Which K-factor should I start with?

Start inside the verified default band of 0.40 to 0.45, which covers most sheet metals: 0.42 for cold-rolled carbon steel, 0.43 for 5052-H32 aluminum, 0.45 for stainless, and 0.40 for annealed aluminum at standard radii. Drop to the sharp-radius value, 0.33 for soft aluminum and 0.38 for steel, when the inside radius is below one thickness.

How do I recompute a bend allowance row?

Bend allowance equals pi divided by 180, times the bend angle from flat, times (inside radius + K times thickness). Row one of the table: 1.5708 times (1.5 + 0.63) = 3.35mm for 1.5mm cold-rolled steel at 90 degrees with a 1.5mm inside radius and K of 0.42. Every row lists thickness, radius, K, and the angle so the arithmetic checks.

Why does the bend deduction here differ from other charts?

This table computes bend deduction with the in-house reference form, K times t times (180 minus the included angle) times 0.01745. The geometric form, 2(R + t) times tan(A/2) minus BA, adds the outside setback and returns larger deductions. The bending guide covers that derivation and when shops use each form.

Does thickness alone change the K-factor?

No. K tracks material hardness and the ratio of inside radius to thickness. The thickness columns reflect the forming regime typical at each gauge: radii below one thickness are common at 1mm and below, and radii of 1 to 3 times thickness dominate from 1mm to 6mm on standard dies.

What K-factor applies above a 3 times thickness radius?

0.50, for every material in the standard air-bend chart. Generous radii on heavy plate are the usual case, and the value is the same whether the sheet is aluminum, steel, or stainless.

Do these values apply to bottoming or coining?

No, the table is for air bending. The standard chart puts bottoming higher, 0.42 to 0.48 depending on radius class and hardness, with coining between it and air bending. The bending guide explains the three forming methods.

How do I verify the value for my material batch?

Cut a test blank of known length, bend it on the production tooling, measure the resulting flanges, and back-calculate the factor the machine and material actually produced. Treat a blank computed from table values as a first-article starting point, because temper, batch, and tooling wear all shift the real K-factor.

Sheet Metal Bend Allowance Table

K-factor by material and thickness class plus computed bend allowance and bend deduction rows with every input shown, on the 0.40 to 0.45 default band.

Most common sheet metals bend with a K-factor between 0.40 and 0.45, a default band verified against in-house fabricator data (PC-070). This page is the data companion to the sheet metal bending guide: a K-factor lookup table by material and thickness class, plus bend allowance (BA) and bend deduction (BD) rows computed from the standard formulas with every input shown, so any result can be recomputed from the row itself. The bending guide carries the concepts: what the K-factor is, how BA and BD relate, springback, and the full flat-pattern method.

For calculation, bend allowance uses BA = π/180 × A × (R + K × t), and bend deduction uses the reference form BD = K × t × (180° − included angle) × 0.01745, where A is the bend angle measured from flat, R the inside radius, and t the thickness. Both derivations, and the geometric BD form that adds the outside setback, are on the bending guide.

How to use the K-factor table

The columns are radius regimes, not thickness limits

Two variables move the K-factor: material hardness and the ratio of inside radius to thickness. Thickness alone does not. The public air-bend chart behind this table (sheetmetal.me) groups values by radius class: sharp bends at R below one thickness, standard bends at R = 1 to 3 times thickness, generous bends above 3 times thickness. The thickness columns stand in for the regime each gauge usually sees: thin sheet at 1mm and below is where sub-thickness radii get formed (the in-house minimum-radius rule of 0.5 × t, PC-067, makes them feasible), while mid and thick gauges run at R = 1 to 3 × t on standard dies, where, as Durma Press notes, the inside radius forms as a fraction of the V-die opening, their chart pairing common air-bend radii at roughly 1.1 to 1.25 times thickness.

Choosing K when the temper is unknown

Start inside the verified default band that covers most materials (PC-070), then correct for radius class: a radius sharper than one thickness drops soft aluminum to 0.33 and steel to 0.38, and a radius above three times thickness raises any material to 0.50. The shop’s own value, measured from a test bend on the production tooling, overrides any number in this table.

