × (R + K × T)OSSB = tan(A / 2) × (R + T)BD = 2 × OSSB − BA
And the flat-blank length for a two-flange part whose leg dimensions are measured to the outside faces is:
Flat length = Leg 1 + Leg 2 − BD
Three things about those variables trip people up in practice.
R is the inside radius, measured after springback. Not the punch tip radius, not the nominal radius on the drawing. On air bending the achieved radius is set mostly by the die opening, which is why the same nominal R2 on a drawing can come off two different brakes as two different parts.
A is the included bend angle in degrees as the part sits finished — 90° for a right-angle flange, not 90° minus springback. Springback is handled separately, in the brake, not in the flat pattern.
T is actual measured thickness, not nominal. A coil of 2.0 mm 5052-H32 that measures 1.94 mm changes BA by 0.04 mm per bend — and across four bends that is 0.16 mm, half a ±0.2 mm band gone before anyone touches the brake.
| Variable | Where it comes from | Typical error if guessed |
|---|---|---|
| A (bend angle) | Finished drawing | ±0.5–1.0° → up to 1.75 mm at a 100 mm flange tip |
| R (inside radius) | Die opening, not the punch | ±0.5 mm → ±0.8 mm of arc length per 90° bend |
| T (thickness) | Mill certificate / micrometer | ±0.06 mm → ±0.04 mm on BA, ±0.08 mm on the flat blank |
| K (K-factor) | Material, R/T ratio, process | ±0.05 → ±0.16 mm per 90° bend on 2 mm |
That last row is the one nobody writes down, and it deserves its own section.
Sheet metal K-factor: the one number nobody agrees on
The K-factor is the position of the neutral axis expressed as a fraction of thickness: K = t / T, where t is the distance from the inside face of the bend to the neutral axis. If the neutral axis sat exactly in the middle of the sheet, K would be 0.5. In real bends it never does — the neutral axis migrates toward the inside surface as the bend gets tighter, because compression on the inside face is confined while the outside surface is free to stretch. Type K factor sheet metal into a search box and you get ten values between 0.33 and 0.50; nearly all of them are right for somebody's alloy, die and process, and wrong for yours.
The textbook table most engineers meet first looks like this:
| R / T ratio | Soft (5052-O, copper) | Medium (SPCC, 5052-H32) | Hard (6061-T6, 304) |
|---|---|---|---|
| R < T | 0.33 | 0.38 | 0.40 |
| R = 1–3 T | 0.40 | 0.43 | 0.45 |
| R > 3 T | 0.50 | 0.50 | 0.50 |
Those numbers are a reasonable starting point. They are also why flat patterns are wrong, for four concrete reasons:
- They are air-bending numbers. Bottoming and coining push the neutral axis inward differently. Coining a 2 mm bend can shift K by 0.01–0.03 against the same part air-bent.
- They ignore the die. On air bending the achieved radius is roughly
R ≈ V / 6 ≈ 0.16 × V, so the die opening — not your drawing — decides which row of the table applies. Change from a V12 to a V16 die on 2 mm material and you move R/T from 1.0 to about 1.3, which moves K. - They are averages across a temper range. "5052" covers O through H38 tempers whose yield strength differs by more than a factor of three.
- CAD defaults are not measurements. Several packages ship with a K near 0.44 — the classic reference value printed in Machinery's Handbook — and that default gets shipped to the laser cutter without ever being checked against a test bend.
A measured K is the cheapest accuracy you will ever buy. Bend a coupon of the actual coil, in the actual die, at the actual angle; measure the leg lengths; back-solve K; write that number into the process sheet. It turns bend allowance from an estimate into a process constant. A production shop doing low-volume CNC machining alongside fabrication should have a K table per material-thickness-die combination, not one global constant.
One warning worth putting in bold: if a supplier's K table lists values in millimetres, it is wrong. K is dimensionless by definition. That error appears in more than one widely read online guide.
Worked example: a 2 mm 5052-H32 bracket, in millimetres and inches
Take a simple L-bracket. Material 5052-H32 aluminium, T = 2.00 mm, bend angle A = 90°, inside radius R = 2.00 mm (1 T), die opening V = 12 mm (6 T). Legs measured to the outside faces: 50 mm and 80 mm.
Step 1 — pick K. R / T = 1.0, medium-hard alloy → K = 0.43 from the table above. If this were a production part we would confirm it with a coupon bend.
Step 2 — bend allowance.
