Every sheet metal part starts as a flat blank, and getting from a dimensioned model back to that blank is where most bending mistakes happen. Three numbers decide it: the inside bend radius, the K-factor and the bend allowance. Get them wrong and flanges come out short, holes go oval and a multi-bend enclosure accumulates error until the door no longer fits. This guide works through what physically happens in the bend, which radius and K-factor to start from, how bend allowance and bend deduction differ, where holes and reliefs have to sit, and how to write a bend on a drawing so the part comes back right the first time.
Key takeaways
- Start at 1× material thickness for the inside radius on mild steel and soft aluminium, 1.5× on stainless, and 1.5–2× on 6061-T6. Tighter than that cracks the outer surface.
- The K-factor is not a material constant. It shifts with radius, thickness, tooling and forming method — 0.44 is a starting point for mild steel, and the only reliable value comes from a test bend on the actual tooling.
- Bend allowance and bend deduction are two routes to the same flat length. Know which convention your CAD system expects, because entering the wrong one doubles the error.
- Most bend defects are location defects, not process defects. A hole too close to the bend, a flange too short for the V-die, or a missing corner relief will scrap a part regardless of how good the brake is.
- SanJun runs the calculation, then proves it with a test bend. We are a sheet metal fabricator: we hold the measured dimensions and the first-article record, and we do not issue listings or certificates of compliance, and we do not run UL 9540A.
What actually happens when sheet metal bends?
When a press brake folds a sheet, the outside surface of the bend stretches and the inside surface compresses. Between those two zones sits a plane that does neither — the neutral axis. Everything in bend calculation flows from where that neutral axis sits, because the neutral axis is the only part of the material whose length you can predict.
That is the whole reason flat patterns go wrong. A flat blank is cut to the length the neutral axis will need after forming, not to the sum of the outside dimensions. If you dimension a part by its outside faces and then cut the blank to that number, every bend adds error, and a part with four or five bends ends up measurably short.
Two more properties of the bend follow from the same mechanics. The material work-hardens at the bend, which is why stainless and hard aluminium both spring back more and crack sooner than mild steel. And the region around the bend is a forming zone: anything sitting in it — a hole, a slot, a tab — will be pulled out of shape as the material flows.
Which inside bend radius should you specify?
The inside bend radius is the radius on the inside face of the bend. It is set by the punch tip radius and the die opening, and it drives both cracking risk and flat-pattern accuracy. Bending too tightly cracks the outer surface; the practical floor is roughly one material thickness for mild steel and soft aluminium, and more for harder alloys.
| Material | Minimum inside radius | Why | Notes |
|---|---|---|---|
| Cold-rolled steel (SPCC / DC01) | 1.0 × thickness | Most forgiving of the common sheet metals | Bend perpendicular to the grain where the part allows it |
| Stainless 304 / 316 | 1.5 × thickness | Work-hardens quickly at the bend | Expect noticeably more springback than mild steel |
| Aluminium 5052-H32 | 1.0 × thickness | The most bendable common aluminium alloy | Our default aluminium for bent enclosures |
| Aluminium 6061-T6 | 1.5–2.0 × thickness | Cracks easily in the T6 temper | Annealing or a softer alloy is usually the cheaper fix |
| Galvanized steel (SGCC / SECC) | 1.0 × thickness | Similar to mild steel | Zinc protects cut edges sacrificially after bending |
If a drawing does not call out a radius, most fabricators default to roughly 1× thickness, which is the safest and most economical choice, and the one your tooling rack is most likely to already hold. Two rules make the radius cheap: use one consistent radius across the whole part so no tool change is needed, and bend perpendicular to the roll ing grain wherever the flat pattern allows it, because a bend running with the grain cracks at radii that would otherwise be fine.
What is the K-factor, and where does the neutral axis sit?
The K-factor is the position of the neutral axis expressed as a fraction of material thickness, measured from the inside face. If the neutral axis sits at 44% of the thickness up from the inside surface, K = 0.44.
