Key takeaways
- Bend allowance is the length of the neutral axis through the bend, and it is what the flat blank has to contain.
- The K-factor locates the neutral axis between the inside surface and the mid-thickness, and it moves with the radius to thickness ratio.
- Bend deduction converts two formed leg lengths into a flat length, so the blank is shorter than the sum of the legs.
- A radius below the material minimum is a cracking and tool wear decision, not a spreadsheet rounding error.
Three numbers that are often confused
Bend allowance, bend deduction and K-factor describe the same geometry from different directions. The bend allowance is the arc length of the neutral axis through the bend. The bend deduction is the amount you subtract from the sum of the two outside leg lengths to get the flat length. The K-factor is the fraction of the thickness at which the neutral axis sits, measured from the inside surface.
In a press brake or a stamping die, the metal on the inside of the bend compresses and the metal on the outside stretches. Somewhere between them is a layer that keeps its length. That layer is the neutral axis. It is not exactly at mid-thickness, because the bend is not a pure geometry exercise: friction, tool pressure and the material's strain behaviour all pull it toward the inside.
If the flat blank ignores the bend allowance, the formed part comes out short on both legs. The error is small on a single 90 degree bend and grows with every additional bend, which is why a bracket with six bends can finish outside tolerance even when each individual bend looks acceptable.
What the K-factor is doing
The K-factor is usually between 0.33 and 0.50 for cold-rolled steel. A value near 0.33 suits a tight bend where the neutral axis stays close to the inside surface. A value near 0.50 suits a generous radius where the strain is spread through the thickness and the neutral axis approaches mid-thickness. The ratio that drives the change is the inside radius divided by the thickness.
The practical point is that K is not a material constant you can look up once. It depends on the radius to thickness ratio, the forming method and the tooling. Air bending, bottoming and coining all produce different strain patterns, so the same material can need a different K for each route. Confirm the value on the first trial by measuring the formed part.
The bend allowance formula
The bend allowance for an arc is the radius of the neutral axis multiplied by the bend angle in radians. Written with the inside radius R, the thickness t and the K-factor, it becomes: bend allowance equals pi times the quantity R plus K times t, multiplied by the bend angle in degrees, divided by 180.
That single expression covers the arc. To get a flat length, you also need the setback, which is the distance from the bend tangent point to the outside corner. The outside setback for one side is the quantity R plus t multiplied by the tangent of half the bend angle. The bend deduction is twice the outside setback minus the bend allowance. Flat length is leg one plus leg two minus the bend deduction.
The tangent term is why a 90 degree bend is easy and a 30 degree bend is not. At small angles the setback shrinks quickly, and a small error in the angle or the radius has a larger effect on the deduction.
A worked example in 2.0 mm mild steel
Take a 90 degree bend in 2.0 mm mild steel with an inside radius of 2.0 mm, a K-factor of 0.42, and two outside legs of 30 mm and 20 mm. The neutral axis radius is 2.0 plus 0.42 times 2.0, which is 2.84 mm. The bend allowance is pi times 2.84 divided by 2, which is 4.46 mm.
The outside setback is 4.0 mm multiplied by the tangent of 45 degrees, which is 4.0 mm. Twice that is 8.0 mm, so the bend deduction is 8.0 minus 4.46, which is 3.54 mm. The flat length is 30 plus 20 minus 3.54, which is 46.46 mm. A blank cut to 50 mm would produce a part with legs about 1.8 mm long on each side, and the error would be blamed on the press.
The numbers are illustrative, but the structure is not. Every bend needs its own allowance, and the flat pattern is the sum of the straight sections plus the allowance for each bend.
| Line | Value | Where it comes from |
|---|---|---|
| Thickness, t | 2.0 mm | Nominal gauge, confirm mill tolerance |
| Inside radius, R | 2.0 mm | Punch or die geometry |
| Bend angle | 90 degrees | Drawing |
| K-factor | 0.42 | Starting value for this radius to thickness ratio |
| Neutral axis radius | 2.84 mm | R plus K times t |
| Bend allowance | 4.46 mm | Arc length through the bend |
| Outside setback, one side | 4.00 mm | (R plus t) times tan(angle/2) |
| Bend deduction | 3.54 mm | Twice setback minus bend allowance |
| Flat length | 46.46 mm | 30 plus 20 minus 3.54 |
Illustrative only. Confirm the K-factor and the tooling route with the supplier before releasing a blank.
