K-factor in sheet metal bending: values and how to measure it

The K-factor in sheet metal bending is the position of the neutral axis as a fraction of the sheet thickness, measured from the inside surface of the bend. On 2 mm CRCA at an inside radius of 2 mm it is typically 0.42, which gives a 90° bend allowance of 4.46 mm; assume the common default of 0.50 and the same bend becomes 4.71 mm.

A quarter of a millimetre does not sound like much until it is multiplied by four bends and sits against a ±0.5 mm assembly tolerance. K is the one number in the flat pattern that most designers never measure and most CAD systems fill in with a default.

What follows is what K is geometrically, the values that apply across the radius range, a coupon procedure that produces your own K in about ten minutes of shop time, and the cases where no single K works.

What the K-factor measures

When a sheet bends, the outer fibres stretch and the inner fibres compress. Somewhere between them a layer stays at its original length. That layer is the neutral axis, and K is its distance from the inside surface divided by the thickness.

For a thin elastic beam the neutral axis is at mid-thickness, K = 0.50. Bending sheet metal is not elastic: the neutral axis shifts toward the inside radius as the bend gets tighter relative to thickness, because the plastic zone grows and the strain distribution becomes asymmetric. That is why K falls to about 0.33 at R/t 0.5.

Geometrically, K sets the arc radius that the bend allowance is measured along: BA = (π/180) × θ × (R + K × t). Nothing else in the formula is uncertain once the tool is chosen. R comes from the die opening, t from the coil, θ from the drawing, and K is the term that carries all the assumptions.

K-factor in sheet metal bending by radius-to-thickness ratio

Values are for 90° air bends on cold-rolled mild steel. The allowance and deduction columns are calculated on 2 mm sheet at the radius shown, so the effect of K alone is visible.

The table is a starting point, not a lookup. The R/t ratio is only known after the die is chosen, and the die is often chosen to suit an existing tool rather than the drawing.

Why K is not a property of the material alone

Four inputs move K, and only one of them is the metal.

• Tooling. Air bending, bottoming and coining put the material under different stress states. Coining forces the material into the punch radius and shifts the neutral axis further, so a coined bend needs its own K.
• Radius-to-thickness ratio. This is the dominant term. A 2 mm part bent at R2 and the same part bent at R10 are two different K values on the same drawing.
• Strain hardening. A material with a high n value spreads strain further through the section, which moves the neutral axis. Stainless and high-strength low-alloy grades behave differently from plain CRCA.
• Die opening. Because the die sets the natural radius, changing from an 18 mm to a 50 mm V die on 3 mm sheet can move the inside radius from about 3 mm to 8 mm, and K from 0.44 to roughly 0.47 with it.

The practical consequence: a K-factor is only meaningful as a triple of material, thickness and die. Storing one number per part, or one number for the whole shop, guarantees a flat pattern that is right for one job and wrong for the next.

Measuring K from a bend coupon

This procedure takes one coupon, one bend and a pair of callipers.

1. Cut a coupon of known thickness, 200 mm × 80 mm, from the production coil. Measure the thickness with a micrometer in three places and use the average.
2. Measure the coupon length to 0.05 mm and record it as the flat length.
3. Bend it 90° in the production die, at a position near the middle.
4. Let it cool, then measure the inside radius with radius gauges or on a profile projector. Measure both outside flange lengths with callipers.
5. Back-calculate. Bend deduction = sum of outside flanges − flat length. Bend allowance = 2 × (R + t) − deduction. K = (allowance ÷ 1.5708 − R) ÷ t.

Worked example: 2.0 mm CRCA, flat length 200.00 mm, formed inside radius 2.10 mm, outside flanges measuring 101.85 mm and 101.77 mm.

Flange sum 203.62 mm, so the deduction is 3.62 mm. Allowance is 2 × (2.10 + 2.00) − 3.62 = 4.58 mm. Then 4.58 ÷ 1.5708 = 2.916 mm of neutral axis radius, minus 2.10 mm of inside radius gives 0.816 mm, divided by 2.00 mm of thickness gives K = 0.41.

Three coupons from three coils will typically land within 0.02 of each other. If they do not, the thickness or the radius measurement is usually the cause.

What a 0.02 error costs

The sensitivity is easy to state: for a 90° bend, the allowance changes by 1.5708 × t × ΔK.