BA = (π / 180) × 90 × (2.00 + 0.43 × 2.00) BA = 1.5708 × (2.00 + 0.86) = 1.5708 × 2.86 = 4.49 mm
Step 3 — outside setback.
OSSB = tan(45°) × (2.00 + 2.00) = 1.000 × 4.00 = 4.00 mm
Step 4 — bend deduction.
BD = 2 × 4.00 − 4.49 = 3.51 mm
Step 5 — flat blank — the number the laser cuts, and the whole point of the sheet metal bend allowance calculation.
Most of that edge condition comes off the laser, and our sheet metal laser cutting guide explains which parameter produced it.
Flat = 50 + 80 − 3.51 = 126.49 mm
Now the same part in inches, which is where the mixed-unit drawings get caught: T = 0.0787 in, R = 0.0787 in, K = 0.43.
BA = 1.5708 × (0.0787 + 0.43 × 0.0787) = 1.5708 × 0.1125 = 0.1768 in (4.49 mm) OSSB = 1.000 × (0.0787 + 0.0787) = 0.1575 in (4.00 mm) BD = 2 × 0.1575 − 0.1768 = 0.1382 in (3.51 mm) Flat = 1.9685 + 3.1496 − 0.1382 = 4.9799 in (126.49 mm)
Both systems agree to two decimals, which is the point: if your CAD model gives a different flat length, the discrepancy is almost always a K-factor or a radius definition, not the formula.
| Quantity | Metric | Imperial | Note |
|---|---|---|---|
| Thickness T | 2.00 mm | 0.0787 in | measured, not nominal |
| Inside radius R | 2.00 mm | 0.0787 in | ≈ V / 6 |
| K-factor | 0.43 | 0.43 | coupon-confirm before production |
| Bend allowance BA | 4.49 mm | 0.1768 in | neutral-axis arc |
| Outside setback OSSB | 4.00 mm | 0.1575 in | tan(A/2)·(R+T) |
| Bend deduction BD | 3.51 mm | 0.1382 in | 2·OSSB − BA |
| Flat blank | 126.49 mm | 4.9799 in | L1 + L2 − BD |
What happens if K was wrong by 0.05? ΔBA = 1.5708 × T × ΔK = 1.5708 × 2.00 × 0.05 = 0.16 mm per bend. One bend is recoverable. Four bends in the same direction is 0.63 mm of accumulated error — which is why a four-flange box drawn at ±0.3 mm is a different manufacturing problem from a four-flange box drawn at ±0.8 mm.
Sheet metal springback: why a 90° bend is not programmed at 90°
Sheet metal bend allowance tells you how long the flat must be; springback tells you what angle the brake must be programmed to. Metal is elastic: release the punch and every bend relaxes a little — the finished angle is always slightly more open than the angle that was formed. That relaxation is springback, and it is the reason a brake operator programs 88° to get 90°.
Springback scales with the ratio of yield strength to elastic modulus (σy / E) and with the bend radius ratio R/T — which is why the sheet metal material properties you pick matter more than the alloy family name on the drawing. Wide radius, high yield, thin material: more springback. Tight radius, soft material, heavy overbend: less.
| Material | σy / E × 10³ | Springback at R/T ≈ 1 | Practical note |
|---|---|---|---|
| SPCC (cold-rolled steel) | ≈ 1.2 (σy 250 MPa) | 0.5–1.5° | predictable, stable coil to coil |
| Al 5052-H32 | ≈ 2.5 | 1–3° | temper drift shows up here first |
| Al 6061-T6 | ≈ 3.9 | 2–8° | published figures disagree widely |
| SUS 304 | ≈ 1.0 | 2–5° | work hardening raises it above the ratio prediction |
| Brass (half-hard) | ≈ 2.7 | 1–3° | consistent, easy to compensate |
Two honest caveats. First, the σy/E ratio predicts the *trend*, not the number: 304 stainless springs back far more than its ratio suggests because it work-hardens aggressively during forming, which is why shops treat stainless as a separate compensation case rather than a row in a table. Second, published springback figures for 6061-T6 range from about 2° to 8° depending on whether the source measures air bending or bottoming — a spread discussed openly in press-brake literature such as The Fabricator's springback primer. For 304 and 6061-T6 treat the ratio column as a ranking, not a formula: it will tell you which compensates more, never by how much. Compensation has to be measured on the actual tool and batch.