The important and frequently missed point is that the K-factor is not a material constant. It moves with the bend radius, the thickness, the tooling, and whether the bend is air-bent, bottomed or coined — and it moves with the alloy, which is why the material selection guide is worth reading before the flat pattern is programmed. A K-factor copied from a table will get you close; one measured on the machine will get you a part that fits.
| Material | Typical K-factor (air bending) | Practical starting point |
|---|---|---|
| Soft aluminium (5052-H32) | 0.38–0.42 | 0.40 |
| Mild steel (SPCC) | 0.40–0.46 | 0.44 |
| Cold-rolled steel | 0.42–0.44 | 0.44 |
| Stainless 304 / 316 | 0.38–0.45 | 0.42 |
| Hard aluminium 6061-T6 | 0.42–0.45 | 0.44 |
These are starting points, not absolutes. The only way to get a K-factor accurate to within a few thousandths is to bend a test coupon on the shop's exact tooling and back-calculate from the measured result. That is also why the K-factor belongs on the first-article record: once a material, thickness and radius combination has been proven, the value can be reused the next time that combination comes through, and the second program does not pay for the first program's learning curve.
How do bend allowance and bend deduction differ?
Both answer the same question — how long is the flat blank — and they simply approach it from opposite ends. Confusing them is one of the most common sources of a systematically short or long part.
- Bend allowance (BA) is the arc length of material consumed along the neutral axis through the bend. It is added to the straight legs: BA = (π ÷ 180) × θ × (R + K × T), where θ is the bend angle in degrees, R the inside radius, K the K-factor and T the thickness.
- Bend deduction (BD) is what you subtract from the sum of the outside flange dimensions: Flat length = leg 1 + leg 2 − BD.
Worked example: a 90° bend in 2 mm mild steel with a 2 mm inside radius and K = 0.44 gives BA = (π ÷ 180) × 90 × (2 + 0.44 × 2) = 1.5708 × 2.88 ≈ 4.52 mm. That is the length of material the bend consumes, and the flat pattern has to account for it.
Why it matters proportionally: on a part with four bends, a K-factor error of just 0.02 compounds into roughly 0.35–0.5 mm of total error. Against a bend angle tolerance of ±0.5° and a linear tolerance of ±0.1 mm, that is the difference between a door that closes and a door that needs a file. Most modern CAD systems compute both values automatically once you enter a K-factor — the discipline is knowing which convention your software expects and using it consistently. Our press brake bending calculator runs bend force, K-factor and bend allowance through a worked 2 mm CRS example.
Why does springback decide whether the angle lands?
Sheet metal is elastic. After the punch releases, the part relaxes back by a small amount, so a 90° bend comes off the brake at slightly more than 90°. The accepted compensation is to overbend: the tooling drives past the target angle so the relaxed part lands on it. Stainless and aluminium recover more than mild steel, so they need more compensation.
On sharp bends the recovery is commonly in the range of 1° to 3°, and more on hard alloys. Two things follow in practice. First, the compensation angle has to be measured on the same material, thickness and tooling — it is not a number you can carry across a change of alloy. Second, for a critical angle, bottom bending or coining holds the angle far better than air bending, because the material is set under pressure rather than allowed to relax. The trade is tonnage and tooling wear, so it is worth spending only where the drawing actually needs it.
What is the minimum flange length, and why do short flanges fail?
A flange has to be long enough for the V-die to grip it before the bend starts. If it is not, the part slips into the die opening, the bend lands in the wrong place, and the flange never measures true — no amount of operator skill fixes it, because the material was never supported.
The rule used on our floor, and the one worth putting on a drawing, is minimum flange length = 4× material thickness + inside radius. For 2 mm material with a 2 mm radius that is 10 mm. Below that you need a different approach: a wider flange, a smaller die opening, or a hem or return flange to give the tooling something to hold.
The related number is the V-die opening, typically 6× to 8× material thickness for air bending mild steel, and tighter for stainless and aluminium to avoid stretching the outer surface. The die opening sets the natural inside radius in air bending, which is why calling out a radius that is not on the tooling rack forces a tool change — or a compromise the operator did not tell you about.
