What is the bend allowance formula?

Bend allowance (BA) = pi x (R + K x T) x (A / 180), where R is the inside bend radius, K is the K-factor, T is material thickness and A is the bend angle in degrees. It gives the arc length of material consumed by one bend. Add the bend allowance to the sum of the straight flange lengths and you have the flat pattern length.

What is the K-factor?

The K-factor expresses where the neutral axis sits inside the bend, as a fraction of thickness. A K of 0.33 means the neutral axis is one third of the way through the material from the inside face; 0.5 would be the mathematical centre. It shifts with the bend radius and the material's yield strength: tighter radii push K down, and high-strength alloys push it down further because less material is in tension or compression.

What is bend deduction and how is it different from bend allowance?

Bend deduction (BD) is what you subtract; bend allowance is what you add. BD = 2 x outside setback - BA. Using the wrong one is the classic flat-pattern error. Bend deduction is usually easier for a shop because the outside setback is a measurable value on the finished part, so quote the formula to whichever convention your CAD tool uses and check it against a first article.

Why do two shops produce different flat lengths for the same drawing?

Almost always because of the K-factor assumption. A shop using K = 0.33 and one using K = 0.42 on the same 2mm material at the same radius will land several millimetres apart on the developed length, and every hole in the flat moves with it. The fix is to state the K-factor on the drawing, or to dimension features in the finished condition rather than the flat.

How much does spring-back affect the final angle?

Spring-back is the elastic recovery of the material after the load is released, so the part opens up. Mild steel at 1x t radius typically springs back 1 to 3 degrees, aluminium alloys 3 to 5, and stainless or high-strength steels 4 to 8. Over-bending by the expected spring-back and letting it relax is standard practice, which is why repeatability is quoted as plus or minus 1 degree rather than exact.

What is the difference between air bending, bottoming and coining?

Air bending presses the punch into a die opening without the material touching the bottom - the most common method, high flexibility, wider radius tolerance. Bottoming closes the material fully into the die corners for a tighter radius at higher force. Coining presses the full flat faces together to control the thickness precisely, for high-strength or spring-critical material. Most laser-cut-and-bend work is air bent.

Does the bend radius change the flat length as much as the thickness?

Yes, and less obviously. On 2mm mild steel at 90 degrees, going from a 1x t radius (2mm) to a 3x t radius (6mm) takes the bend allowance from 4.40mm to 10.68mm - roughly 6mm of extra flat length for that single bend. That is not obvious when you add up the leg dimensions, and it is why generous radii do not always cost less: they consume flat length, and on a nested layout that flat length is material.

How should I dimension a bent part to avoid flat-pattern disputes?

Dimension the finished part, not the flat. Use the flange lengths as measured after bending, reference the bend line as a dimensioned reference, and if a hole has to land in a specific place after forming, either state the K-factor you are using or move the operation to after bending. The DFM rules for this are on the sheet metal design guidelines page.

Bend Radius and Bend Allowance

The developed length of a bent sheet is not the sum of its legs. Somewhere inside every bend, metal is stretched on the outside and compressed on the inside, and the neutral layer between them is what consumes the extra length. This page gives the formula, the K-factor values, the difference between bend allowance and bend deduction, and a full worked example.

The Four Values You Need

Term	Symbol	What It Means
Material thickness	T	Nominal thickness of the sheet being bent.
Inside bend radius	R	Radius of the concave side of the bend. It is not chosen independently — it is a consequence of the tooling and the thickness.
K-factor	K	Where the neutral axis sits, expressed as a fraction of thickness, measured from the inside face.
Bend angle	A	The angle through which the material is bent, in degrees. 90° is the common case.

Inside radius is not free. On standard air-bending tooling the achievable inside radius is roughly one material thickness. Asking for a smaller radius does not simply sharpen the corner — it changes the tooling and the flat length. The design rules are in design for sheet metal.

The Bend Allowance Formula

BA = π × (R + K × T) × (A / 180)

Bend allowance is the arc length of material consumed by one bend.

The flat pattern length is then:

Flat Length = Sum of flange lengths + Sum of bend allowances

One bend allowance per bend. A part with four bends has four bend allowances.

Bend Deduction: The Same Problem, Subtracted

Most CAD tools work in bend deduction rather than bend allowance, because the outside setback is easier to measure on a real part:

BD = 2 × OSSB − BA

OSSB = outside setback, the distance from the mold line to the outside of the bend.

Getting these two backwards is the single most common flat pattern error. If a shop quotes a flat length 4mm short on a four-bend part, the usual cause is a sign error between the two conventions — not a K-factor disagreement.

K-Factor by Material and Radius

K is not a property of the metal alone. It moves with the bend radius and the yield strength, because both change how much material sits in tension versus compression.

