Press Brake Bending: The 16 Tonnes per Metre in a 2 mm Bend, the 0.8 mm K-Factor Error in Every Flat Pattern, and Why 304 Comes Back at 87°

Engineering guide to press brake bending: the 1.42 air-bending force equation, why the inside radius floats at 0.16 × V-die opening, K-factor and bend allowance/bend deduction arithmetic, the 0.8 mm flat-pattern error, springback in mild steel, 304 and 6061-T6, ram deflection and crowning on a 3 m brake, DFM rules and per-bend cost.

·

Press Brake Bending: The 16 Tonnes per Metre in a 2 mm Bend, the 0.8 mm K-Factor Error in Every Flat Pattern, and Why 304 Comes Back at 87°

A laser cuts a flat blank to ±0.1 mm. A press brake folds it into a bracket with four 90° bends. The part arrives at inspection with every flange 0.6 mm short, the first bend at 88.6° and the last one with a stretched hole that no longer accepts its bolt. Nothing failed. The laser held tolerance, the brake held tolerance, the operator did what the drawing said. Three modelling errors stacked up instead, and all three were in the arithmetic that happened before anyone touched metal.

Almost every enclosure, chassis, panel, cabinet, bracket and machine guard that leaves a sheet metal shop passes through a press brake, and the machine itself is unforgiving in a specific way: it is a beam, not a rigid body, and its output angle is a function of depth, not force. That combination makes sheet metal bending one of the few common fabrication processes where a designer's spreadsheet can be wrong by more than the machine's entire error budget.

This guide works through the numbers in the order a part meets them: the force the ram must deliver, the radius the die will actually produce, the flat length the blank must be cut to, the angle the material gives back when the load is released, and the deflection that decides whether both ends of a 3 m bend match in the middle.

Air bending is a three-point bend, not a die impression

An air bend has exactly three lines of contact: the punch tip and the two die shoulders. The sheet never touches the bottom of the V. The punch pushes the material into the opening, the material wraps the tip, and the angle is set by how far the tip descends below the shoulder plane. Stop the ram early and you get 120°. Push it 0.2 mm deeper and you get 88°.

This is the single most important mechanical fact about the process: in air bending, angle is a depth problem, not a force problem. Once the bend zone is fully plastic through the thickness, additional force does not close the angle further in any useful, controllable way. It marks the part, flattens the die shoulders and, at the extreme, thins the bend zone. That is why a modern CNC brake's Y-axis repeatability, typically 0.01 mm on a servo-electric machine and 0.02–0.05 mm on a proportional hydraulic one, matters more than its tonnage for angle control.

The two other forming modes behave differently:

Air bending dominates because it needs the least force, tolerates the widest material variation and lets one die set produce any angle. The price is that the radius is not yours to choose, and the angle depends on machine stiffness.

The force: where 1.42 comes from, and what it is hiding

Treat the sheet as a rectangular beam spanning the die opening, loaded at the centre. For an elastic-perfectly-plastic section, the plastic moment per unit width is:

A simply supported span carrying a central load P develops M = PL/4 at mid-span, so collapse occurs at:

where V is the die opening and b the bend length. That is the whole structure of the tonnage equation: force proportional to flow stress, to thickness squared, to bend length, and inversely to die opening. The empirical coefficient in every shop formula absorbs the parts the plastic-hinge model ignores: friction at the die shoulders, the wrap of the sheet around the punch tip, strain hardening beyond the yield point, and the fact that the real contact geometry is not a clean three-point beam.

The standard metric form, with F in kN, R_m in MPa, and t, L and V in mm:

For mild steel at 450 MPa and a 1 m bend length this collapses to the shop shorthand F \approx 65\,t^2/V tonnes, or roughly 8 tonnes per metre per millimetre of thickness when the die is 8× the thickness. Bystronic's catalogue uses a slightly different coefficient, C = 1 + 4t/V, which gives C = 1.50 at V = 8t and C = 1.33 at V = 12t; the 1.42 constant is C evaluated near V \approx 9.5t. In other words, the two "different" formulas are the same formula sampled at different die ratios, and the 1.42 version runs about 5–6% low at the 8× rule. Amada-Promecam's chart at R = 45 kgf/mm² uses 1.5 outright.

