Sheet Metal Bend Deduction Calculator

Use this Sheet Metal Bend Deduction Calculator to estimate the material to subtract from two outside flange dimensions when developing a single-bend sheet metal flat pattern. Enter material thickness, inside bend radius, bend angle, and K-factor to calculate Bend Deduction (BD), Bend Allowance (BA), and Outside Setback (OSSB). Add both outside flange dimensions to calculate an optional Flat Length. The result is a planning estimate, so validate it against your actual material, tooling, bend table, and test bend before releasing production blanks.

Sheet Metal Bend Deduction Calculator

01 / Parameters

Define the bend

mm

T / measured stock thickness

mm

R / finished inside radius

deg

Rotation from flat: 0° flat, 90° right angle.

K

Use a verified supplier value, CAD bend table, or test bend.

Optional flat length Outside dimensions

Measure A and B from the theoretical outside mold-line apex to each flange end.

mm
mm

02 / Output

Bend development

Live result
Bend deduction / BD2.866mm
Bend allowance / BA
3.134 mm
Outside setback / OSSB
3.000 mm
Radius / thickness
1.000
Flat length
97.134 mm
Single-bend geometry and outside flange conventionA sheet metal cross-section showing the inside radius, material thickness, bend angle, theoretical outside mold-line apex, and outside flange dimensions.theta = 90 degR = 1.500 mmT = 1.500 mmOutside flange A to mold-line apexTheoretical apex
Outside flanges are measured to the theoretical mold-line apex; the drawing is not to scale.
Values are estimates. Validate the final blank with production material, tooling, and a test bend.

Bend allowance

BA = theta x (R + K x T)

Theta is in radians. BA is the neutral-axis arc length consumed by the bend.

Bend deduction

BD = 2 x OSSB - BA

Subtract BD from the sum of two outside mold-line dimensions.

Flat length

A + B - BD

A and B must both use the outside mold-line apex convention.

The calculator does not predict springback, cracking, minimum radius, tooling feasibility, or production tolerance.

How to Use the Calculator

Choose MM or IN

The calculator opens in millimeters (MM). Choose inches (IN) to convert the existing dimensional values. The angle and K-factor do not change during a unit switch. Displayed metric dimensions use three decimal places; imperial dimensions use four.

Enter Material Thickness (T)

Enter the measured stock thickness, not a nominal gauge label. Thickness must be greater than zero. For gauge references, see ShincoFab’s sheet metal gauge thickness chart.

Enter Inside Bend Radius (R)

Enter the finished inside radius produced by your tool and material combination. Radius must be greater than zero. A tooling nose radius, drawing radius, and achieved formed radius may not be identical, so use the convention that matches your bend table.

Enter Bend Angle

Enter the angle through which the material rotates from flat. A flat sheet is 0°, a right-angle bend is 90°, and a finished 60° inside angle corresponds to a 120° rotation from flat. Values must be greater than 0° and less than 180°.

Enter K-factor (K)

Enter an effective K-factor from a verified supplier value, CAD bend table, or test bend. The calculator accepts 0.00 through 0.50. Do not treat the default 0.330 as a material guarantee; K-factor changes with material temper, radius-to-thickness ratio, grain direction, bend method, tooling, and calibration. ShincoFab’s K-factor guide provides additional shop-floor context.

Add Outside Flange A and B (Optional)

Enter both outside flange dimensions to calculate Flat Length. Measure A and B from the theoretical outside mold-line apex to the end of each flange, and use the same datum for both values. Leave both blank when you only need the bend quantities. Entering only one flange produces a paired-input error.

Review Results, Reset, or Copy

Results update as inputs change. Reset values restores the documented 1.500 mm, 1.500 mm, 90°, 0.330, 50.000 mm, and 50.000 mm example in the active unit system. Copy results places the inputs, conventions, and available outputs on the clipboard; browser permissions may require manual selection instead.

What the Results Mean

Bend Deduction (BD)

Bend Deduction is the amount subtracted from the sum of two outside flange dimensions to estimate a single-bend flat length. It is the primary result in this tool.