How close can holes, slots and reliefs sit to a bend?
This is the largest single source of rework on bent enclosure parts, and it is entirely preventable at the drawing stage. Anything inside the forming zone gets dragged as the material flows, so features have to sit clear of it — measured to the tangent of the bend, not to the bend centreline, which is the mistake that makes the calculated clearance look adequate when it is not.
| Feature | Minimum clearance to bend | What happens if you ignore it |
|---|---|---|
| Round hole | 2.5 × thickness + inside radius | The hole goes oval and will not accept the fastener or connector it was cut for |
| Slot | 4 × thickness + inside radius | Slots distort more than round holes because the long edge is fully in the flow |
| Bend relief (width) | ≥ 1 × thickness | Material tears at the corner where the bend line ends on an edge |
| Bend relief (depth) | ≥ inside radius + thickness | A shallow relief does not reach past the deformation zone and tearing continues past it |
| Z-bend step height | ≥ 2.5 × thickness | Below this the tooling cannot make the part at all — it is a design change, not a tolerance question |
A food machinery customer lost 340 stainless doors to a single missing notch. The design was a 1.5 mm 304 lid with a 20 mm return on all four sides, cut and bent in one setup. On the first article, every corner split 3–5 mm down the bend line — not a crack visible in the drawing, but one you could catch a fingernail on, and in a washdown plant a contamination trap and a rejected part. The fix took four minutes at the CAM station: a relief notch at the end of each bend line. The cost was the 340 doors already cut.
What do hems, reliefs and corner joints add?
A hem — the edge folded back on itself — is the cheapest stiffness and the cheapest safe edge you can buy, but only if the return length is at least four times the material thickness. Four forms cover most work: an open hem (folded back with a gap, inside diameter at least 1× thickness) is easy to form and tolerant of coating thickness but leaves a visible slot; a teardrop hem (folded back with a rounded eye, inside diameter around 1× thickness) has no sharp slot and is the best compromise for painted or coated sheet; a closed hem is folded flat and gives the most stiffness; and a raw edge is cheapest but leaves a handling hazard.
The catch with closed hems outdoors is that they trap pretreatment chemistry and water. On an outdoor part, either specify a drain path or use a teardrop instead — a sealed pocket that cannot drain will push corrosion out along the hem within a season.
Corner joints deserve the same early attention, because they change the flat pattern rather than the finish. Welded-and-dressed, folded interlock, riveted-and-sealed and corner-post are four different nests, not four finishes on the same part, so deciding late means re-nesting the whole blank. Our hems, bend reliefs and corner joints guide covers the geometry and the nine checks we run on every flat pattern before it goes to the laser.
Which bending defect comes from which cause?
Almost every bend defect traces to one of four causes, and each has a specific fix. Tightening tolerances is rarely the answer. What does help is catching the defect at first article rather than at final assembly — the inspection plan that does that is set out in our quality control and inspection guide.
| Defect | Cause | Fix |
|---|---|---|
| Cracking on the outside of the bend | Radius too tight, or bend running with the grain | Increase radius to 1.5× thickness or more; bend perpendicular to the grain; consider a softer alloy |
| Angle out of tolerance | Springback not compensated for that material | Overbend by the measured recovery; use bottom bending for critical angles |
| Warping or twist | Uneven stress, thin stock, or unbalanced bend sequence | Balance the bend sequence; add ribs or a return flange; use standard tooling |
| Oval or displaced holes | Hole or slot inside the forming zone | Move the feature clear by 2.5×t + R (holes) or 4×t + R (slots), or machine it after bending |
| Short or misshapen flange | Flange shorter than 4× thickness + radius | Lengthen the flange, narrow the V-die, or add a hem |
How do you specify a bend on a drawing?
A bend that is fully specified removes the guesswork and the risk pricing that goes with it. State:
- Material and measured thickness — nominal thickness is not the thickness the part bends at. A 2.0 mm coil arriving at 1.97 mm bends at 1.97 mm.
- Inside bend radius — one consistent value, and one your fabricator's tooling rack holds.