Air-bending force per metre of bend, 1 m bend length, die opening V = 8t:

Thickness · V die · Mild steel 450 MPa · 304 stainless 650 MPa · 6061-T6 310 MPa · S700 800 MPa

1.0 mm · 8 mm · 8.1 t · 11.8 t · 5.6 t · 14.5 t

1.5 mm · 12 mm · 12.2 t · 17.6 t · 8.4 t · 21.7 t

2.0 mm · 16 mm · 16.3 t · 23.5 t · 11.2 t · 29.0 t

3.0 mm · 24 mm · 24.4 t · 35.3 t · 16.8 t · 43.4 t

4.0 mm · 32 mm · 32.6 t · 47.1 t · 22.4 t · 57.9 t

6.0 mm · 48 mm · 48.9 t · 70.6 t · 33.7 t · 86.9 t

Three consequences follow directly from the exponents.

Thickness is quadratic. Doubling the thickness on the same die quadruples the force. A 100-tonne brake that bends 3 mm mild steel comfortably over 3 m (73 t at 24.4 t/m) cannot bend 6 mm over the same length at all (147 t), and it cannot bend 4 mm over 3 m either (98 t, which is nominally inside the rating but not at a full-length bend).

Die opening is inverse. Opening the die from 8t to 12t cuts the force by a third, which is exactly why heavy plate is bent over wide dies and why a fabricator reaching for a narrow die to get a tight radius pays for it in tonnage.

Material strength is linear. 304 stainless at 650 MPa needs 45% more force than mild steel at the same thickness. That single ratio drives most of the tooling damage in a mixed-material shop.

The margin the formula does not include

The formula gives the force for a 90° air bend of a given length. It does not account for:

The radius you get, not the radius you drew

In an air bend the inside radius is not set by the punch tip. It floats as a fraction of the die opening, because the sheet wraps the tip under a contact pressure high enough to deform the tip region plastically. The empirical fractions:

Material · Inside radius as a fraction of V · Source convention

Mild steel / cold-rolled · 0.15–0.17 × V · "20% rule" baseline, median 16%

Hot-rolled pickled and oiled · 0.14–0.16 × V · Lower yield, softer surface

304 / 316 stainless · 0.20–0.22 × V · Higher flow stress and work hardening

5xxx soft aluminium · 0.13–0.15 × V · Low modulus, low yield

Galvanised mild steel · 0.15–0.17 × V · Coating has negligible effect on radius

So a 3 mm mild steel part run over a 24 mm die comes out at an inside radius of about 3.8 mm, whether the drawing says 1.0 mm or 5.0 mm. This is the conversation that stalls more sheet metal quotes than any other, and it has a quantitative answer.

Suppose the design genuinely needs R_i = 1.0 mm on 3 mm sheet. Solving the radius rule for the die opening:

A 6.25 mm die is roughly 2t wide, far outside the 6–12t working range. The force at that opening:

against 24.4 t/m over a 24 mm die. A 3.84× tonnage penalty, a die that will mark the outside face, a punch tip that must be no larger than 1 mm radius, and a bend zone that may need bottoming to hold the radius at all. That is the honest cost of a sharp radius on thick sheet, and it is why the DFM answer is almost always: use the natural radius, or move to a thinner gauge, or accept a coining operation and a slower process.

The same arithmetic runs the other way. A 1 mm part in an 8 mm die floats to R \approx 1.3 mm; in a 12 mm die it floats to 1.9 mm. If the radius matters functionally (a fatigue-critical fillet, a mating surface, a coating bend test), specify it and let the fabricator pick the die. If it does not, write "R as formed" and save everyone a tooling change.

Minimum flange: the die sets the shortest leg you can hold

The blank must rest on both die shoulders with enough material for the punch to load it without the part tipping into the opening. Empirically the minimum flange is about 0.78 × V, which at the 8× rule lands near 6.2 × t:

V die · Minimum flange, 90° · Min flange for a 2 mm hem allowance

8 mm · 6.2 mm · ~10 mm

16 mm · 12.5 mm · ~16 mm

24 mm · 18.7 mm · ~23 mm

32 mm · 25.0 mm · ~30 mm

A 10 mm flange on 3 mm sheet in a 24 mm die is not a difficult bend, it is an impossible one: the part drops into the V. The fabricator's options are a narrower die (more tonnage, tighter radius), a special short-flange punch, or a different bend sequence that forms the short leg first while the part is still a long blank. All three cost money, and all three are avoidable at the design stage.

