CostKit

Sheet Metal & Press Parameters

Sheet metal quotes rarely disagree over arithmetic; they disagree because nobody can say what radius the part is bent at and how much clearance the die carries. Too tight a radius tears the outside, too little clearance leaves burrs nobody can remove cheaply, and uncompensated springback puts every assembly hole out of position — and all three move cost out of "processing" and into rework and die repair. This page collects bend, blanking, springback and tooling figures in one place, with what fails outside each range.

Sheet metal parameters move with material temper, rolling direction, die condition and press rigidity. The values below are a digest of common handbook and shop-floor ranges: general starting points, not mandatory clauses. Final numbers come from trial parts and the die maker's recommendation. The references at the foot of the page cover the bend-allowance method (DIN 6935) and general tolerance practice (ISO 2768) — they do not endorse one particular die's clearance.

1. Inside bend radius and the K-factor

Bending stretches the outside and compresses the inside, leaving a neutral layer whose length does not change. The K-factor is where that layer sits as a fraction of thickness: K = 0.33 puts it 0.33t from the inside face. Flat length follows the neutral-layer arc, BA = θ(rad) × (r + K·t) — exactly the formula behind the bend allowance calculator here, which follows DIN 6935. That is why a K that is wrong by 0.05 shifts a ten-bend enclosure blank by 3–5 mm and scraps the lot.

MaterialMinimum inside radius rminTypical r/tK at that bandWhat fails outside the range
Cold rolled steel SPCC 0.5t 1.0 0.33–0.38 Below 0.5t the outside surface tears and the inside corner wrinkles; too low a K makes the blank short and the finished size oversize
Galvanised steel SGCC 0.6t (1.0t for heavy coatings) 1.0–1.5 0.35–0.40 A tight radius cracks the zinc on the outside and exposes base metal — rust starts along the bend line within months
Electro-galvanised SECC 0.6t 1.0 0.35–0.40 Same as SGCC, but the thinner coating is more brittle and shows fine crazing at tight radii
Stainless 304 1.0t (1.2t for half-hard) 1.5–2.0 0.42–0.47 Below the limit the outside shows orange-peel or micro-cracks, and work hardening makes springback worse
Aluminium 5052-H32 0.8t (0.5t in O temper) 1.0–1.5 0.40–0.45 Too tight a radius cracks along the rolling direction; keep the bend line at least 45° to it or the crack rate doubles
Brass C2680 0.5t 1.0 0.38–0.42 Material piles at the inside corner and the outside wall thins — good ductility does not stop the wrinkling
High-strength steel DP590 1.5t 2.0–3.0 0.45–0.48 Below the limit it cracks outright, and springback scatters up to 2° across a batch — straightening will not rescue it

K is not a constant; it rises with r/t: about 0.28 at r/t = 0.3, 0.30 at 0.5, 0.33 at 1.0, 0.37 at 2.0, 0.41 at 3.0, 0.45 at 5.0, approaching 0.50 at r/t ≥ 10. At small radii the deformation concentrates through the thickness and drags the neutral layer inward; at large radii the bend approaches pure stretching and the layer returns to the mid-plane. Shops default to 0.33 at r/t ≈ 1, which is also this site's default input — but thin sheet at a tight radius (r/t < 0.5) comes out short at 0.33, and thick sheet at a large radius comes out long. Both need their own value.

Minimum radius follows ductility: cold rolled mild steel manages 0.5t, 304 stainless needs 1.0t, high-strength steel needs 1.5t. Specify below the limit and the supplier has two options — anneal first, or fail to make a good part at all. The first is cost, the second is lead time. Bend height has a floor too: roughly r + 2t, otherwise the punch cannot hold the flange and the short leg comes out as an arc instead of a corner.

2. Blanking clearance: quote it as a percentage of thickness, never in millimetres alone

Blanking clearance is the single-sided gap between punch and die, and the trade quotes it as a percentage of thickness because it scales with thickness. Clearance sets the four zones of the cut face: roll-over, burnish, fracture, burr. Done right, roughly a third of the face is burnished and the burr stays under 0.05 mm. Too small and you get secondary shear with tall hard burrs and fast edge wear; too large and the roll-over grows, the fracture band roughens and the burr curls. The cut face is itself an acceptance item — plenty of drawings simply say "burr ≤ 0.1 mm".