On 2 mm sheet, 0.02 of K moves each bend by 0.06 mm. A four-bend bracket accumulates 0.25 mm, and a six-bend enclosure 0.38 mm. Against a ±0.5 mm general tolerance that is most of the budget spent on a number nobody measured.

The error is worse when the assumption is 0.50 against a true 0.38 at R/t 1. On 2 mm sheet the allowance difference is 1.5708 × 2 × 0.12 = 0.38 mm per bend, which puts a four-bend box 1.5 mm out on the developed length. That is the size of gap that turns into a re-cut blank and a late delivery.

K in the CAD model and K at the brake

Most sheet metal CAD packages ship a default K, often 0.5, sometimes 0.44, and apply it to every bend in the part. The model then produces a flat pattern that is internally consistent and externally wrong.

Two habits close the gap. Build the sheet metal table against the die set, not against the software default, and name the table by die opening so it is obvious when the wrong one is applied. Then, at first-off, measure the formed part and correct the table rather than the part: if the flange is long by 0.3 mm and the bend is right, the flat is short and the table is where the fix belongs.

On our brake the bend table lives with the tool in the Delem control, and the programme carries the table that matches the die loaded for that job. When a job moves to a different die, the flat is recalculated before the blank is cut, not after.

K on stainless, aluminium and coated sheet

The K mechanism is the same, but the numbers are not transferable.

Austenitic stainless such as 1.4301 work-hardens, springs back more and needs a larger formed radius for the same die opening. If you keep the mild-steel K, the model predicts a tighter radius than the shop produces, and the flat comes out long.

Aluminium alloys vary more than steel between grades. 5052 bends cleanly at moderate radii, while the higher-strength tempers crack at radii that CRCA handles without trouble, which is why the minimum radius question comes before the K question.

Coated and galvanised sheet behaves close to the base metal for K, because the coating is microns thick compared with the sheet. The coating does change friction and can crack on a tight bend, so the radius decision is driven by the finish, not by the allowance. Minimum bend radius by material covers the radius side.

Where a single K-factor stops working

Four cases need a different model rather than a better number. Coining drives the material into the punch and the neutral axis moves with the punch radius. Hemming folds the sheet back on itself with a completely different strain pattern. Large-radius forming, where R/t is above 5, behaves close to elastic, so the neutral axis is near mid-thickness and the allowance approaches the simple arc. And deep drawing is not a bend at all: the material is stretched over a punch and the blank size comes from draw allowance, not bend allowance.

For roll-formed sections and bump-formed radii, the tooling supplier's compensation beats any general formula.

How Ganesh sets the bend table

Bending runs on a 200 T, 5-axis CNC press brake with a 4,450 mm bed and Delem control, working to 10 mm thickness. The bend table for a new part is set at first-off from the measured radius and the measured flange lengths, then tied to the die set and the material batch.

Blanks are laser cut on a 12 kW fibre laser with a 40 ft × 16 ft bed, supported by 6 kW and 3 kW machines, so the cut features that the flat pattern references are held within ±0.1 mm typically. ISO 9013 classifies thermal cut quality from 0.5 mm to 32 mm, and a clean cut edge matters at the bend line because a dross-heavy edge starts cracks on tight radii.

Parts are accepted to ±0.5 mm general tolerance, tighter on critical features by agreement, with first article inspection available. The bend allowance calculator runs the arithmetic with your own K, and how to calculate bend allowance walks through the full flat-length calculation. Springback, which moves the radius that K is derived from, is covered in how springback affects pressed components. The bending capability page lists the machine and the thickness range, and the bending, welding and assemblies hub indexes the cluster.

What to put on the drawing

• Inside radius per bend, with a tolerance, or a note that the radius follows the die and a value to be confirmed at first-off.
• Bend angle and its tolerance. ISO 2768-1 covers angular dimensions where no tolerance is given, but its general classes are usually looser than a bend that controls assembly.
• The material standard and thickness, so a substitution can be assessed before it changes K.
• Which radius definition the drawing uses, inside or outside, stated once in the title block.
• Grain direction where a tight radius sits across the rolling direction.
• The flat pattern marked reference only, with the note that the supplier's bend table governs.

Bend test evidence, where the customer asks for it, would follow ISO 7438, which specifies the method for assessing a material's capacity for plastic deformation in bending and the test report content.

None of this replaces the coupon. Ten minutes at the brake produces a K that matches your die, your coil and your machine, and that number is worth more than any table in a design guide, including this one.