The flat pattern: where the 0.8 mm lives

The blank length is computed by unwrapping the neutral axis, the surface inside the material that neither stretches nor compresses. Its position is described by the K-factor:

K runs from about 0.33 at tight bends to 0.50 in pure bending, where the neutral axis sits at mid-thickness. Tight bends push it inward because the inner fibres compress and thicken while the outer fibres thin. Typical values in air bending:

Material · K, thin sheet · K, thicker sheet

Mild steel / cold-rolled · 0.33 · 0.38–0.42

304 / 316 stainless · 0.38 · 0.40–0.42

5052-H32 aluminium · 0.40 · 0.43

6061-T6 aluminium · 0.42 · 0.45

Galvanised steel · 0.40 · 0.42

With the neutral axis located, the bend allowance, which is the arc length through the bend:

and the outside setback, the distance from the bend tangent point to the theoretical sharp corner:

The bend deduction, which is what you subtract from the sum of the outside dimensions, is twice the setback minus the allowance:

For a 90° bend these simplify to BA = 1.5708(R_i + Kt) and OSSB = R_i + t.

A worked bracket, three K-factors

Take a 3 mm mild steel bracket, two 90° bends, outside legs of 50 mm and 30 mm, formed over a 24 mm die so R_i = 3.8 mm.

K-factor · Bend allowance · Bend deduction · Flat length

0.33 · 7.524 mm · 6.076 mm · 73.92 mm

0.42 · 7.948 mm · 5.652 mm · 74.35 mm

0.50 · 8.325 mm · 5.275 mm · 74.73 mm

The spread between the tight-bend value and the mid-thickness value is 0.80 mm per bend. On a four-bend part, that is 3.2 mm, or sixteen times the ±0.2 mm cut tolerance a fibre laser holds. The blank is not wrong because the laser missed; it is wrong because the model picked a K-factor that does not describe what the die does to that material at that radius.

The same effect at a thinner gauge: a 1.5 mm enclosure with four 90° bends over a 12 mm die moves 1.13 mm in flat length between K = 0.33 and K = 0.45, which is enough to put a pierced hole 1 mm out of position relative to the mating panel.

Why the CAD flat pattern and the shop's flat pattern disagree

Every CAD package ships a default. Some use K = 0.5 as a neutral placeholder, some use a bend table built for a specific tooling set, some default to a bend deduction table that was calibrated on 1.2 mm cold-rolled steel in 1998. The shop's brake has its own answer, and it is not a constant: the effective K depends on die opening, punch radius, material strength, coating and the bend angle.

Three practical consequences:

  1. Send formed dimensions, not flat patterns. A DXF of the flat is a claim about a process the designer cannot see. A STEP of the formed part plus "R as formed, ±0.5° per bend" lets the fabricator apply their own table.
  2. Calibrate with a strip test. Bend a 100 mm × 20 mm strip of the actual material lot at the actual die, measure the developed length, back-solve K from the bend allowance equation. Half an hour of shop time removes the largest error term in the whole chain.
  3. Never mix K-factor sources within one part. A bracket modelled with K = 0.5 for the first bend and a table-driven value for the second will be internally inconsistent before it is cut.

One further subtlety: for bends made parallel to the rolling direction, the material's ductility is lower and its springback higher, and the radius must grow by roughly 1.5× to avoid cracking. A flat pattern is not the only thing that changes when the nesting rotates the part 90°.

Springback: why 304 comes back at 87°

Release the load and the elastic part of the bend recovers. The bend zone is a stress gradient, not a uniformly yielded block: an elastic core survives in the middle of the thickness, and it is that core that springs the part open. The scaling is captured by a simple relation, derived from the plastic moment and the elastic unloading stiffness of a rectangular section:

The two ratios that matter are the geometric one, R_i/t, and the material one, flow stress over elastic modulus. Everything else, including the die, acts through those two. A gentle bend over a wide die has a large R_i/t and springs back much more than a tight bend; a high-strength steel has a large \sigma_f relative to a steel-like modulus and springs back more than mild steel at the same geometry.

