Sheet Metal Bend Allowance Calculator

Use this sheet metal bend allowance calculator to estimate the material consumed by a bend before you release a part for fabrication. Enter the material thickness, inside radius, bend angle, K-factor, and the two outside flange dimensions to calculate bend allowance (BA), bend deduction (BD), outside setback (OSSB), and an estimated flat length.

Sheet Metal Bend Allowance Calculator
01 / Parameters

Define the bend

in
T / stock gauge
in
R / tool nose radius
in
First outside flange
in
Second outside flange
90°
Included angle of the bend
0.33
Typical air-bend range: 0.30 - 0.45
02 / Output

Cut-ready numbers

LIVE CALC
Bend allowance / BA
0.132
in
Bend deduction / BD0.120 in
Outside setback / OSSB0.126 in
Flat length (A + B - BD)1.880 in
Bend section / neutral axis90°
R + K·TTθneutral axisK-factor locatesthe stretch line
Values are estimates. Confirm with your tooling, material and bend chart.
Bend allowance
BA = θ × (R + K × T)

θ is the bend angle in radians. The neutral axis length becomes the material consumed by the bend.

Bend deduction
BD = 2 × (R + T) × tan(θ/2) − BA

Use BD when your outside dimensions are measured to the mold line.

Flat length
A + B − BD

Add your two outside flange dimensions to get a cut-length estimate.

For production work, validate the K-factor against a test coupon. Springback, grain direction, tooling radius and material temper can shift the result.

How to Use the Calculator

Step 1: Choose the unit system

Select IN for inch-based drawings or MM for metric drawings. The calculator converts the dimensional fields when you switch units. Bend angle remains in degrees, and K-factor remains a unitless ratio.

Step 2: Enter material thickness (T)

Enter the actual sheet thickness, not only the nominal gauge name. For example, use 0.063 in or 1.60 mm when that is the measured or specified stock thickness. Thickness affects both the neutral-axis location and the outside mold-line calculation.

Step 3: Enter the inside radius (R)

Use the finished inside bend radius created by the selected punch, material, and forming method. Do not substitute the punch nose radius if the resulting part radius is different. A change from 1.0 mm to 2.0 mm can materially change the flat pattern, especially on a large bend angle.

Step 4: Enter Flange A and Flange B

Enter the two outside flange dimensions measured from the bend intersection or mold-line convention used on your drawing. These values are used only for the flat-length estimate. If your drawing uses inside dimensions or tangent dimensions, convert them to the same outside convention before relying on the result.

Step 5: Set the bend angle and K-factor

The calculator uses the included bend angle in degrees. A 90 deg bend is the default example. K-factor describes the neutral-axis position as a fraction of the material thickness measured from the inside surface. A starting value between 0.30 and 0.45 is common for air bending, but the correct value depends on the material, tooling, grain direction, and process.

What Each Result Means

Bend Allowance (BA)

Bend allowance is the length of material along the neutral axis that is consumed by the bend. It is the most direct result when you are building a flat pattern from tangent lengths. For the default example (T = 0.063 in, R = 0.063 in, 90 deg, K = 0.33), the calculator returns approximately 0.132 in.

Bend Deduction (BD)

Bend deduction is the amount removed from the sum of two outside flange dimensions to estimate the flat blank. With the same default example, BD is approximately 0.120 in. If the outside flange dimensions are 1.000 in and 1.000 in, the single-bend flat-length estimate is 1.880 in.

Outside Setback (OSSB)

Outside setback is the distance from the outside mold-line intersection to the tangent point of the bend. It is useful for layout, inspection, and checking whether a feature is close to the bend zone. OSSB is not a substitute for a part-specific bend-clearance review.

Flat Length

For one bend using outside flange dimensions, the calculator uses Flange A + Flange B - BD. This is a practical estimate for a simple two-flange part. Multi-bend parts require a bend table or CAD flat-pattern workflow that accounts for every bend, datum, corner condition, and bend sequence.

Bend Allowance Formulas

The calculator uses the following equations:

BA = theta x (R + K x T)

BD = 2 x (R + T) x tan(theta / 2) - BA

OSSB = (R + T) x tan(theta / 2)

Flat Length = Flange A + Flange B - BD

In these equations, theta is the bend angle converted from degrees to radians, R is the inside radius, T is the material thickness, and K is the unitless K-factor. For the default 90 deg example, theta is 1.5708 radians.

The equations describe ideal geometry. Real parts also respond to material hardness, tensile strength, grain direction, rolling condition, tooling wear, press force, lubrication, and springback. Treat the output as a starting point for process planning, not as a guaranteed production dimension.