- Bend angle and the tolerance on it — ±0.5° is achievable on a simple bend; ±1° is more realistic on hard-to-access or tight-radius bends.
- Which dimensions are critical — outside flange dimensions and hole positions usually are; let ISO 2768-m carry everything else.
- Burr direction where it matters — free to specify on the drawing, expensive to fix after the part is finished.
- Grain direction constraint if the part has a bend that must not run with the grain.
What not to write is "flat pattern per fabricator" alongside fully dimensioned outside faces. That puts the same dimension under two authorities, and the argument happens after the parts are cut. Our DFM design guide covers the wider set, and the tolerance guide covers what sheet metal holds on the features around a bend.
Frequently Asked Questions
What is the minimum bend radius for sheet metal?
Start at 1× material thickness for cold-rolled steel and 5052-H32 aluminium, 1.5× for stainless 304 and 316, and 1.5–2× for 6061-T6, which cracks easily in that temper. If a drawing does not call out a radius, most fabricators default to about 1× thickness. Bending perpendicular to the grain lets you work at the tight end of those ranges.
What K-factor should I use for mild steel?
0.44 is the usual starting point for cold-rolled or mild steel in air bending, with a realistic band of 0.40–0.46. Treat it as a starting point, not a constant: the K-factor shifts with radius, thickness, tooling and forming method, so the only reliable value comes from a test bend on the actual tooling and a back-calculation from the measured part.
What is the difference between bend allowance and bend deduction?
Both give the flat blank length from opposite ends. Bend allowance is the arc length consumed along the neutral axis, added to the straight legs: BA = (π ÷ 180) × θ × (R + K × T). Bend deduction is what you subtract from the sum of the outside flange dimensions. Most CAD systems compute both once you enter a K-factor — the discipline is knowing which convention your software expects.
How much springback should I expect?
On a sharp bend, recovery is commonly 1°–3°, and more on hard alloys; stainless and aluminium recover noticeably more than mild steel. The compensation is to overbend by the measured recovery for that material, thickness and tooling. For a critical angle, bottom bending or coining holds the angle far better than air bending, because the material is set under pressure rather than allowed to relax.
What is the minimum flange length for a press brake?
At least 4× material thickness plus the inside radius — for 2 mm material with a 2 mm radius, 10 mm. Below that the V-die cannot grip the flange before the bend starts, so the part slips, the bend lands in the wrong place and the flange never measures true. The fix is a longer flange, a narrower die opening, or a hem.
How close can a hole be to a bend?
Keep round holes at least 2.5× material thickness plus the inside radius from the bend, and slots at least 4× thickness plus the radius, measured to the tangent of the bend rather than its centreline. Closer than that and the feature is pulled into the forming zone: holes go oval and slots distort more than holes because their long edge sits fully in the flow.
Can you bend 6061-T6 aluminium without cracking?
Often, but not at a 1× thickness radius — 6061-T6 in that temper wants 1.5–2× thickness, and bending across the grain at a tight radius will crack it. If the design cannot take the radius, the cheaper fix is usually a softer alloy such as 5052-H32 rather than annealing, because annealing adds a process step and a distortion risk.
Do you provide inspection records for bent parts?
Yes — we measure the first article, record the K-factor and compensation used, and hold that record so the next run of the same material, thickness and radius does not repeat the setup. We do not issue listings or certificates of compliance, and we do not run UL 9540A; where a project needs a witnessed third-party test or a certificate naming a standard, that is agreed at RFQ and run by the named laboratory.
Get your bends right the first time
Bending is predictable once the three numbers are under control: inside radius, K-factor and bend allowance. Start from 1× thickness and 0.44 for mild steel, keep holes and slots out of the forming zone, give the die a flange it can grip, and confirm all of it with a test bend on the tooling that will actually run the job. Send us the drawing and we will review the flat pattern, flag the features that will move, run the calculation and return a quotation within 24 hours. For how bending fits the wider workflow, see our nine-step fabrication process.
Need CNC-bent sheet metal parts? Send your drawings for a free DFM review and a quotation within 24 hours.