Flat pattern of a bent part: blank length, K-factor and bend deduction

Why a flat pattern is needed

A bent sheet part is cut as a flat blank and then bent. If the blank length is taken as the plain sum of the drawing sizes, the finished part comes out longer or shorter than needed: in each bend the outer part of the sheet stretches, the inner part is compressed, and the length between them stays unchanged only in the neutral layer.

So the blank length is calculated as the sum of the straight parts and the arc lengths along the neutral layer. The error in one bend is small, but in a part with four to six bends it adds up and can take a size out of tolerance.

Basic formulas

The arc length along the neutral layer of one bend: BA = π · α/180 · (r + K · s). Here α is the bend angle in degrees, that is how far the flange turns (90° for a right angle), r is the inside radius, s is the thickness, K is the neutral layer position factor.

The corner setback is the distance from the start of the arc to the «virtual» corner where the flange surfaces would meet without a radius. For the outer surfaces sb = (r + s) · tan(α/2), for the inner ones sb = r · tan(α/2). The straight part of a flange equals the drawing size minus the corner setbacks at its ends.

The bend deduction BD is the same correction written differently: BD = 2 · (r + s) · tan(α/2) − BA. The flat pattern for outside sizes equals the sum of the sizes minus BD over all bends. For a right angle, r = s = 3 mm and K = 0.38 the deduction is 5.5 mm.

How the sizes are dimensioned on the drawing

The formula depends on it, so the first question to the drawing is what the sizes are measured to. Outside sizes run to the virtual corner of the outer surfaces, inside sizes to the virtual corner of the inner surfaces, and sometimes the drawing gives the lengths of the straight parts up to the start of the bend.

• outside sizes: straight part = size − (r + s) · tan(α/2) at each end;
• inside sizes: straight part = size − r · tan(α/2) at each end;
• lengths of straight parts: straight part = size, only the arcs are added to the sum.

A wrong mode gives a deviation of several millimetres in every bend: for a 3 mm sheet and a 3 mm radius the difference between outside and inside sizes in one right angle is 2 · s = 6 mm per bend.

The K-factor

K shows at what share of the thickness from the inner surface the neutral layer lies. With a very large radius the bend hardly deforms the sheet, the layer lies in the middle and K is close to 0.5. The smaller the radius relative to the thickness, the more the neutral layer shifts towards the inner surface and the smaller K is.

The table below gives the values the calculator takes in the «auto» mode for steel. They are practical guides, not requirements of a standard: the real K depends on the material, rolling direction, angle, tool and bending method, so for precise parts it is confirmed by a trial bend.

Example: U-profile

Take a U-profile with outside sizes of 30, 100 and 30 mm, a thickness of 3 mm and an inside radius of 3 mm, two right angles. The r/s ratio is 1, and from the table K = 0.38.

Bends in opposite directions: Z and omega

The formulas do not change when adjacent bends go in different directions. The size of the middle flange is taken between the virtual corners lying on the surfaces where they are formed: for a Z-profile it is the distance between the outer corner of the first bend and the outer corner of the second, and on the drawing it coincides with the overall height of the profile.

An omega profile and a tray with sides have four bends. The sum of the deductions accumulates, so on such parts the difference between the plain sum and the correct flat pattern is the largest: in the calculator example an omega with sizes of 20, 30, 100, 30 and 20 mm at a thickness of 2 mm is almost 15 mm shorter than the plain sum.

Radius and air bending

The bend radius is set by the drawing or determined by the tool. In air bending on a press the inside radius is proportional to the die opening, roughly 0.16 of the opening, and the smallest flange that can still be bent is about 0.7 of the opening. The force for the chosen die is calculated by the air bending formula or the calculator.

A radius smaller than the sheet thickness risks cracks in the bend zone on many steels, and a very large radius increases springback. Both limits depend on the steel grade and the rolling direction, so the minimum radius for a critical part is agreed with the production.

Where the error comes from

Three main sources: the uncertainty of K, the scatter of the radius and the change of sheet properties between batches. For a right angle a change of K by 0.05 gives about 0.08 · s per bend, that is 0.24 mm for a 3 mm sheet and about 1 mm for a 12 mm sheet; in a part with six bends this adds up.

That is why the flat pattern of critical parts is checked by a trial bend: one blank is bent, measured, K or the length is corrected if needed and only then the batch is started. Springback is corrected by setting the press, not by the length of the flat pattern.

What to state on the drawing of a bent part

• the thickness and the steel grade;
• the inside radius of every bend and the angle (or the inside angle between the flanges);
• what the sizes are dimensioned to: outer corners, inner corners or the lengths of the straight parts;
• the rolling direction, if it matters for strength or appearance;
• tolerances on linear sizes and angles;
• the flat pattern as a reference size: it is given by agreement, because the final length depends on the manufacturer’s tool.

The general rules for KM and KMD drawings are covered in the article Rules for KM and KMD drawings.

Standards and validity

The formulas in the article are the general geometry of sheet bending, not requirements of a particular standard. The values of K, radius and error are practical guides. Tolerances on the sizes and angles of bent parts are taken from the drawing and the order conditions.