Sheet Metal Bending: Methods, Tolerances and Design Rules

Sheet metal bending turns a flat blank into a three-dimensional part, and nearly every dimension on that part traces back to the inside bend radius. This guide covers press brake methods, bend allowance and K-factor with a worked example, flange and hole rules, relief, springback, crowning, tooling, hemming, roll and tube bending, material data, tolerance and radius tables, ten design rules, and drawing callouts.

What Bending Does to the Material

A bend stretches the outer fibers, compresses the inner fibers, and leaves one layer at its original length. That layer is the neutral axis, and its position as a fraction of thickness is the K-factor that sets how much flat stock the bend consumes.

Bend strain at the outside surface follows 1 / (2R/t + 1): 20% at R = 2t, 33% at R = t, 50% at R = 0.5t. Mild steel at 25 to 30% elongation survives R = t; 6061-T6 at 10 to 12% does not survive 33% and cracks.

The bend also thins the section 5 to 15% and work hardens it. Convert any gauge callout with the sheet metal gauge chart before calculating: 16 gauge steel and 16 gauge aluminum differ by 15% in thickness.

Air Bending, Bottoming and Coining

Air bending presses the sheet into a V-die without touching the walls, so ram depth sets the angle and die opening sets the radius. Bottoming stamps the punch radius into the part against the die walls. Coining flows metal at five to ten times the tonnage and nearly removes springback.

Air bending is what most shops quote, but the radius is not yours to choose: V = 8t gives R ≈ 1.3t, V ≈ 6t gives R ≈ t, V ≈ 12t gives R ≈ 2t. A 1 mm radius on 2 mm stock via an 8t die comes back at 2.6 mm.

Coining only pays off in high-volume stamping, so what you buy on a CNC press brake is air bending with the control compensating for springback.

Inside Radius and the K-Factor

The K-factor is the distance from the inside surface to the neutral axis divided by thickness, and 0.42 is a workable default for air bending near R/t = 1 in mild steel.

Typical values are 0.33 at R/t = 0.5, 0.42 at 1.0, 0.45 at 2.0, 0.47 at 3.0 and 0.50 above 5.0. K moves with die opening, friction and yield strength, so two shops running the same alloy can land 0.3 mm apart on flat length.

Bend Allowance, Bend Deduction and a Worked Example

Bend allowance is the neutral axis arc length through the bend; bend deduction is what you subtract from the sum of outside dimensions to get the blank. Both describe one geometry, and mixing them is the most common flat-pattern error.

• Bend allowance: BA = θ (R + K t), with θ in radians
• Outside setback: OSSB = (R + t) tan(θ / 2)
• Bend deduction: BD = 2 (OSSB) − BA
• Flat length = sum of outside dimensions − sum of deductions

Worked example. 2.0 mm mild steel, 90° bend, 2.0 mm inside radius, outside flanges 50 mm and 30 mm, K = 0.42.

1. Angle in radians: 1.5708.
2. Neutral radius: 2.0 + (0.42 × 2.0) = 2.84 mm.
3. BA = 1.5708 × 2.84 = 4.46 mm.
4. OSSB = (2.0 + 2.0) × tan 45° = 4.00 mm.
5. BD = 8.00 − 4.46 = 3.54 mm.
6. Flat length = 50 + 30 − 3.54 = 76.46 mm.

Cut at 76.46 mm and both flanges finish on size. Cut at 80 mm and each flange ends 1.8 mm long; over four bends the error reaches 7 mm.

Values are 90° bends with R = t and K = 0.42; the deduction triples from 2 mm to 4 mm. Shifting K to 0.33 moves this blank 0.28 mm, enough for a formed part to match its bend table yet sit 0.3 mm off the CAD flat.

Bending Force and Tonnage

Air-bend tonnage follows one formula: 1.42 times tensile strength in MPa, times thickness squared, times bend length, divided by 1000 times the V opening. Mild steel at 450 MPa needs about 8 tonnes per meter per millimeter of thickness.

F (kN) = 1.42 × σ_b × t² × L / (1000 × V)

Tonnage scales with length and thickness squared: 4 m in 3 mm needs 96 tonnes, 6 m in 6 mm close to 300. Use 1.5× for 304 stainless and 0.6× for aluminum, and add a third of the force when you go from an 8t to a 6t die.

Minimum Flange Length and Hole-to-Bend Distance

Keep every flange at least 4t + R long and every hole edge at least 2.5t + R from the bend line. Below those limits the flange pulls into the die opening and the hole stops being round.

The die-based flange limit is V/2 + t + R, or 5t + R on an 8t die, so design to the larger number: 2 mm steel at a 2 mm radius needs a 12 mm flange on an 8t die and about 10 mm on a 6t die.

Hole distortion is material flow. A 6 mm hole 3 mm from the bend line in 2 mm steel finishes 6.3 by 5.6 mm, outside tolerance on a clearance hole. Move it, pierce after forming, or slot it parallel to the bend line.