That is what "batch-compensated bend angles" means in practice: the angle is verified on first-piece inspection, adjusted for that coil and that tool set, and then sampled through the run rather than trusted once. If your supplier cannot describe how they compensate springback, they are measuring the finished part and hoping. Ask to see the first-piece inspection records for the last run of a part like yours; they should name the coil, the tool set and the measured angle.
Minimum bend radius and grain direction: why charts disagree by 3×
Neither the sheet metal bend allowance nor the springback compensation will save a bend whose radius is below what the material can take. Search for the minimum bend radius of 6061-T6 and you will find recommendations from 1 T to 6 T. All of them are defensible, because they are answering different questions.
The physical limit comes from tensile strain on the outside surface of the bend:
ε = T / (2R + T)
Set that strain equal to the material's elongation at fracture and solve for R. For 6061-T6, with elongation in the 8–12% range, that gives R ≈ 3.7–5.8 T. For 5052-H32 at 12–18% elongation, R ≈ 2.3–3.7 T. For 304 stainless at 40%+ elongation, R ≈ 0.5–0.75 T. And for SPCC at roughly 28%, R ≈ 1.0–1.3 T.
| Material | Strain-derived radius (safe) | Commonly quoted shop minimum | When each applies |
|---|---|---|---|
| Al 5052-H32 | 2.3–3.7 T | 0.5–1.5 T | shop minimum for non-cosmetic flanges; strain radius for visible or anodised faces |
| Al 6061-T6 | 3.7–5.8 T | 1–3 T | T6 is unforgiving; bend across grain and expect surface checks at the tight end |
| SUS 304 | 0.5–0.75 T | 1–2 T | generous radius is cheap here; springback dominates anyway |
| SPCC | 1.0–1.3 T | 0.5–1 T | most forgiving common sheet; the strain row assumes ~28% elongation |
The gap between the two columns is not a contradiction. Published shop minimums assume you are bending across the grain, accepting some surface roughening, on a part that will be painted. The strain-derived column is what you use when the bend is cosmetic, anodised, load-bearing or fatigue-cycled.
Grain direction is the variable people forget. Rolled sheet has directional grain, and a bend running parallel to the grain can require roughly twice the radius of a bend running across it before the outside face cracks. On a part with bends in both directions, the tight-radius bends should be laid out across the grain during nesting — a decision that has to be made before the laser cuts, not after.
If a design genuinely needs a radius tighter than the material allows, there are three honest exits: change the temper (5052-O instead of H32, or 6061 formed annealed and then heat treated), machine the feature instead of forming it, or split the part. Our CNC milling service covers the machining route, and metal stamping versus CNC covers where forming stops making sense at all. Cosmetic faces are the worst case: a cosmetic brushed aluminium panel shows every strain line that a painted industrial bracket hides.
V-die opening and tonnage: the hidden variable behind every number above
The die opening is the variable that quietly rewrites your sheet metal bend allowance. On a press brake running air bending — which is most of them — the die opening, not the punch, sets the inside radius. The working rule is V = 6 × T to 8 × T, and the achieved radius follows at roughly R ≈ V / 6 ≈ 0.16 × V.
So a "2 mm, R2" bend is only reproducible if the die is specified too. V12 gives R ≈ 2 mm. V16 gives R ≈ 2.7 mm and a K-factor pulled from a different row of the table. That is the quiet reason two shops can quote the same drawing and deliver parts that do not interchange.
Tonnage follows the same variables. The classic imperial rule for mild steel, with T and V in inches:
Tonnage per foot = 575 × T² / V
For our 2 mm bracket in a V12 die: T = 0.0787 in, V = 0.4724 in → 575 × 0.00619 / 0.4724 = 7.5 US tons per foot, which is about 220 kN per metre. In SI form with t and V in millimetres the same relationship is ≈ 661 × t² / V kN/m — the same rule converted, not an independent standard.
| Material | Multiplier on the steel figure | Process | Multiplier |
|---|---|---|---|
| Aluminium (5052 / 6061) | 0.50–0.65 | Air bending | 1.0 |
| Brass | 0.50–0.65 | Bottoming | 3–5× |
| Cold-rolled steel (SPCC) | 1.00 | Coining | 8–10× |
| Stainless 304 | 1.45–1.60 |
Applying that: our bracket in aluminium needs about 0.6 × 7.5 = 4.5 tons per foot (≈ 132 kN/m), so a 300 mm bend length needs roughly 40 kN — comfortably inside a mid-size brake. Move the same part to 304 stainless and the requirement goes to about 7.5 × 1.5 = 11.3 tons per foot (≈ 330 kN/m), or 99 kN over the same 300 mm. Same geometry, same drawing, two and a half times the machine.
