How to calculate bend allowance and bend deduction

How to calculate bend allowance in one line: for a 90° bend it is 1.5708 × (R + K × t). A 3 mm CRCA part bent at a 3 mm inside radius with K = 0.44 has 6.79 mm of bend allowance, a 5.21 mm bend deduction, and a flat length 5.21 mm shorter than the sum of its two outside dimensions.

Getting that number wrong is how a bracket arrives 2 mm long on a 200 mm flange and nobody can say whether the laser was wrong, the brake was wrong or the drawing was wrong. The allowance is a property of the tool and the material, not of the machine alone, and it changes whenever either changes.

The steps below use the standard air-bend formula, show the arithmetic for each input, give the allowance and deduction by thickness, and list the four things that make a released flat pattern disagree with the formed part.

How to calculate bend allowance: the formula and its three inputs

The formula is BA = (π/180) × θ × (R + K × t), where θ is the bend angle in degrees, R is the inside radius in millimetres, t is the sheet thickness in millimetres and K is the position of the neutral axis as a fraction of the thickness.

Three of those inputs are routinely misread.

• θ is the bend angle, not the included angle. A 90° corner has θ = 90°. A 120° included angle is θ = 60°, and using the included angle overstates the allowance by 50%.
• R is the inside radius after forming, not the punch radius. On an air bend the material springs back and the radius grows, and on a large die opening the radius is set by the die, not the punch. A punch with R1 in a 50 mm V die will not produce R1 on 3 mm sheet.
• K is a measured material and tool property. It sits between 0.33 for a tight bend and 0.50 where the neutral axis reaches mid-thickness. K-factor in sheet metal bending covers how to determine it; assume 0.42 only as a starting point.

The 1.5708 is π/2, which is the 90° case only. For any other angle, keep the (π/180) × θ term explicit.

Worked example: 3 mm CRCA, 90°, R3

Take a channel with a 250 mm outside base and an 80 mm outside leg, 3 mm CRCA, inside radius 3 mm, K = 0.44.

Step 1, neutral axis offset: R + K × t = 3 + 0.44 × 3 = 4.32 mm.

Step 2, bend allowance: 1.5708 × 4.32 = 6.79 mm.

Step 3, outside setback: (R + t) × tan(θ/2) = 6 × tan 45° = 6.00 mm per side, so 12.00 mm for both.

Step 4, bend deduction: 2 × setback − BA = 12.00 − 6.79 = 5.21 mm.

Step 5, flat length: 250 + 80 − 5.21 = 324.79 mm.

Check the result against the formed part: the two outside faces add to 330 mm, and 5.21 mm of that material is consumed by the corner. If the laser cuts 330 mm, the part finishes 5.21 mm long. If it cuts 324.79 mm and the brake uses the same die and the same material, the legs come out at 250.0 and 80.0 within the brake's flange tolerance.

Bend allowance and deduction by thickness

Values are for 90° air bends on 350 MPa cold-rolled steel with the inside radius at 1.0t, a die opening of 6t and a K-factor that rises with R/t.

Read the table as a starting point, not as a bend table. Every value depends on the measured radius, and the measured radius depends on the die that is actually loaded. A shop running an 8t or 10t die on the same gauge gets a larger radius, a larger allowance and a shorter flat for the same outside dimensions.

Bends that are not 90°

The angle term scales the allowance linearly, but the setback uses the tangent of half the angle, so the deduction does not scale the same way.

For a 60° bend on the same 3 mm material at R3, K = 0.44: BA = (π/180) × 60 × 4.32 = 4.52 mm. Setback = 6 × tan 30° = 3.46 mm per side. Deduction = 2 × 3.46 − 4.52 = 2.40 mm.

So a 60° bend on a 250 + 80 mm part gives a flat of 327.60 mm, not the 324.79 mm of the 90° case. On a part with mixed angles, calculate each bend separately and sum the deductions; averaging them is how a bracket ends up 1.5 mm over.

For bends above 90° (an acute corner), the same formula holds, but the punch and die must allow the flange to rotate past the vertical, and the tooling limits in minimum flange length for press brake parts apply before the arithmetic matters.

Why the radius in the table is not the radius you draw

On an air bend the sheet touches the punch at a line and the die at two shoulders. The inside radius forms as a fraction of the die opening, roughly 0.15 to 0.18 × V on mild steel, and the punch radius only caps it when the punch is blunter than the natural radius.