Material	R < 1×t	R = 1×t	R = 2×t	R = 4×t
Mild steel (Q235 / S235)	0.32–0.38	0.38–0.42	0.42–0.46	0.46–0.50
Stainless 304 / 316	0.30–0.35	0.36–0.40	0.40–0.44	0.44–0.48
Aluminium 5052 / 6061	0.30–0.36	0.36–0.42	0.42–0.46	0.46–0.50
High-strength steel (>600 MPa)	0.22–0.28	0.28–0.34	0.34–0.40	0.40–0.45

Use the midpoint of the range for quoting. If the flat pattern carries features whose position matters after bending, state the K-factor on the drawing instead of leaving each supplier to pick — see the hole spacing rules for why the resulting millimetre differences matter.

Worked Example: 2mm Mild Steel, 90° Bend

A U-channel with two 50mm flanges and a 60mm web, in 2mm Q235 mild steel, formed with standard tooling at a 2mm inside radius.

Step	Calculation	Result
Inside radius R	Standard tooling at 1×t on 2mm	2.0 mm
Material thickness T	Nominal	2.0 mm
K-factor K	Mild steel at R = 1×t, midpoint of 0.38–0.42	0.40
Bend angle A	Each of two bends	90°
Bend allowance per bend	π × (2.0 + 0.40 × 2.0) × (90/180)	4.40 mm
Total straight legs	50 + 50 + 60	160.0 mm
Flat pattern length	160.0 + (2 × 4.40)	168.80 mm

Now check the sensitivity. If the shop had assumed K = 0.33 instead of 0.40, the bend allowance becomes 4.18mm and the flat length 168.36mm — 0.44mm out on a two-bend part. On a four-bend bracket that difference roughly doubles, and the last feature ends up close to 1mm from where the drawing put it.

Spring-Back

Sheet metal is elastic, so it recovers part of its deformation when the load is released and the part opens up. Shops compensate by over-bending and letting it relax, which is why press brake repeatability is quoted as a range rather than an exact angle.

Material	Expected Spring-Back at 90°, R = 1×t	Handling
Aluminium 5052	3° to 5°	Over-bend and check on the first article; anneal condition varies between coils.
Aluminium 6061-T6	4° to 6°	Temper matters more than alloy. Verify per batch.
Mild steel Q235	1° to 3°	Stable and forgiving; the easiest material to bend repeatably.
Stainless 304 / 316	4° to 7°	High spring-back plus higher forming force. Anneal condition changes it.
High-strength steel >600 MPa	5° to 8°	Narrow process window; needs tighter incoming material control.

Air Bending, Bottoming and Coining

Method	How It Works	Use When	Cost Impact
Air bending	Punch presses into the die opening; material never touches the die bottom	Default for laser-cut-and-bend work; prototypes and low volume	Lowest — standard tooling
Bottoming	Material is closed fully into the die corners	Tighter inside radii, repeatability across batches	Moderate — requires matched tooling
Coining	Full flat faces pressed together to control thickness	High-strength or spring-critical material where thickness must be controlled	High — dedicated tooling and higher force

Our press brake work is air bent on 100t / 3200mm capacity with ±1° repeatability. Tight radii or controlled thickness are quoted case by case.

Common Mistakes

#	Mistake	Consequence	Correct Approach
1	Using bend allowance where the tool expects bend deduction	Flat length short by roughly 2×OSSB per bend	Confirm the convention with the supplier before releasing the flat.
2	K-factor assumed rather than stated	Holes land off position; parts rejected at assembly	State K on the drawing, or dimension in the finished condition.
3	Adding one bend allowance for a multi-bend feature	Channel or box collapses; parts do not assemble	One allowance per bend, counted individually.
4	Ignoring spring-back	Flange sits outside its mating part	Allow for material spring-back; verify on the first article.
5	Tight radius requested with no tooling note	Per-part tooling charge quoted unexpectedly	Design at 1×t or above unless appearance demands tighter.
6	Flange height below 1×t	Tool interference, corner cracking, rework	1.5×t minimum, 2×t for functional or visible flanges.
7	Flat pattern with no bend-line reference	Bend location ambiguous; every bend lands differently	Add the bend line as a dimensioned reference on the flat.
8	Bend allowance rounded too early	Compounding error across several bends	Keep full precision through the calculation; round once at the end.

Related Sheet Metal Pages

Design for Sheet Metal — minimum flange, radius and hole spacing rules
Sheet Metal Material Selection — which alloy to specify and why
Tolerance and Surface Finish — how bend variation lands in your tolerance stack
Sheet Metal Fabrication Service — press brake capacity and lead times

Have a flat pattern that keeps moving? Send the drawing with the material grade and we will return the developed length, the K-factor used, and any feature whose position changes after bending.

Request a Flat Pattern Review

← Design for Sheet Metal

Material Selection →