Measured springback for 90° air bends without bottoming:

Material · Springback at R_i/t \le 1 · Springback at R_i/t = 2–5

Soft aluminium, soft copper · 0–1° · 1–2°

Low-carbon steel (cold-rolled) · 0.5–1.5° · 1–3°

304 austenitic stainless · 1.5–3° · 3–5°

6061-T6, 5xxx-H3x aluminium · 2–4° · 4–8°

HSLA steel · 2–4° · 4–7°

Dual-phase / AHSS · 3–6° · 6–12° or more

That is the 87° in the title: 304 stainless at R_i/t \approx 1 gives back 2–3°, so a 90° punch stroke produces an 87–88° part. Mild steel gives back 0.75–1°, which is why a shop that mostly runs cold-rolled steel can get away with a 0.5° fudge factor and then fails the first stainless job.

The springback factor quantifies the correction:

Program 93° to land 90° when springback is 3°. Note the side effect: the radius also grows. A 2.0 mm inside radius bent to land at 90° with S_f = 1.0345 finishes at 2.07 mm, so a springback correction that only fixes the angle still leaves the radius adrift.

Three ways shops handle it:

The practical tolerance to design to is ±0.5° per bend for a well-controlled air bend, ±1° for long bends where deflection dominates, and ±0.25° only with angle measurement and a stable material lot.

The 3 m problem: deflection, crowning and the canoe

A press brake is two beams pushed apart. Under load the ram bows upward and the bed bows downward, so the punch does not penetrate as deeply at mid-span as it does near the uprights. On a 3 m machine the elastic difference is on the order of 0.15 mm at the centre. The part comes out tight at both ends and open in the middle, the shape every operator calls a canoe.

The sensitivity is brutal because the process is depth-controlled:

Compensation comes in three forms. Pre-crowned beds are machined with a fixed curve, which is only correct at one load. Mechanical crowning uses a row of wedges under the die to create an adjustable opposite curve. Hydraulic crowning puts cylinders in the lower beam and is the most accurate, with automatic systems holding angle variation along the bend line to about ±0.5°. The rule of thumb is that crowning matters for bends longer than roughly 1–1.5 m; below that, deflection is usually inside the angle tolerance.

Two related failure modes are routinely misdiagnosed as crowning:

The realistic tolerance stack for a bent part: backgauge repeatability ±0.05 mm, flange length ±0.2 mm, angle ±0.5° short bends and ±0.7–1.5° long bends, hole-to-bend position ±0.3 mm because two process errors combine. Calling ±0.1 mm on a flange length is asking the brake to be a machining centre, and the quote will reflect the sorting and rework it takes to pretend.

Material behaviour that changes the numbers

Mild steel (S235 / A36, 400–470 MPa). The baseline. K ≈ 0.33–0.42, springback 0.5–1.5°, radius 0.16V. Forgiving, cheap, and the material every rule of thumb was calibrated on.

Galvanised steel (Z275, DX51D). The coating is 275 g/m² total, about 19 µm of zinc per side at 7.14 g/cm³. It does not change the bend force materially (the base steel is often 400 MPa rather than 450), but it changes three other things: the coating cracks in tension at tight radii, the low-friction surface lets the sheet slide in the die and shifts the bend line, and any subsequent welding of the bend zone risks liquid metal embrittlement because zinc melts at 419 °C and penetrates the steel grain boundaries under tensile stress. K runs around 0.40. Keep the inside radius at 1.0–1.5t minimum and never specify a coined radius on galvanised sheet.

304 / 316 stainless (520–720 MPa). Two effects compound. The higher flow stress raises the tonnage by about 45% at the same thickness, and austenitic stainless work-hardens steeply during the bend, so the outer fibres reach much higher flow stress than the mill certificate's yield suggests. Springback at R_i/t \approx 1 is 1.5–3°, rising to 3–5° at R_i/t = 2–5. The radius also floats higher, 0.20–0.22V, so the same die produces a larger radius than it would in mild steel. Stainless galls against tool steel; a polished punch and a lubricant are not optional on visible parts.

6061-T6 aluminium. Modulus 69 GPa, roughly a third of steel, so springback is 2–4× worse at the same geometry (2–4° at R_i/t \le 1, 4–8° above). Minimum bend radius is 3–5t and the material cracks rather than yields if pushed tighter; the crack runs along the bend and is often only visible after anodising. 5052-H32 is the bending grade, at 1–2t minimum radius.

