How to Calculate Flat Length (K-Factor)

Flat Length Is Not a Simple Sum
A part bent at a right angle with 50 mm and 30 mm legs does not have a flat length of 80 mm. It is shorter.
When bending, the outside is stretched and the inside is compressed, and length is redistributed. It is not conserved. If you cut blanks ignoring this difference, the finished dimensions will not match.
Neutral Axis
In a sheet cross-section, the outer surface is in tension and the inner surface is in compression. So between them there is a layer with no change in length. This is called the neutral axis, and flat length is calculated relative to it.
The neutral axis is not at the middle of the thickness; it shifts toward the inside (compression side). Two explanations are given for this, and they are not mutually exclusive.
- Metal responds more readily to tension than to compression
- During bending, sheet thickness decreases by 10 to 15% (thinning), and this thinning moves the neutral axis toward the inside
K-factor
The ratio that expresses the position of the neutral axis is the K-factor.
K = t / T
t is the distance from the inner surface to the neutral axis, and T is the sheet thickness. K = 0.5 means the center; the smaller it is, the further toward the inside.
The commonly used range is 0.3 to 0.5, but the upper limit is not fixed. Industry reference materials state "typically 0 to 0.5, and values above or below are possible." In practice, cases of 0.4 to 0.6 for hard steel and 0.46 to 0.50 for stainless steel have been reported, and bottoming and coining raise K compared with air bending. Do not assume 0.5 is the upper bound.
Calculating Flat Length
Bend allowance (BA) is the arc length measured along the neutral axis.
BA = (π/180) × bend angle × (R + K × T)
The part in parentheses is the neutral axis radius: the position shifted outward by K×T from the inside radius R.
In practice, bend deduction (BD) is used more often.
Flat length = flange A + flange B − BD
The relationship between BA and BD is as follows.
BD = 2 × OSSB − BA
OSSB (outside setback) = (R + T) × tan(bend angle / 2)
In the earlier example, the amount by which the length falls short of 80 mm corresponds to BD.
K-factor Is Not a Constant
Treating the K-factor as a material constant and quoting it from a table introduces error. It is a condition-dependent variable.
| Variable | Effect |
|---|---|
| Material | Neutral axis position differs with ductility |
| R / T ratio | The smaller R/T is, the smaller K is. For mild steel air bending, K changes from 0.38 → 0.43 → 0.50 across R/T ranges |
| Forming method | Air bending / bottoming / coining |
| V-die size | The same drawing gives different results on different equipment |
| Rolling direction | Bend direction relative to grain direction |
In Air Bending, the V-die Determines the Radius
Air bending forms the part with three-point contact between the punch and the two die shoulders, so the inside radius is determined by the V-groove width, not by the punch shape. A commonly used rule of thumb is as follows.
Ri ≈ V / 6 (V/6 to V/8 depending on the source)
In other words, even if you write R on the drawing, the actual R changes with the dies the shop owns, and when R changes K changes, and as a result the flat length differs.
Tendencies by Forming Method
| Method | Characteristics | Springback |
|---|---|---|
| Air bending | Three-point contact; die width determines R | Large |
| Bottoming | Pressed to the bottom of the die | Reduced |
| Coining | Pressed to the neutral axis; fully formed | Minimal |
Quantitative differences vary between sources, so treat this as a trend only.
In Practice
The exact K-factor is settled by measurement, not calculation. Bend a test piece and back-calculate. Sheet metal shops keep tables based on their own equipment.
In other words, the K-factor is the equipment owner's data, not something the person placing the order should calculate.
Recommendations When Ordering
- Provide a 3D model (STEP) or finished dimensions. This is the most important.
If you calculate the flat pattern yourself and send it, any mismatch with the shop's K is carried straight into the error. If you provide the finished shape, the shop unfolds it based on its own equipment. - If you must provide a flat pattern, state the K-factor used.
Writing something like "This flat pattern is based on K=0.42" lets the shop verify or recalculate it. - Specify the inside bend R.
If it is not specified, the shop's standard die is used. - State the reference surface for bend dimensions.
If you do not state whether it is inside, outside, or center, interpretations will differ by the sheet thickness.
Minimum Bend Radius
If the inside radius is too small, cracks form on the outer surface. The minimum R depends on material ductility.
We do not give numbers. In our research, values such as SPCC (cold-rolled steel) 0.4 to 1T, AL5052 (5052 aluminum) 0.5 to 1.5T, AL6061-T6 (6061 aluminum) 2 to 6T, and SUS304 (304 stainless steel) 1 to 3T were found, but they vary widely by source, and depend on temper (H32/T6/annealed), thickness range, and forming method. Fixing a single table requires measured data from the equipment and material supplier.
The qualitative trends are as follows.
- AL5052-H32 — Elongation 12 to 25%. Good bendability
- AL6061-T6 — Elongation 8 to 10%. Higher cracking risk than 5052, so a larger minimum R is needed
- SUS304 — High work hardening and large springback
Rolling Grain Direction
Bending parallel to the rolling grain direction increases cracking risk. The rule is to bend perpendicular to the grain; if parallel bending is unavoidable, increase the minimum radius by 50 to 100%. When nesting many parts on a large sheet, this direction governs the nesting.
Springback
When the forming force is removed, elastic recovery occurs. A part formed to 90° may spring back to 88°. In practice, this is compensated by overbending.
Springback increases under the following conditions.
- The higher the material strength
- The larger the bend radius R
- The thinner the sheet
It is especially pronounced in SUS304 and high-strength aluminum. Compensation is the equipment owner's domain.
FAQ
My CAD calculates the flat pattern. Can I use it as is?
The default K value in CAD is an assumed value. If it does not match the shop's actual equipment, the error is carried straight through. It is fine for reference, but risky to use as a cutting instruction.
Isn't K=0.33 the standard?
It is a widely quoted approximation but not a universal value. As the R/T ratio grows, it approaches 0.5.
Which is safer to provide: a flat pattern or a 3D model?
A 3D model is safer. Flat patterns depend on equipment conditions, so having the equipment owner calculate them gives less error.
Summary
- When bending, outside tension and inside compression redistribute length
- The flat pattern is based on the neutral axis, and the ratio of its position is the K-factor
- K is not a constant. It depends on material, R/T, forming method, and V-die, and 0.5 is not an upper limit either
- In air bending, the V-die width determines the actual R (Ri ≈ V/6)
- Providing the finished shape (STEP) is safer than calculating and sending a flat pattern
Upload a drawing and we can review bendability and flat dimensions together.
Have a part to machine?
Upload a drawing to see your quote.



