Every folded sheet-metal part starts life as a flat blank. If the blank is the wrong length, every flange after the first bend inherits the error: holes drift away from their datums, slots stop lining up with the mating part, and an enclosure that looked perfect in CAD will not close on the bench. The cause is almost always the same. The flat pattern was developed with a bend allowance that does not match how the material actually behaves on the press brake.
This article explains what happens to the metal in a bend, how bend allowance, bend deduction and the K-factor fit together, and how to measure a K-factor for your own material and tooling so flat patterns come out right first time.
What happens to the metal in a bend
When sheet is bent, the material on the inside of the bend is compressed and the material on the outside is stretched. Somewhere between the two faces is a layer that neither shortens nor lengthens. This is the neutral axis, and its length through the bend is what the flat blank has to supply.
In a flat sheet the neutral axis sits exactly at mid-thickness. As the sheet bends, it moves towards the inside face, because the inside is being squeezed harder than the outside is being stretched. How far it moves depends mainly on how tight the bend is compared with the thickness, which is why the inside radius matters so much.
The terms you need
- T: material thickness.
- Ri: inside bend radius. In air bending it is set mostly by the V-die opening, not by the punch tip.
- A: bend angle, measured as the angle the flange is bent through (90° for a right-angle flange).
- K-factor: the position of the neutral axis, as a fraction of the thickness measured from the inside face. K = 0.5 means mid-thickness.
- Bend allowance (BA): the length of the neutral axis through the bend.
- Outside setback (OSSB): the distance from the tangent point of the bend to the outside mould line, where the two outside faces would meet.
- Bend deduction (BD): how much to subtract from the sum of the outside dimensions to get the flat length.
The K-factor and bend allowance
The neutral axis follows an arc of radius Ri + K·T through the bend. Its length is the bend allowance:
BA = (π ÷ 180) × A × (Ri + K × T)A in degrees. BA is the length of material the bend consumes, measured along the neutral axis.
Most drawings are dimensioned to the outside faces of the flanges, so it is often easier to work with the bend deduction. For a bend of angle A:
OSSB = tan(A ÷ 2) × (Ri + T)
BD = 2 × OSSB − BAFor a 90° bend, tan(45°) = 1, so OSSB is simply Ri + T.
The flat length then follows from either set of dimensions. Using the straight lengths up to the tangent points, add the bend allowance. Using the outside dimensions from the drawing, subtract the bend deduction for each bend.
Flat length = L1 + BA + L2
Flat length = a + b − BDA worked example
Take a simple L-bracket in 2 mm mild steel, with outside dimensions of 50 mm and 30 mm, a 90° bend and a 2 mm inside radius. Using the rule-of-thumb K-factor of 0.45 for 2 mm sheet (see the table below):
- BA = (π ÷ 180) × 90 × (2 + 0.45 × 2) = 1.571 × 2.90 = 4.56 mm
- OSSB = tan(45°) × (2 + 2) = 4.00 mm
- BD = 2 × 4.00 − 4.56 = 3.44 mm
- Flat length = 50 + 30 − 3.44 = 76.56 mm
Now see what happens if a different K-factor is assumed for the same part:
| K-factor | Bend allowance | Bend deduction | Flat length |
|---|---|---|---|
| 0.33 | 4.18 mm | 3.82 mm | 76.18 mm |
| 0.45 | 4.56 mm | 3.44 mm | 76.56 mm |
| 0.50 | 4.71 mm | 3.29 mm | 76.71 mm |
Half a millimetre per bend does not sound like much. On a four-bend enclosure lid the error grows to around 2 mm on the blank, which is more than enough to make a lid that will not fit, or holes that miss their inserts.