HSLA and dual-phase steels. Yield strengths of 550–1,000 MPa with a steel modulus mean large elastic cores and springback of 6–12° at moderate radii. These grades are where angle measurement stops being a luxury: overbending a fixed 4° works until the coil changes and the lot-to-lot yield spread moves the angle by more than a degree.

Grain direction. Bending across the rolling direction is the default because ductility is highest there. Bending parallel to it requires roughly 1.5× the radius to avoid edge cracking and adds 1–1.5° of springback. A part that is fine in one nesting orientation can crack in another, which is why nesting software that ignores grain direction produces intermittent scrap.

The DFM checklist, with the numbers attached

  1. Pick one thickness and one die per part where possible. Every die change is a setup; every setup is 20–40 minutes of a ₹1,000/h machine. A part that needs a 6t die for one flange and an 8t die for the rest pays twice.
  2. Specify the natural radius. R_i \approx 0.16V for mild steel, 0.21V for stainless. If the drawing needs a different radius, say so explicitly and expect a tooling charge.
  3. Keep flanges at or above 0.78V, which is about 6t at the 8× rule. Short flanges are the most common reason a part cannot be made as drawn.
  4. Keep holes at least 2.5t + R_i from the bend line. Closer than that and the hole becomes an oval, because the bend zone stretches the material around it.
  5. Add bend reliefs where two bends meet. Relief width at least t, depth at least R_i + t. Without them the corner tears or puckers.
  6. Leave at least 3t between adjacent bend lines. Closer and the second bend re-forms the first one's bend zone.
  7. Tolerance what the process can hold. ±0.5° per bend, ±0.2 mm flange, ±0.3 mm hole-to-bend. Tighter means 100% inspection.
  8. Avoid bends within one material thickness of a laser-cut edge on high-strength or hard-temper material; the heat-affected zone is the crack initiation site.
  9. Model with the shop's K-factor, or send formed geometry. Do not mix a CAD default with a shop table.
  10. For 6061-T6, specify 3–5t minimum radius and bend across the grain. If the design cannot afford that radius, the material is wrong, not the process.

The cost arithmetic behind a bend

A press brake's economics are dominated by setup, not by cycle time, and that shape decides which parts are cheap.

Assume a 100 t × 3 m CNC brake at ₹1,000 per machine hour, a 25-minute setup (tooling change, program recall, first-article check), and 9 seconds per bend including handling and repositioning:

Bends per part · Setup amortised · Run time · Cost per bend

4 · ₹417 · ₹10 · ₹107

20 · ₹417 · ₹50 · ₹23

200 · ₹417 · ₹500 · ₹4.6

The same bend costs 23 times more on a four-bend part than on a two-hundred-bend part. This is why sheet metal quotes are so sensitive to batch size and why a prototype bracket that looks trivial on a drawing can quote at several hundred rupees: the machine spends most of its time being set up, not bending.

Now put the flat-pattern error back into the same frame. A 300 × 200 × 3 mm mild steel blank weighs 1.41 kg (7850 kg/m³); at ₹60/kg the material is about ₹85, and laser cutting adds roughly ₹30. Call it ₹115 per blank. A K-factor error of 0.8 mm per bend produces flanges 0.8 mm short on a ±0.5 mm drawing, so the first batch of 100 blanks becomes ₹11,500 of scrap plus the laser time and the lead time. The fix costs half an hour of strip testing.

The cost model also explains two shop behaviours that frustrate designers. Shops quote the die they have, not the die the drawing implies, because a die change is a setup. And they quote a wider tolerance than the drawing asks for when the drawing asks for less than the process can hold, because the alternative is to price in inspection and rework.

What to send a fabricator

The most useful package for a bent sheet metal part is smaller than most designers expect:

Everything else, including the die, the K-factor and the bend sequence, belongs to the shop, and a shop that is allowed to own those decisions will hit the tolerance more often than one that is handed a flat pattern and told to match it.

If you have a sheet metal part in STEP or DXF and want quotes from fabricators who will tell you which of these rules your design breaks, upload it to FabFlow and compare quotes with the bending assumptions stated up front. A quote that names its die opening and its K-factor is a quote you can hold someone to.

More FabFlow blog posts