Bend Relief

Bend relief is a notch at the end of a flange where it meets a wall, and it stops the tear that starts at that inside corner. Make it at least t wide and R + t deep, so 2 mm by 4 mm on 2 mm steel at a 2 mm radius.

Without relief the flange and the wall fight for the same material and the corner stretches or tears.

Springback and How to Compensate

Springback is the elastic recovery that opens a bend after the punch lifts, which is why a commanded 90° lands at 92°. It runs under 1° in annealed mild steel and 5° or more in 304 stainless and 6061-T6.

Typical values: mild steel 0.5 to 2°, galvanized 1 to 2°, 304 stainless 2 to 5°, 5052 aluminum 2 to 4°, 6061-T6 3 to 6°.

Compensation belongs in the control: a CNC brake overbends by the calculated amount, and angle-measurement systems correct to ±0.5° across a batch. Do not add two degrees to the drawing, because a 92° callout for a 90° part produces 94°.

Crowning and Long Bends

Crowning compensates for ram and bed deflection, which otherwise leaves the middle of a long bend shallower than its ends. A table bows a few tenths of a millimeter over 4 m at full load, which shows up as 1 to 2° across the part.

Manual shims are setup-specific, wedge crowning curves the bed, and hydraulic or CNC crowning holds ±0.5° on a 4 m bend. On any panel over 2 m, ask whether the shop has active crowning.

Press Brake Tooling

Punch and die choice fixes the inside radius, the minimum flange and the tonnage. Standard punches are rated near 1000 kN per meter, and a narrow tip on thick stock can exceed that before the machine does.

The V opening matters most: at least 6t for air bending, 8t as the usual default, giving R ≈ 0.16V. Narrower raises tonnage and can mark the inside of the bend.

Hemming

Hemming folds the edge back on itself to remove the sharp edge and hide the burr. A flat hem folds flush and leaves an edge about two thicknesses deep, a teardrop hem leaves an open loop, and a rope hem wraps a wire inside.

A flat hem needs a flange of at least 6t and two steps: a pre-bend to about 30° on a sharp punch, then a flattening pass in a hemming die. One-hit closing tears the outside.

Hem allowance runs 1.5t to 2t for a flat hem and 2t + R for a teardrop, and the edge must be deburred first or the burr starts a crack.

Roll Bending and Folding

Roll bending passes sheet between rolls to make cylinders, arcs and tank sections rather than sharp corners. Three-roll machines are the default; four-roll machines add a pre-bend that shrinks the flat left at each end.

A 3-roll machine forms from about 1.5 times its top roll diameter upward, and thickness capacity falls as radius tightens: 6 mm at a 1000 mm radius may become 3 mm at 200 mm.

Folding clamps the sheet and rotates a beam, giving a sharp 0.5t to 1t radius with no die marks for visible enclosures. It runs out around 4 mm in mild steel, with a 10 to 20 mm minimum flange set by the clamping beam.

Tube Bending

Tube bending uses rotary draw bending, where a mandrel supports the inside while a wiper die and pressure die control the outside. Without a mandrel the minimum centerline radius is 2 to 2.5 times OD; with a mandrel and tight tooling, 1 to 1.5 times OD.

Wall thinning runs 10 to 15% at CLR = 2 OD and up to 25% at 1 OD, so a 2 mm wall finishes near 1.6 mm. Ovality is specified at 5% or less; wrinkles on the inside mean the mandrel sits too far back.

Cut holes before bending: tube laser cutting handles the straight length, while cutting after bending needs a fixture to locate a hole on a curve.

Mild Steel, Stainless and Aluminum Compared

Mild steel bends predictably. Stainless work hardens, needs about 50% more tonnage and springs back two to five degrees. Aluminum marks on the dies, springs back more than steel, and splits at a tight radius in hard tempers.

Stainless work hardens so the outside ends stronger than the core, and it galls on uncoated tooling, which picks up material and marks the part. Use protective film, a generous punch radius and a bend across the grain.

Aluminum splits before it yields visibly: 5052-H32 forms to about 1.5t, while 6061-T6 needs 3t to 4t and still cracks along the rolling direction. A tight radius in T6 means specifying T4 and aging after forming, or moving to 5052.

Galvanized G90 cracks its zinc below about 1t.

Minimum Inside Radius by Material

Minimum inside radius is the radius below which the outside surface cracks, quoted as a multiple of thickness for 90° bends at room temperature.

Grain direction decides the tight cases. Bending parallel to the rolling direction concentrates strain along inclusions, so for any radius near the minimum, place the bend line perpendicular to the rolling direction.

Bending Tolerance by Part Length

Bending tolerance widens with length because die deflection, crowning, thickness variation and thermal drift accumulate along the bend. A typical shop holds ±0.2 mm at 500 mm and ±1.5 mm at 6 m, with angles near ±1°.

Add about ±0.1 mm per additional bend when dimensions chain bend to bend, and dimension from a common datum instead. Mill tolerance on 2 mm cold-rolled is commonly ±0.08 to ±0.10 mm, worth 0.05 mm of deduction per bend.