Practical consequences worth writing into the drawing: state the die opening where it matters, keep all radii in a part identical so the brake runs one setup, and remember that every die change is a setup — which is a cost item as real as material.
What the finish does to your bend
Sheet metal bend allowance gets you the right flat; the finish then moves the part after the brake has already hit its tolerance. Coatings are not free, and they are not symmetric. Two rules matter for bent parts.
Form first, coat after. Anodising, powder coating and plating are applied to the finished formed part. Coating a flat blank and then bending it cracks the film at the bend — the outside fibre of a 2 mm bend at R2 is being stretched by about a third (ε = T / (2R + T) = 33%), and no organic coating survives that.
Every coating adds thickness to every surface. Typical build, per surface:
| Finish | Typical thickness per surface | Effect on a bent assembly |
|---|---|---|
| Anodising Type II | 5–25 µm | closes clearances by roughly half the build per surface |
| Anodising Type III (hard) | 25–75 µm | MIL-PRF-8625F guidance: minimum radii of 0.79 / 1.59 / 2.38 mm for under-25 / 25–50 / over-50 µm coats |
| Powder coating | 60–120 µm | can fill thread clearance and tight hinge gaps |
| Zinc / nickel plating | 5–25 µm | small, but enough on a 0.1 mm slip fit |
| Passivation (stainless) | negligible | no dimensional impact |
The anodising split is worth stating precisely: the oxide layer grows both outward and inward, and the common rule of thumb is that about half the coating thickness appears above the original surface. Treat that as a rule of thumb, not a specification — measure it if the fit is tight.
The practical failure always looks the same sort of small. A lid is designed with a 0.05 mm slip fit, the assembly is anodised at 20 µm, and 0.02 mm of the clearance is gone — 40% of the fit, on a dimension nobody had flagged as critical. If a part is anodised, the drawing should say so on the dimension that matters, because CNC parts finishing changes the dimension after the brake has already hit its tolerance. Our anodizing aluminium page covers how the sequence is documented, and amplifier front panels shows where this sequence is decided every day.
Tolerance reality: what a drawing can actually hold
Sheet metal bend allowance is exact arithmetic applied to a process that is not. The formulas are exact; the shop is not. Here is what a well-run brake cell holds on 0.5–6 mm sheet, and what it costs to go tighter:
| Feature | Routine capability | Tight (costs more) | Why it moves |
|---|---|---|---|
| Single flange length | ±0.25–0.50 mm | ±0.10–0.15 mm | K-factor accuracy, back-gauge repeatability |
| Bend angle | ±0.5–1.0° | ±0.25° | springback compensation quality |
| Hole-to-bend position | ±0.20–0.40 mm | ±0.10 mm | accumulated from bend, not from laser |
| Across 3+ bends | ±0.8–1.6 mm | ±0.4 mm | error accumulates, it does not average out |
| Flatness on large panels | 0.5–1.0 mm over 1 m | fixture-controlled | weld distortion, not bending |
Two numbers make the cost case better than any argument. A 1° angle error moves the tip of a 100 mm flange by 100 × tan(1°) = 1.75 mm. And tightening a flange tolerance from ±0.5 mm to ±0.25 mm typically adds, in our experience, 15–40% to the bending cost, because it forces coupon calibration, more frequent sampling and slower cycle times — not because the machine is less capable. Your mileage will vary with batch size; what does not vary is the direction.
The highest-leverage thing an engineer can do is stop over-tolerancing — most bending dimensions are better served by the general tolerance classes in ISO 2768-1 than by a hand-written ±0.2 mm on every flange. Where a drawing also carries geometric callouts, ASME Y14.5 is the framework most buyers reference, and it should be named on the RFQ so both sides are measuring the same way. Our CNC machining tolerance guide covers the same principle for machined parts, and what drives machining cost shows why the last 0.1 mm is always the most expensive one.
There is also a process ceiling: once bend-related accuracy becomes the binding constraint rather than the feature itself, the part has stopped being a sheet metal part. At that point CNC prototyping or machining from solid — often simply CNC milled parts instead of a bent assembly — is cheaper than fighting the brake. Tight tolerances also complicate pressed-in nuts and studs, whose hole pattern inherits every bend error behind it.