Choosing a starting K-factor
In the workshop, the quickest starting point is a K-factor for each sheet thickness. These are the rule-of-thumb values we start from for steel sheet:
| Thickness | K-factor (rule of thumb) |
|---|---|
| 1.25 mm | 0.25 |
| 1.5 mm | 0.30 |
| 2 mm | 0.45 |
| 3 mm | 0.50 |
The K-factor is not a property of the material alone. It depends on the ratio of inside radius to thickness, the bending method (air bending, bottoming or coining), the tooling and, to a lesser extent, the material grade and grain direction. As a starting point, the German standard DIN 6935 gives a more general approximation based on the Ri/T ratio:
K ≈ 0.325 + 0.25 × log10(Ri ÷ T) for Ri/T < 5
K = 0.5 for Ri/T ≥ 5A good first estimate for steel. Always confirm it with a test bend on your own tooling.
| Ri / T | K-factor (approx.) | Typical situation |
|---|---|---|
| 1 | 0.33 | Inside radius equal to thickness, common in air bending |
| 2 | 0.40 | Wider V-die or softer, thicker material |
| 3 | 0.44 | Generous radius |
| 5 or more | 0.50 | Large radius, neutral axis at mid-thickness |
Remember that in air bending the inside radius comes from the die, not from the drawing. A common rule of thumb for mild steel is that the inside radius is roughly 15 to 17 percent of the V-die opening. If your model uses a 1 mm radius but the shop forms the part on a 16 mm V-die, the real radius will be closer to 2.5 mm and the flat pattern will be wrong before the K-factor is even considered.
Measuring your own K-factor with a test bend
The most reliable K-factor is one measured on the same material, thickness and tooling that will make the production parts. It takes ten minutes and a pair of callipers.
- Shear or laser-cut a strip of the production material, for example 100 mm long and at least 30 mm wide, and measure its length L0 accurately.
- Bend it to 90° on the press brake with the punch and die you will use for the real parts.
- Measure the two outside leg lengths a and b, and check the inside radius Ri with a radius gauge.
- Calculate the bend deduction: BD = a + b − L0.
- Calculate the bend allowance: BA = 2 × OSSB − BD, with OSSB = Ri + T for a 90° bend.
- Solve for the K-factor: K = (BA ÷ (π/180 × A) − Ri) ÷ T.
For example, a 100 mm strip of 2 mm steel that measures 51.9 mm on each leg after bending, with a 2 mm inside radius, gives BD = 3.8 mm, BA = 8.0 − 3.8 = 4.2 mm and K = (4.2 ÷ 1.571 − 2) ÷ 2 ≈ 0.34. That is noticeably lower than the 0.45 rule of thumb for 2 mm, which is exactly why the test is worth doing. Bend two or three strips and average the result, and repeat the test for each thickness and die combination you use regularly.
Making it stick in CAD
A correct K-factor only helps if every model uses it. Most 3D CAD packages let you set the bend allowance per part, per feature or from a shared table, and the safest approach is to make the table the single source of truth.
- Keep one bend table or gauge table per material and thickness, with the radius and K-factor (or bend deduction) your shop actually achieves.
- Model with the inside radius the tooling produces, not a default value.
- Check the flat pattern length against a hand calculation for at least one bend on a new part.
- Put the bend radius, the K-factor or bend table used, and the bend direction on the flat-pattern drawing, so the shop can see the assumptions.
- If parts are made by a subcontractor, ask for their bend data before you release DXF files, or send the folded model and let them develop the blank on their own settings.
Quick checklist
- Is the inside radius in the model the one the die will produce?
- Is the K-factor based on a test bend, a shop bend table or at least the DIN 6935 estimate for this Ri/T?
- Are the drawing dimensions outside, inside or to the mould line, and was the right formula used?
- Has one flat length been checked by hand?
- Does the drawing state the bend radius and the bend data used?
Getting the flat pattern right is cheaper than any amount of rework. A ten-minute test bend and a shared bend table remove most of the guesswork.
If you have a part that keeps coming out of the press brake slightly wrong, or you are setting up bend tables for a new material, send us the drawing or model. We can check the flat pattern development and help you build bend data that matches your tooling.