Good sheet metal design (DFM) comes down to respecting three things the press brake cannot ignore: bend allowance, the K-factor of your material, and relief cuts at bends and corners. Get them right and a flat pattern folds to print on the first article; get them wrong and flanges land long, corners tear, and holes near bends distort. In our AS9100-certified Ahmedabad shop we form parts on a 160-tonne, 3200 mm press brake, and the blanks that fold cleanly all share the same discipline. This guide walks through the bend-allowance maths, realistic K-factor values, minimum flange and radius rules, and where to place relief cuts — with the numbers we actually use when reviewing a quote. Whether you model in SolidWorks, Fusion or Onshape, the physics of cold-forming steel is identical, and design for manufacturability is what turns a tidy CAD model into a cheap, repeatable part.
Key Takeaways
- Flat length is not flange sum: good sheet metal design subtracts a bend deduction, because the neutral axis stretches.
- K-factor is measured, not guessed: realistic mild-steel values are 0.38–0.44, not the CAD default of 0.5.
- Relief prevents tears: bend relief at least as wide as the thickness, plus corner relief where two bends meet.
- Mind the minimums: inside radius ≥ 1× thickness, flange ≥ roughly 4×T + R.
- Keep holes clear: ≥ 2.5×T + R from a bend, ≥ 2×T from an edge.
Bend allowance and the neutral axis
When sheet metal bends, the inside surface compresses and the outside stretches. Between them lies a layer that does neither — the neutral axis — and its length sets your flat blank. That is why you cannot just add flange lengths: the neutral axis sits inside the geometric centre, shifted toward the inside radius, so a naive flat pattern always comes out too long. The bend allowance (BA) is the arc length of that neutral axis through the bend. To lay out a single-bend part:
- Read the two outside flange lengths, A and B, from the model.
- Bend allowance: BA = (π ÷ 180) × angle × (R + K × T), where angle is the bend angle, R the inside radius, T the thickness, and K the K-factor.
- Bend deduction: BD = 2 × (R + T) × tan(angle ÷ 2) − BA.
- Flat length = A + B − BD.
For a 90° bend in 2 mm steel at a 2 mm inside radius with K = 0.4, BA ≈ 4.4 mm and BD ≈ 3.6 mm — so a part measuring 100 mm across its two outside flanges needs a blank near 96.4 mm, not 100. Miss that 3.6 mm and every downstream hole shifts out of position. Sound sheet metal design (DFM) starts with this arithmetic.
K-factor: what it means and realistic values
The K-factor is the fraction of the thickness at which the neutral axis sits: K = t ÷ T, where t is the distance from the inside face to the neutral axis, so it ranges from 0 to 0.5. It rises with the bend radius relative to thickness and with the forming method — tight radii and soft metals push the neutral axis inward (lower K); generous radii and harder tempers push it toward the centre.
| Forming method | Inside radius (R) | Typical K-factor |
|---|---|---|
| Air bending, soft aluminium | R < T | 0.33 |
| Air bending, mild steel | R ≈ 1–3× T | 0.38–0.42 |
| Bottoming | R ≤ T | 0.42–0.45 |
| Coining | R < T | 0.45–0.50 |
DIN 6935, the German standard for cold bending of flat steel, defines bend-allowance calculation with a correction factor that encodes K as a function of the inside-radius-to-thickness ratio — the same physics CAD tools approximate with one K value.
Do not trust a CAD default blindly: SolidWorks ships 0.5, yet real air-bent mild steel is nearer 0.38–0.44. When tolerances are tight we bend a test coupon, measure the developed length, and back-calculate K for that exact lot — full material traceability means we know the grade and gauge precisely. That empirical step separates a first article that passes CMM inspection from one chasing the print by a few tenths. Reliable sheet metal DFM treats K-factor as measured, not assumed.
Minimum bend radius and flange length
Two limits catch designers most often. First, minimum inside bend radius: bend too tight and the outer fibres crack, especially in high-strength or hardened alloys. A safe default is an inside radius ≥ material thickness (1×T) for mild steel and most 5052 aluminium; 6061-T6 and stainless want 1.5–2×T because they work-harden. Grain direction matters too — bending across the rolling grain resists cracking better than along it.