The RFQ checklist that prevents 90% of these problems
This sheet metal bending design guide would not be worth much without a checklist, so here it is. Before you release a bent-part RFQ, have these seven items on the drawing or in the email:
- Material and temper (5052-H32, not "aluminium"), with thickness measured, not nominal.
- Inside radius stated explicitly, plus the die opening if interchangeability matters.
- Bend angle with its tolerance, and whether the tolerance applies to the finished part after coating.
- Grain-direction requirement on cosmetic or tight-radius bends.
- K-factor or bend deduction you used for any flat pattern you supply — otherwise the shop recalculates and the two flats will not match.
- Finish, with the per-surface build allowance called out on fits, threads and hinge gaps.
- Critical dimensions flagged, so inspection effort goes where the risk is — including any laser marking that has to stay inside a coated panel face.
Send STEP or DXF flats; a shop that does design-for-manufacture review will return radius standardisation and nest-efficient sizing, which typically trims 10–20% off unit price before cutting starts. That review is also where stainless steel machining or aluminium CNC machining gets proposed as a substitute for a feature the brake cannot hold — the same call we make on speaker enclosure machining when a multi-bend box cannot hold its gasket line.
FAQ
What is the difference between sheet metal bend allowance and bend deduction?
Bend allowance is the arc length of the neutral axis through the bend, and you add it to the flat legs. Bend deduction is what you subtract from the sum of two leg dimensions measured to their outside faces. They describe the same piece of geometry from opposite directions: BD = 2 × OSSB − BA.
What K-factor should I use for 2 mm aluminium 5052-H32?
Start at 0.40–0.43 for R/T around 1 in air bending, then confirm with a coupon bend in the die you will actually run. A K error of 0.05 on 2 mm material moves each 90° bend by about 0.16 mm, which is enough to lose a ±0.3 mm tolerance across four bends.
How much does springback change a bend angle?
Typically 0.5–1.5° on cold-rolled steel, 1–3° on 5052-H32, 2–8° on 6061-T6 and 2–5° on 304 stainless at R/T ≈ 1. The brake compensates by overbending; the compensation must be measured per coil and per tool set, not read off a chart.
What is the minimum bend radius for 6061-T6 aluminium?
Published figures range from 1 T to 6 T. Strain-limited calculation (ε = T / (2R + T) against 8–12% elongation) gives 3.7–5.8 T for a safe bend; 1–3 T is achievable across the grain on non-cosmetic flanges. If the bend is visible, anodised or fatigue-loaded, design to the larger figure.
Does the V-die opening change my sheet metal bend allowance?
Yes. In air bending the inside radius is roughly V/6, so changing the die changes R, which changes both BA and the R/T row your K-factor comes from. Specify the die opening on any part that must interchange between suppliers or between batches.
Should I bend before or after anodising?
Always form first, then anodise. A 2 mm bend at R2 stretches the outside surface by about a third (ε = 33%), which cracks an anodic or organic film. Budget the coating build into fits and clearances instead — the oxide grows both outward and inward, with roughly half appearing above the original surface.
How tight can bend tolerances realistically be?
Routinely ±0.25–0.50 mm on a single flange and ±0.5–1.0° on angle; ±0.8–1.6 mm accumulated across three or more bends. Halving a flange tolerance usually adds 15–40% to bending cost because it forces calibration and sampling, not because of machine capability.
Can you quote from DXF flats only?
Yes — flats plus a bend table and material specification are enough to quote, and for 3D models the flat pattern is generated and confirmed with a drawing before cutting. What cannot be quoted accurately is a flat with no K-factor and no radius, because the shop has to guess both.
Getting this right before the laser cuts
None of this arithmetic is difficult. What costs money is discovering it late: a flat pattern cut two millimetres long, an anodised lid that no longer closes, a four-bend enclosure whose accumulated error only shows up when your customer's assembly line tries to fit it.
Send the drawing before it is frozen. A supplier who runs laser, brake, weld and finish in-house can tell you which radii to standardise, where grain direction will bite, what the coating will do to the fit, and whether a feature should be machined instead of formed — usually in 48 hours, and usually worth 10–20% of unit cost. If you are comparing partners, choosing a CNC supplier is the checklist to use. This sheet metal bending design guide stops where volumes make the brake irrelevant: above a few thousand parts a year, sheet metal stamping or high speed metal stamping takes over entirely.
Talk to our engineers about your drawing — 48-hour quote, documented first articles, and bend angles compensated per tool set and per coil.