Workshop Reference Chart

Bend Allowance Chart for Sheet Metal

Practical bend allowance and bend deduction values for mild steel, stainless steel and aluminium, organised by thickness, inside radius and included bend angle.

A bend allowance chart turns the geometry of a folded part into a developed length that can be marked, cut and programmed. The tables below cover common workshop combinations in metric and imperial units. Each row states material, thickness, inside bend radius and the K-factor used; the angle columns give both bend allowance (BA) and bend deduction (BD). They are reference values, rounded to three decimal places, rather than a promise that every press brake will produce exactly the same result.

Material temper, tensile strength, rolling direction, punch radius, die opening, bending method and springback all influence the neutral axis. Use these figures for estimating and first-off development, then verify critical or repeated parts with a measured test bend. Once a shop has calibrated values for its regular tooling and material batches, those local values should take priority.

Metric bend allowance and deduction chart

The metric table uses representative K-factors of 0.33 for mild steel, 0.40 for stainless steel and 0.38 for aluminium. Radius is the finished inside radius. A cell such as “2.089 / 1.911” means BA 2.089 mm and BD 1.911 mm.

Imperial bend allowance and deduction chart

The same method works in inches. Common sheet gauges vary by alloy and standard, so thickness is stated directly rather than as a gauge number. All BA and BD results below are inches.

The bend allowance formula

Bend allowance is the length of the neutral axis through the curved bend zone. The neutral axis lies between the compressed inside face and stretched outside face. Its location is expressed by K-factor, measured from the inside face as a fraction of thickness.

Here A is included bend angle in degrees, R is inside bend radius, K is K-factor, and T is material thickness. Radius and thickness must use the same unit. The formula then returns BA in that unit. For a 90° bend, π/180 × 90 simplifies to π/2.

Angle terminology can cause expensive errors. This chart treats 90° as a quarter-circle bend and 30° as thirty degrees of material rotation. Some drawings label the remaining internal angle instead. Confirm whether the drawing angle is the bend rotation or the final included opening before choosing a column.

Relationship between bend allowance and bend deduction

Bend allowance and bend deduction describe the same formed corner from different dimensional systems. BA is added when the straight flange dimensions stop at the bend tangency points. BD is subtracted when the drawing gives outside mould-line flange dimensions. Neither number is universally interchangeable without knowing how the flanges were measured.

OSSB is outside setback. For a 90° bend it equals R + T because tan(45°) is one. Bend deduction contains two setbacks because the theoretical sharp corner extends beyond each tangency point. Subtracting the neutral-axis arc length leaves the total amount removed from the two outside dimensions.

Fully worked metric example

Consider a mild-steel right-angle bracket with two outside legs of 50 mm and 40 mm. The sheet is 2 mm thick, the finished inside radius is 2 mm, and the selected K-factor is 0.33. First calculate neutral-axis radius: R + K × T = 2 + 0.33 × 2 = 2.66 mm. The 90° angle multiplier is π/2, or 1.5708.

The bend line, when the deduction is split symmetrically, lies half the deduction back from the first outside mould line: 50 − 3.822/2 = 48.089 mm from the first blank edge. In real production, bend-line location can also be defined from a backgauge datum or tangency point, so document the chosen convention.

How material and tooling change the chart value

Mild steel

Low-carbon mild steel is usually forgiving and repeatable, but published K-factors still vary with air bending, bottoming and coining. In an air bend, the die opening strongly influences the naturally formed inside radius. Do not automatically substitute the punch nose radius for the measured finished radius.

Stainless steel

Stainless typically needs more force and exhibits more springback. A larger die opening or radius is commonly used to reduce cracking and tonnage. The 0.40 reference K-factor reflects a neutral axis farther from the inside surface, but hard grades and tight tooling should be tested.

Aluminium

Aluminium alloy and temper matter greatly. Soft 1050 or 3003 behaves differently from heat-treated 6061-T6, particularly across the grain. Minimum safe radius may govern the setup before flat-pattern accuracy does. A visible crack means changing the design or process, not merely adjusting BA.

Using the chart on multi-bend parts

Calculate each bend independently. A channel with two 90° bends has two allowances or deductions even if both look identical. If radius, angle or tooling changes, use the appropriate row for each bend. Add all straight tangency-to-tangency lengths and all BAs, or sum the outside flange dimensions and subtract all BDs. Mixing the two systems midway is a common source of double-counting.

Round only the final blank dimension where possible. Rounding every allowance to a coarse fraction can accumulate noticeable error on an enclosure with many bends. Keep at least three decimal places in inches or two to three in millimetres, then apply the shop's cutting tolerance at the end.

Frequently asked questions