That produces two practical rules. If the drawing calls R1 on 3 mm sheet but the die is 50 mm, the shop will produce about R8, and the flat pattern must be built on R8. If the drawing calls R8 but the die is 18 mm, the shop will produce about R3, and a part bent to R3 has a different allowance, a different springback and a different flange length.

This is the single most common reason a flat pattern released with the drawing comes back different: the model was built on the drawing radius and the shop formed the natural radius of its die set.

Four things that move the flat length after release

• Thickness tolerance. Cold-rolled sheet is not exactly nominal. A 0.1 mm variation on 2 mm material changes the allowance by 1.5708 × 0.42 × 0.1 = 0.07 mm per bend, which is 0.27 mm on a four-bend box. Measure the coil and recalculate.
• Material grade. Stainless at 1.4301 work-hardens, springs back more and often needs a larger natural radius, so both K and R move. Aluminium 5052 behaves differently again. Do not reuse a mild-steel bend table.
• Die change at quotation. A supplier who substitutes a different V opening to suit an existing tool changes the radius and therefore the flat. This is a drawing change and should be raised as one.
• Cut edge condition. A laser-cut blank with heavy dross or a notched edge concentrates strain at the bend line and can crack on a tight radius. ISO 9013 classifies thermal cut quality from 0.5 mm to 32 mm, which is the range where a laser-cut edge is typically accepted for bending without dressing.

Where the 5-axis brake changes the answer

Bend allowance is a two-dimensional calculation. A long part bends in three dimensions because the ram deflects in the middle, and a single-axis brake then produces a flange height that varies along the length by 0.3–0.8 mm on a 4 m part.

The 5-axis control on our brake compensates the ram position and the back gauge through the stroke, which keeps the flange dimension consistent along a 4,450 mm bend. What it cannot do is change the allowance: the same arc length applies across the full bed, so a long part cut to the flat length will still finish to the same overall length end to end. Angle drift is the other direction of error, and how springback affects pressed components covers how angle and radius move together after unloading.

Where Ganesh applies this

Bending runs on a 200 T, 5-axis CNC press brake with a 4,450 mm bed and Delem control, working to 10 mm thickness. The bend table for a part is set at first-off from the measured radius and the measured flange lengths, and it is tied to the die set and the material batch rather than to a generic chart.

Blanks come off a 12 kW fibre laser on a 40 ft × 16 ft bed, with 6 kW and 3 kW support machines, so the cut features that the flat pattern depends on are held within ±0.1 mm typically. Parts are accepted to ±0.5 mm general tolerance, tighter on critical features by agreement, with first article inspection available.

The bend allowance calculator runs this arithmetic for your thickness, radius and angle. The bending capability page lists the brake, the bed and the thickness range, and the bending, welding and assemblies hub indexes the rest of the cluster.

What to put on the formed-part drawing

• Inside or outside dimensioning, stated once, in the title block, with a note that the flat pattern follows it.
• Inside radius with a tolerance, or a note that the radius follows the die, with the natural radius quoted.
• Bend angle with a tolerance per bend. ISO 2768-1 covers angular dimensions only where the drawing does not specify a tolerance, and its general class is usually too loose for a bend that controls assembly.
• Material grade and thickness standard, so a substitution can be assessed before it is made.
• Grain direction where a tight radius is involved, because bending across the rolling direction cracks sooner than bending along it.
• The flat pattern, marked reference only, with the note that the supplier's bend table governs.
• Bend sequence where a part cannot be formed in one pass, since the sequence can change which flange is dimensioned from.

The bending tolerance and inspection note explains how these call-outs are verified at first-off.

When the bend allowance formula is the wrong tool

Air bending is what the formula describes. Coining pushes the material into the punch radius and shifts the neutral axis, so a coined part needs a measured K, not a calculated one. Hemming, curling and closed seams fold the sheet back on itself and do not follow the arc model at all. Roll forming of long sections and bump forming of large radii need their own compensation, and deep-drawn parts are governed by draw allowance rather than bend allowance.

Above 10 mm the brake stops being the right process for most parts, and thick plate is cut and welded or formed hot. If your part sits in any of those categories, say so on the enquiry: the flat length will come from a tool trial, and quoting it from a formula would be a guess with a number attached.

Send the drawing with the flat pattern, the material and the quantity, and the bend table will be checked against the die set before the part is released. Use the RFQ checklist to make sure the revision, the quantity and the material standard travel with the file.