Skip to content
SOLID WORKS ClubSOLID WORKS Club

Tools

K-factor calculator for sheet metal bends

Enter the sheet thickness, inside bend radius, bend angle and K-factor, and the calculator gives the bend allowance, bend deduction, outside setback and the flat length of a two-flange part. Or work backwards: bend a test strip of known length, measure its legs, and get the K-factor your press brake actually produces — the value to type into SOLIDWORKS.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Cross-section of a sheet metal bend showing thickness, inside radius, neutral axis and K-factor

The formulas

Value Formula
K-factor K = t / T (neutral axis distance ÷ thickness)
Bend allowance BA = A × (R + K·T), A in radians
Outside setback OSSB = tan(A/2) × (R + T)
Bend deduction BD = 2 × OSSB − BA
Flat length L1 + L2 − BD (legs to the virtual sharp)
K from a test bend BD = L1 + L2 − flat; BA = 2·OSSB − BD; K = (BA / A − R) / T
Diagram comparing bend allowance on the neutral axis with bend deduction from legs to the virtual sharp
Bend allowance is added to legs to the tangent lines; bend deduction is taken from legs to the virtual sharp.

Worked example: 2 mm sheet, 2 mm inside radius, 90° bend, K = 0.5. BA = 1.5708 × (2 + 1) = 4.712 mm. OSSB = tan 45° × 4 = 4 mm, so BD = 8 − 4.712 = 3.288 mm. An L-bracket with outside legs of 60 and 30 mm has a flat length of 90 − 3.288 = 86.71 mm. With K = 0.33 the flat becomes 86.18 mm — half a millimetre shorter.

Choosing a K-factor

Ask your fabricator first: many shops keep their own tables for SOLIDWORKS. If you have nothing else, SOLIDWORKS' tech blog suggests starting at 0.5, and K-factors usually fall between about 0.3 and 0.5. One reseller's rule of thumb by radius:

Inside radius K-factor
R less than T 0.25
R from T to 2T 0.33
R more than 2T 0.5

The most reliable value comes from a test bend: cut a strip, measure it, bend it 90° on the press brake you will use, measure both outside legs, and enter them in the second mode above. Bend deduction should never exceed twice the outside setback; if the calculator returns a K outside 0–1, a leg was measured to the wrong reference.

Using the result in SOLIDWORKS

Type the K-factor in the Bend Allowance section of the Base Flange or the Sheet-Metal feature, or put it in a gauge table so every part uses the same values. K-factor is SOLIDWORKS' default bend calculation; bend tables, bend allowance, bend deduction and bend calculation are the alternatives — see K-factor and bend tables. The flat length shows in the flat pattern and the cut list's bounding box.

Practise it: check the blank of the sheet metal box project.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

What is the K-factor in sheet metal?

+

The position of the neutral axis as a fraction of the thickness: K = t / T. 0 is the inside face, 0.5 the middle and 1 the outside face.

How do I calculate bend allowance?

+

BA = A × (R + K × T), with the bend angle A in radians. A 90° bend in 2 mm sheet with a 2 mm radius and K = 0.5 has BA = 4.712 mm.

What is the difference between bend allowance and bend deduction?

+

Bend allowance is the arc length of the bend on the neutral axis; you add it to legs measured to the bend tangent lines. Bend deduction is subtracted from legs measured to the virtual sharp: BD = 2 × OSSB − BA.

What K-factor should I use?

+

Ask your fabricator first. As a rough guide, about 0.33 to 0.5 for most air bending; one reseller suggests 0.25, 0.33 or 0.5 depending on the radius-to-thickness ratio.