Bend allowance and bend deduction worked rows

Each row below is arithmetic from the inputs shown: thickness t, inside radius R, K from the table below, and the bend angle A measured from flat, so a square corner is A = 90° and a shallow 45° flange is A = 45°. The BD form takes 180° minus the included angle, which is the same number. All rows use R = t, a common specified radius that sits comfortably above the 0.5 × t minimum. BA and BD values are rounded to 0.01mm.

Material	t (mm)	R (mm)	K	A from flat	BA (mm)	BD (mm)
Cold-rolled steel	1.5	1.5	0.42	90°	3.35	0.99
Mild steel	2.0	2.0	0.42	90°	4.46	1.32
Carbon steel	4.0	4.0	0.42	90°	8.92	2.64
5052-H32 aluminum	1.0	1.0	0.43	90°	2.25	0.68
Annealed aluminum	1.5	1.5	0.40	90°	3.30	0.94
304 stainless	3.0	3.0	0.45	90°	6.83	2.12
Cold-rolled steel, shallow bend	2.0	2.0	0.42	45°	2.23	0.66

Reading a row end to end

Take row one. K × t = 0.42 × 1.5 = 0.63, so R + K × t = 1.5 + 0.63 = 2.13. Then π/180 × 90 = 1.5708, and BA = 1.5708 × 2.13 = 3.35mm. Bend deduction: 0.42 × 1.5 × 90 × 0.01745 = 0.99mm. The same two-step arithmetic reproduces every other row, including the 45° row, where the factor is 0.7854 instead of 1.5708.

Applying a row to the flat blank

For a bracket with two 50mm outside flanges bent to the row-one conditions, the flat blank is 50 + 50 − 0.99 = 99.0mm before cutting. How deductions accumulate across the multiple bends of an enclosure is covered on the bending guide.

Material notes and selection

Soft and annealed aluminum

Annealed aluminum carries the lowest values in the table, 0.33 at sharp radii and 0.40 at standard radii, because it is the softest common sheet metal. Enclosure work in annealed tempers should specify K = 0.40 unless the drawing radius drops below one thickness, where 0.33 applies.

Half-hard aluminum and 5052-H32

5052-H32 is the workhorse enclosure alloy, and Durma’s chart carries a single K of 0.43 for it, matching the public chart’s medium-hardness class at standard radii. Two independent references landing on the same number is why this row is printed as a single value rather than a range.

Carbon steel and stainless

Cold-rolled steel holds 0.42 from 18 ga through 12 ga, about 1.2 to 2.7mm, in Durma’s per-gauge chart, so the mid and thick columns share one value. Austenitic stainless runs the highest of the three, 0.40 sharp and 0.45 standard, which means stainless consumes more bend allowance per millimetre of thickness at the same radius.

The 0.50 cap at generous radii

Above R = 3 × t, every material in the standard chart goes to 0.50, which is where heavy plate bent on wide dies lands. If the drawing calls a radius above three times thickness, use 0.50 regardless of the material row.

Accuracy, tolerances, and verification

What table values are good for

These numbers get a first-article blank close, not final. Material batch, temper drift, and tooling wear all shift the real K-factor, which is why PC-070’s band is documented as a default that is calculated per material. The standard practice is a test bend: cut a known flat length, bend it on the production tooling, measure the finished flanges, and use the difference to back out the factor that setup actually produced.

The angle tolerance that rides along

A bend carries an angle tolerance as well as a length dimension, and the angle band is material-specific (verified in-house): soft aluminum about ±1.0° standard and ±0.5° best, carbon steel ±1.0° to ±2.0° standard and ±0.3° to ±0.5° best, stainless ±1.0° to ±1.5° standard (PC-060, PC-060b, PC-060c, PC-061). A blank computed to two decimals can still yield a part at the loose end of its angle band, so tolerance the bend on the drawing rather than rely on blank precision alone.

Limitations

The table covers air bending of common sheet gauges from 1mm and below up to 6mm. It does not cover bottoming or coining, which run different K classes, radius regimes above 3 × t beyond the 0.50 cap, or less common alloys. Values are starting points assembled from public press-brake references plus one in-house verified band, and a shop’s measured value always outranks them. Confirm against the bending guide’s tolerance data and a test bend before committing a production blank.