Ten Design Rules for Bent Sheet Metal Parts

Standardize the radius, keep flanges and holes clear of the bend zone, and dimension in a way the shop can reproduce. The ten rules below are the specific numbers behind those habits.

1. Use one inside radius on the whole part, defaulting to R = t: one die set and one K-factor.
2. Keep every flange at least 4t + R, and 5t + R on an 8t die, or the flange pulls into the die opening.
3. Keep the near edge of every hole at least 2.5t + R from the bend line, and slot it if it must sit closer.
4. Add bend relief at the end of every flange meeting a wall: at least t wide and R + t deep.
5. Size the radius to the die you expect, R ≈ 0.16V: an 8t die on 2 mm stock gives 2.6 mm.
6. Keep bend lines at least 3t from any cutout, weld seam or hole pattern edge, or the feature distorts.
7. Stay at or above 90° included where possible; angles under 60° need acute tooling and raise tonnage.
8. Dimension to the outside mold line with a stated deduction, or inside with a stated allowance, and never mix conventions.
9. Orient tight-radius bends perpendicular to the rolling direction and note the grain requirement on the drawing.
10. Keep the blank inside the brake’s bend length and tonnage: a 6 m panel at 6 mm thick is a 300 tonne bend.

Rule 1 carries the most weight: three inside radii mean three tooling setups and three K-factors, and the cost lands in the quote.

Common Bending Defects and Their Causes

Most defects trace to one of four causes: a radius below the material minimum, a feature inside the deformation zone, a tooling or tonnage mismatch, or a flat pattern built on the wrong K-factor.

Diagnosis is mostly measuring the actual inside radius rather than trusting the nominal one. A part designed for R = 2 mm that leaves the brake at 2.6 mm because the die was 16 mm is short on every flange by about 0.3 mm.

How to Dimension Bends on a Drawing

A bend needs four things on a drawing: finished angle, inside radius, bend direction, and the dimension convention. Missing any one and the shop picks the value, and the flat pattern follows.

Pick one convention. Outside dimensions with a stated deduction match how parts are measured after forming; inside dimensions with an allowance suit enclosure work. Either works, mixing them on one drawing does not.

Use a bend table. List, for each bend number, the angle, radius, direction (up or down) and the deduction used. Show bend centerlines as phantom lines and label them.

Dimension to a real feature. Dimension to the outside mold line or a tangent point, never to the theoretical sharp corner, which is ambiguous about which convention applies.

State who owns the flat pattern. If the fabricator does, give formed dimensions plus the bend table; if you do, give the K-factor so the shop can check rather than guess. That one line prevents the most expensive argument in sheet metal.

Call out tolerance once. A note such as “formed dimensions ±0.5 mm, angles ±1° unless noted” covers most parts. If the part is welded into an assembly, the weld callouts follow AWS A2.4 conventions covered in the welding symbols guide.

FAQ: Sheet Metal Bending Questions

What is the difference between bend allowance and bend deduction?

Bend allowance is the neutral axis arc length through the bend. Bend deduction is what you subtract from the sum of outside dimensions to get the blank. For a 90° bend in 2 mm steel at a 2 mm radius: allowance 4.46 mm, deduction 3.54 mm.

What K-factor should I use for a 90° bend?

Use 0.42 for mild steel when the inside radius is close to the thickness, which covers most air bending. Move toward 0.33 below R = t and 0.50 above 3t, and confirm on a test strip for stainless or aluminum.

What is the minimum flange length for press brake bending?

The general rule is 4t + R. The die-based limit is V/2 + t + R, or 5t + R on an 8t die: for 2 mm steel at a 2 mm radius, 12 mm on an 8t die and about 10 mm on a 6t die.

How far should a hole be from a bend line?

Keep the near edge of the hole at least 2.5t + R from the bend line, which on 2 mm steel at a 2 mm radius is 7 mm. Below 1.5t the hole distorts enough to fail a gauge check; move it, pierce after forming, or slot it.

Why does my part come out short after bending?

Almost always because the flat pattern neglected bend deduction or used the wrong K-factor. Measure the actual radius: if the die produced 2.6 mm instead of the assumed 2.0 mm, every flange is short by about 0.3 mm and the flat pattern needs recomputing.

Getting the Bend Right on the First Pass

Send formed dimensions, a bend table and thickness in millimeters, and a fabricator can hold the tolerances above without a trial loop. YC Prime Precision runs CNC press brakes to 6 m and ±0.1 mm on short flanges, fed by fiber laser cutting to 20 mm, with sheet metal orders shipping in 5 to 12 business days.

For a bracket or enclosure, the sheet metal fabrication overview covers cutting, forming, welding and finishing as one sequence. For bent parts, put the material, thickness, quantity and bend table into your instant quote request and the price comes back without a clarification round. After forming, powder coating adds 60 to 100 microns per face and tightens hole fits, so plan the finish before you release the flat pattern.