Second, minimum flange length. A flange must reach across the die opening or it will not form — it just drops into the V. A practical rule is a flange of about 4×T plus the bend radius; on our 160-tonne brake with a standard die, a 2 mm part wants a flange of roughly 8–10 mm minimum. Shorter flanges need special tooling and cost more. We flag both during the 24-hour quote review. A Pune-based enclosure client kept calling out 5 mm flanges on 2 mm sheet; they formed inconsistently until we lengthened them to 10 mm. Good sheet metal design (DFM) sizes the flange around the tooling, and ties directly to how the blank is first laser-cut to size.
Relief cuts: bend relief and corner relief
Relief cuts stop metal tearing where a bend meets an unbent region. Two kinds matter:
- Bend relief: a small notch at each end of a bend line so the material folds without dragging the adjacent web. Make it at least as wide as the thickness (≥ T) and slightly deeper than the bend radius (≥ R + T). Skip it and you get a torn, distorted corner no pressure will fix.
- Corner relief: where two bends meet, remove material at the intersection — a round or square cut-out sized ≥ T — so the flanges do not collide or pucker, leaving a clean gap for welding or sealing.
These features are cut into the flat blank, so they cost nothing extra when the DXF geometry is right; trouble starts only when relief is forgotten and we must flag a redesign. On one iDEX-linked bracket, adding 2 mm bend reliefs turned a part that cracked on every third piece into a 100% yield run. Robust sheet metal design (DFM) puts relief geometry in at the CAD stage, not after the first batch tears.
Holes, tolerances and a quick DFM checklist
Solid sheet metal design keeps features clear of the bend zone, because features placed too close to a bend distort as the metal flows. Keep holes and slots at least 2.5×T plus the bend radius from the bend line; nearer than that and round holes pull into ovals. Hole-to-edge distance should be at least 2×T so the edge does not bulge. For general tolerances we default to ISO 2768-m (medium) on linear and angular dimensions unless the drawing states otherwise, and call out each critical feature with its own tighter band verified on the CMM; angular bend tolerance on a sound setup runs about ±0.5°, tightening with coining. Before a part reaches the floor, run this check:
- Uniform thickness — one sheet gauge throughout.
- Consistent bend radii — reuse a single radius so we swap tooling less.
- Relief and corner cuts present at every bend intersection.
- Holes ≥ 2.5×T + R from bends, and ≥ 2×T from edges.
- Tolerances stated — do not over-tighten what forming cannot hold.
Send that blank to our CNC press-brake bending and sheet-metal service and it forms right the first time.
Frequently Asked Questions
How do I calculate the flat length of a bent part?
Compute the bend allowance, BA = (π ÷ 180) × angle × (R + K × T), then the bend deduction, BD = 2 × (R + T) × tan(angle ÷ 2) − BA, and subtract BD from the sum of the outside flange lengths. For multi-bend parts, sum the deductions. When in doubt, send the 3D model and we will develop the flat pattern for you.
What K-factor should I use for mild steel?
For air-bent mild steel, 0.38–0.44 is realistic, with 0.4 a safe starting point. Softer aluminium sits nearer 0.33 and coined parts approach 0.5. For tight tolerances we bend a coupon and measure the real value for your material lot.
Why does my part need relief cuts?
Without bend relief, the material at the ends of a bend tears or distorts because it cannot flow freely. A relief notch at least as wide as the thickness and deeper than the bend radius lets the flange fold cleanly, and corner relief does the same where two bends meet.
Can you fix DFM issues in my file?
Yes — every quote gets a 24-hour engineer review that flags tight radii, short flanges, missing relief and crowded holes, with suggested fixes. We can also cut and form a first article for CMM verification before a batch, since there is no minimum order quantity.
Sheet metal design that folds to print on the first article is engineered, not hoped for — bend allowance, an honest K-factor, adequate relief and sane tolerances do most of the work. Send us your STEP or DXF with the material and thickness, and an engineer will return a flat pattern, a manufacturability review and a firm price. Request a 24-hour quote.