Practical Fabrication Checklist

Before releasing a flat pattern or sending a drawing to production, verify the following:

  1. Confirm the actual material thickness, grade, temper, and grain direction.
  2. Confirm the finished inside radius with the selected punch and die opening.
  3. Use one dimension convention for the entire drawing: outside, inside, or tangent.
  4. Check holes, slots, fasteners, and embosses against the bend deformation zone.
  5. Keep features outside the bend zone whenever possible, especially on thin stock.
  6. Validate the selected K-factor with a test bend or a proven internal bend table.
  7. Measure the first article and update the bend table before releasing repeat work.

For related design checks, review ShincoFab’s sheet metal tolerance chart, hole-to-bend distance chart, and sheet metal hole-size and minimum-feature chart.

Why Your CAD Flat Pattern May Differ

CAD systems often use a material-specific bend table, a different bend-angle convention, or a calibrated bend deduction rather than the generic K-factor equation above. They may also include corner relief, bend sequencing, hem conditions, flange shortening rules, and a manufacturing database maintained by your shop.

When a CAD result and this calculator disagree, first compare the definitions rather than changing the K-factor blindly. Check whether both workflows use the same included angle, inside radius, thickness, flange datum, and outside-versus-inside dimension convention. Then compare both results against a measured test coupon.

Frequently Asked Questions

These answers cover the questions we hear most often when a preliminary bend calculation does not match a drawing, CAD flat pattern, or formed test part. Use them to check your dimensioning convention, choose a sensible starting K-factor, and understand when a production bend table or DFM review is more appropriate than a generic calculator.

What is the difference between bend allowance and bend deduction?

Bend allowance is the neutral-axis arc length added to tangent lengths to account for the bend. Bend deduction is subtracted from two outside flange dimensions to estimate the flat blank. They describe the same bend from different dimensioning conventions, so the correct choice depends on how your drawing or CAD system defines the flanges.

Start with a shop-proven value, often in the 0.30 to 0.45 range for air bending, then validate it against the actual material and tooling. Aluminum, stainless steel, mild steel, sharp tools, wide die openings, and different grain directions can all shift the neutral-axis position. A test coupon is more reliable than a universal default.

Your CAD system may use a calibrated bend table, a different bend-angle convention, or a bend deduction measured from production data. It may also apply corner relief, bend sequencing, and feature-specific rules. Compare thickness, inside radius, angle, K-factor, and flange datum first. Do not adjust one value until the conventions match.

Yes, as a first-pass estimate, provided you validate the result for the selected alloy, temper, thickness, and tooling. Stainless steel and aluminum can show different springback and forming behavior than mild steel. Confirm the inside radius, press-brake setup, and K-factor with a test bend before releasing a production flat pattern.

Springback is normally handled through the press-brake setup, over-bending, tooling selection, or a calibrated bend table rather than by hiding a correction inside the basic K-factor. Measure the formed angle and flange dimensions on the first article, record the correction, and apply the proven process value to repeat parts.

The displayed flat length is intended for one bend with two outside flange dimensions. A multi-bend part needs the allowance or deduction for each bend, plus a consistent datum and bend sequence. Use a CAD flat-pattern workflow or a shop bend table for multiple bends, hems, offsets, and formed corners.

Need a Production-Ready Flat Pattern?

The calculator is useful for early design checks, but production parts benefit from a drawing-specific review. ShincoFab can review bend radii, flange lengths, material thickness, hole-to-bend clearance, feature placement, and the manufacturing sequence before fabrication.

Request a DFM review or fabrication quote and upload your drawing with the material grade, thickness, finish, quantity, and target delivery date. A clear drawing convention helps our engineers confirm the bend calculation and return a manufacturable flat pattern.

Whatsapp

+86 13392819510

Address

Building 1, No.8, Second Street, Huangjiang Town,
Dongguan City, Guangdong Province

Socials

Facebook Youtube
Please enable JavaScript in your browser to complete this form.
Click or drag files to this area to upload. You can upload up to 3 files.

ShincoFab specializes in precision sheet metal fabrication, delivering high-quality custom metal solutions to clients worldwide with advanced technology and expert craftsmanship.

Contact Info

  • Building 1, No.8, Second Street, Huangjiang Town, Dongguan City, Guangdong Province
  • Whatsapp: +86 13392819510
  • [email protected]

Support

Get In Touch

Ready to start your sheet metal project? Contact the ShincoFab team to discuss your custom fabrication requirements. We support you through design, manufacturing, and delivery—at every stage.

Facebook-f Youtube
Scroll to Top