Minimum inside radius by material
The minimum inside radius is a formability limit. For mild steel, an inside radius at or above one thickness is a reasonable default. For stainless steel and high-strength grades, the limit rises, often to one and a half or two times thickness, because the outer fibre reaches its strain limit sooner and the material work-hardens as it bends.
Copper and brass are more forgiving in the annealed condition, but they are usually specified in a temper that trades formability for spring force. A half-hard brass contact will crack at a radius that an annealed strip would take without complaint. Aluminium sits in between, and its surface is prone to galling, so the tool needs a good finish and the lubricant needs attention.
The direction of the bend relative to the rolling direction also matters. Bending across the rolling direction is generally more tolerant than bending along it, where the elongation available at the edge is lower. If the part is critical, mark the grain direction on the drawing and ask the supplier to lay out the strip accordingly.
A sharp punch radius is not a free way to hold a small bend
The punch nose sets the inside radius, but a nose below the material minimum raises the strain, the springback and the tool wear. The saving in setup is paid back in cracks and sorting.
Tooling limits that override the calculation
In air bending, the die opening sets the inside radius more than the punch nose does. A common starting point is an opening of six to eight times the thickness for mild steel, with the exact value depending on the material and the required radius. A narrow opening gives a smaller radius but needs more force per metre and leaves less room for the punch.
A stamping die is different from a press brake because the form is built into the tool. The punch nose, the die shoulder and the clearance all fix the radius, and the material is forced to follow. Changing the radius means changing the tool, so the radius should be settled before the die is designed.
The same applies to bend relief. A bend that runs to the edge of the part needs a relief notch, or the material tears as it is pulled around the corner.
Verify on the first article, then lock the setting
The first article is where the calculated allowance meets the real material. Measure the formed legs, the inside radius and the bend angle, then compare them with the drawing. If the legs are consistently long or short, the flat blank or the bend deduction is wrong. If the angle drifts, the issue is springback or the tool setting, not the allowance.
Record the K-factor that reproduces the measured part, the coil lot and the tool setup. When the coil lot changes, check the first few parts again: a different mill heat can shift the yield strength enough to move both the springback and the finished leg length.
- Measure both legs and the inside radius on the first part
- Back-calculate the K-factor from the blank that worked
- Record the coil lot, the tool setup and the bend angle
- Recheck after a material lot change or a tool regrind
- Keep the flat pattern revision with the drawing revision
Frequently asked questions
What is the difference between bend allowance and bend deduction?
Bend allowance is the arc length of the neutral axis through the bend, and it is added to the straight sections in the flat pattern. Bend deduction is the amount subtracted from the sum of the outside leg lengths to get the same flat length. They describe the same bend from opposite directions.
What K-factor should I use for sheet metal?
A common starting range is 0.33 to 0.50, moving upward as the inside radius to thickness ratio grows. Use a value near 0.42 for a radius close to the thickness in mild steel, then confirm it on the first article. Air bending, bottoming and coining can all need different values.
How do I calculate the flat length of a part with several bends?
Add the straight sections between bend tangent points, then add the bend allowance for each bend. Alternatively, add the outside leg lengths and subtract the bend deduction for each bend. Mixed angles and radii need each bend calculated separately.
Can I use a smaller radius than the material minimum?
It is possible in soft material with a good tool, but the risk of cracking, high springback and short tool life rises quickly. For stainless and high-strength steel, stay at or above the supplier's recommended minimum and ask for a bend trial before releasing the tool.
Sources and further reading
- DIN 6935, Cold bending of flat steel products
- ISO 2768-1:1989, General tolerances, linear and angular dimensions
- Qumek DFM reviews and flat pattern checks for stamped parts
Qumek Engineering Desk
Engineering team
The engineering team behind Qumek drawings, DFM notes, tolerances and inspection standards. Every guide is reviewed against the drawings and processes used on live programmes.
Check the flat pattern before the die is cut
Send the formed drawing with the material, thickness and bend radii. The engineering desk will review the allowance, the minimum radius and the tooling route.
Send a drawing