MaterialThickness t (mm)Single-sided clearance (%t)In millimetresWhat goes wrong off the range
Cold rolled steel SPCC 0.5–1.0 5–6 0.03–0.06 Too small: secondary shear, tall burrs, fast edge wear. Too large: big roll-over, rough fracture band, burrs that curl over
Cold rolled steel SPCC 1.0–3.0 6–8 0.06–0.24 Under-clearance on thick stock raises blanking force by 20%–30% and stalls a small press
Galvanised / electro-galvanised 0.5–2.0 5–7 0.03–0.14 Too small squeezes zinc into the edge, which peels and forces frequent die cleaning
Stainless 304 0.5–2.0 5–7 0.03–0.14 Too small accelerates work hardening and chips the edge; too large leaves hard burrs that cost more to remove than the die saved
Aluminium 5052 0.5–3.0 6–8 0.03–0.24 Too small cold-welds aluminium onto the edge and needs resharpening every few thousand strokes; too large tears the edge
Brass C2680 0.5–2.0 5–6 0.03–0.12 Too small leaves tall hard burrs; hand deburring is priced per part and easily eats the material saving
High-strength steel DP590 1.0–3.0 8–12 0.08–0.36 Too small rounds the edge within 20,000 strokes; too large leaves an almost entirely fractured face that fails the drawing

A classic mismatch: the quote says "clearance 0.1" without saying per side or total, or what thickness. On 1.5 mm cold rolled steel, 0.1 mm total means 3.3%t per side — already too tight, so burrs and edge wear arrive early. Agree on "single-sided clearance as %t" and neither side can misread it. Blanking force follows F = L · t · τ (L = shear perimeter, τ ≈ 0.8 σb) with a 1.2 safety factor; tightening clearance by one percentage point raises the force by roughly 8%–10%, which is enough to stall a small press. The stroke rate and die life built into the stamping cost calculator assume this band.

3. Springback and compensation

Springback is elastic recovery on unloading: the stretched outer fibres contract when the punch lifts and the angle opens up. It grows with the yield-to-modulus ratio and with r/t, and shrinks with tighter die clearance and more hold-down force. The engineering answer is not to calculate it exactly but to over-bend — set the die 1°–3° past nominal so the part lands on the angle after recovery — then correct from the first-off part. Stainless and high-strength steel spring back the most and scatter the most, which is why those dies usually get an adjustable angle.

Material / caseSpringback on a 90° bendCompensationWhat goes wrong off the range
Cold rolled steel SPCC (r/t ≈ 1) 1°–2° Over-bend 1°–1.5°, correct from the first-off measurement One degree off is 17 mm at the end of a 1 m part — assembly holes simply will not line up
Galvanised steel SGCC 1°–2.5° Over-bend 1.5°, raise the hold-down force to stop outer-layer slip The zinc layer is in tension on the outside, so scatter is wider than on cold rolled
Stainless 304 2°–4° Over-bend 2°–3°, or narrow the V opening Large and scattered springback: 2° spread within a batch fails any gauge
Aluminium 5052-H32 2°–3° Over-bend 2°, re-check after 24 h H32 work-hardens, and natural ageing keeps moving the angle after forming
Aluminium 5052-O 0.5°–1° No over-bend — run to nominal Annealed sheet barely springs back; applying the steel over-bend over-folds the part
Brass C2680 1°–2° Over-bend 1° Over-bending thickens the inside corner and thins the outside, showing as a colour band along the line
High-strength steel DP590 4°–6° Over-bend 4°–5°, add a bottom bead or a negative angle Without compensation the holes miss, and filing to fit is a whole extra operation
Large radius r/t > 10 Multiply the material figure by 1.5–2 Use a pressure pad or a flattening step; only trial parts settle it Springback at large radii is the hardest to control — calculation gives direction, production needs a trial die

Unspecified angle tolerance follows ISO 2768 general tolerance practice, banded by the shorter leg: about ±1° below 10 mm, ±0°20′ between 50 and 120 mm, ±0°5′ above 400 mm. In other words, one degree on a 1 m part is 17 mm at the end — "close enough" passes on a small bracket and simply will not assemble on a large one. A drawing that says "bend 90°" without a tolerance class leaves both sides with their own reading, and that ambiguity causes more disputes than the parameter itself.

4. Tooling and press: check tonnage before you discuss life

Sheet metal die cost lands almost entirely on two things: edge life and whether the press has the tonnage. Each resharpening adds 200k–300k strokes; the die does not fail suddenly, the burr just creeps up until hand deburring covers for it — a hidden cost line that ends up under "other" on the quote. Insufficient tonnage is blunter still: a stalled ram, a distorted frame, a wrecked die, and none of it appears in the price.

ItemTypical valueWhat goes wrong off the rangeCost impact
Blanking edge life (mild steel) 500k–1M strokes per sharpening A dull edge takes burrs from 0.05 mm to 0.2 mm, discovered only at assembly Die amortisation and resharpening
Blanking edge life (stainless) 200k–400k strokes Chipping and local collapse; repair means weld build-up and regrinding Amortisation doubles and lead time slips
Press-brake V-die life 100k–200k strokes A worn V groove drifts the bend angle month by month; no machine setting brings it back Replacement inserts and downtime
V opening V 6t–8t (t ≤ 3 mm); 8t–10t for plate Too small: tiny inside radius, high force, cracked outside face. Too large: big radius, big springback Sets the required tonnage and the hourly rate
Bend force (air bending) F = 1.2 × 1.42 σb L t² ÷ (1000 V), kN Exceeding the tonnage stalls the ram and distorts the frame — the die goes first Machine selection, and therefore machine cost
Blanking force F = L · t · τ with τ ≈ 0.8 σb, times a 1.2 safety factor Overload chips the edge and drops flywheel speed Machine and die strength
Die shut height Must sit between the press maximum and minimum shut height It will not fit, or it never bottoms and every part misses on height New die set or a different press

Bend force for air bending: F = 1.2 × 1.42 σb L t² ÷ (1000 V). One metre of 2 mm steel at σb 450 MPa over a 16 mm V needs about 160 kN; close the V to 12 mm and it becomes 213 kN. On a 100 t press, choosing the narrow V overloads it outright. That is why "a smaller inside radius" is never only a cosmetic request — it changes tonnage, springback and cracking risk together. How tonnage reaches cost is in the sheet metal cost calculator and machine hour rate.

How the parameters become cost

Judge on the sum of the three, not on any one being optimal: tightening clearance for a better cut face may cost more than a deburring step, and pushing the radius to its limit may cost annealing and cracking.

The eight numbers to ask for at quotation

  1. Material grade and temper (SPCC or DP590, O temper or H32 — same thickness, completely different springback)
  2. Thickness and thickness tolerance (tolerance decides whether clearance needs an offset)
  3. Inside radius and bend height (both, not just the angle — a die cannot be laid out from an angle alone)
  4. K-factor or bend allowance (whoever calculates the blank owns the result; do not let "experience" estimate it)
  5. Single-sided blanking clearance, written as %t with the thickness beside it
  6. Angle and burr acceptance (which ISO 2768 class, burr limit in millimetres)
  7. Die life commitment (how many strokes, how many resharpenings included)
  8. Press tonnage and V opening (they set how thick and how long the part can be, and the radius floor)

A supplier who answers all eight has actually laid out the die; one who cannot is quoting "cut it long and trim on the floor". If the route is still open, start from process selection and confirm the part belongs in sheet metal at all rather than extrusion or casting.

Four common mistakes

  1. Treating the K-factor as a constant. 0.33 holds at r/t ≈ 1. Thin sheet at a tight radius comes out short, thick sheet at a large radius comes out long, and both miss the drawing.
  2. Quoting one clearance number without saying per side or total. A factor of two in the gap is a factor of three in burr height, and the argument resurfaces at die approval, inspection and repair.
  3. Assuming springback can be calculated away. It moves with material lot, rolling direction and hold-down force; calculation gives direction only, so production needs over-bend, first-off measurement and an adjustable die.
  4. Fixing the radius before checking tonnage. A smaller radius means a narrower V and force that rises inversely. Work out the force, pick the press, then choose a radius it can actually make.

Frequently asked questions

The drawing gives no inside radius — what do I use?

Start at r = t (cold rolled, r/t ≈ 1, K 0.33), the most general combination. If the design needs tighter, check the material's minimum in the second column of table one, then confirm the press can take the V opening — V is normally at least 6t and the inside radius lands near V/6. That is the physical floor behind "the radius cannot just be smaller".

Why do two suppliers differ by 4 mm on the same blank?

Most often a different K-factor (0.33 versus 0.40), then a different definition of bend deduction (outside or inside dimensions). Put K and the deduction convention in the drawing notes; it settles the 4 mm before it becomes an argument. The bend allowance tool here works from the DIN 6935 neutral-layer arc, so you can compare directly.

Why is stainless both harder to bend and prone to cracking?

304 work-hardens fast: the outer fibres harden as they deform and eat their own ductility. That is why the minimum radius is 1.0t and springback is roughly double that of mild steel. Keep the bend line at 45° or more to the rolling direction, use a softer temper, or anneal locally before bending — all three are costs that belong in the design stage.

The die was quoted at 500k strokes, but burrs appear at 200k. Whose problem?

Check three things: whether clearance followed thickness, whether the material matched the agreement (galvanised wears differently from cold rolled), and whether resharpening happened on schedule. Any one of the three being off makes half the quoted life normal. Write "how many resharpenings, and how life steps down after each" into the contract — far more useful than one total number.

Related: Sheet metal cost calculator · Bend allowance · Stamping cost calculator · Stamping die estimator · Process selection · Glossary

References

  1. Calculation of bend allowances for sheet metal DIN · DIN 6935
  2. General tolerances — linear & angular, geometrical ISO · ISO 2768-1 / 2768-2

Basis for the parameters above. Links go to the publisher or its search page; the standard text itself is sold by the publisher. Price references are public market ranges, not supplier quotations.