Bend Allowance (BA)

Bend Allowance is the arc length along the neutral axis through the bend. It represents the material consumed by the curved region in the selected calculation model.

Outside Setback (OSSB)

Outside Setback is the distance from a bend tangent reference to the theoretical outside mold-line apex. It uses the inside radius plus material thickness in the formula below.

R/T Ratio

R/T Ratio is the inside bend radius divided by material thickness. It is shown as a comparison value so you can spot a radius convention or input mismatch; it is not a forming-feasibility check.

Flat Length

Flat Length is A + B - BD when both outside flange dimensions are valid and the result is greater than zero. It remains unavailable when A/B are blank, paired incorrectly, or incompatible with the calculated deduction.

Bend Deduction Formula and Assumptions

The calculator uses one bend, a constant inside radius, the outside mold-line flange convention, and a user-supplied effective K-factor. The angle is the rotation from flat and is converted to radians before calculating the neutral-axis arc.

theta_rad = theta_deg x pi / 180
BA = theta_rad x (R + K x T)
OSSB = tan(theta_rad / 2) x (R + T)
BD = 2 x OSSB – BA
Flat Length = A + B – BD

For the default example (T = 1.500 mm, R = 1.500 mm, theta = 90°, K = 0.330, A = 50.000 mm, B = 50.000 mm), the unrounded calculation is approximately:

BA = 3.134 mm
OSSB = 3.000 mm
BD = 2.866 mm
Flat Length = 97.134 mm
R/T Ratio = 1.000

For a broader reference, compare the sheet metal bend allowance and bend deduction chart with the actual bend data used by your shop. The chart and this calculator are reference tools, not substitutes for a verified process value.

Practical Design and Fabrication Checklist

  • Confirm the drawing’s angle definition and convert an interior angle to rotation from flat before entering it.
  • Measure actual material thickness and record alloy, temper, coating, and lot when those details affect the bend table.
  • Use the achieved inside radius for the selected punch, die, material, and bend method rather than assuming the tool nose value is exact.
  • Keep the K-factor source with the revision of the CAD flat pattern or bend table used for the job.
  • Confirm that outside flange A and B are both dimensioned to the same theoretical mold-line apex.
  • Check grain direction, bend sequence, nearby holes, tabs, notches, and minimum flange conditions before cutting.
  • Account separately for springback and inspect a controlled test bend before releasing a production nest.
  • Keep rounding until display or documentation; do not round intermediate values during a multi-step review.

ShincoFab’s sheet metal DFM checklist and sheet metal forming services pages provide related design and process context.

Why Calculator Results May Differ

A CAD system may use a material-specific bend table, a different angle convention, an inside-dimension method, or a calibrated bend deduction rather than the generic K-factor equations here. Supplier data may use nominal thickness, a different temper, a different radius-to-thickness ratio, or a different press-brake method.

Production can also differ because of springback, grain direction, tooling wear, die opening, achieved radius, machine calibration, measurement datum, and material lot variation. The calculator does not predict cracking, minimum bend radius, bend proximity interference, springback compensation, or guaranteed tolerance. Use a test coupon and update the effective K-factor or bend deduction when production evidence shows a difference.

Frequently Asked Questions

These answers address common differences between a preliminary flat-pattern estimate, a CAD bend table, a supplier’s deduction chart, and a formed production part. Check the angle, dimension datum, material condition, and tooling assumptions before treating two numbers as contradictory.

What is bend deduction in sheet metal?

Bend Deduction is the amount subtracted from two outside flange dimensions to estimate the flat length of a single bend. In this calculator, BD = 2 x OSSB - BA.

Bend Allowance is the neutral-axis arc length consumed by the bend. Bend Deduction converts that bend behavior into the amount subtracted from outside mold-line dimensions, so the two values are related but serve different dimensioning workflows.

Enter rotation from flat: 0° for flat sheet and 90° for a right-angle bend. If your drawing gives a 60° interior angle, enter 120° because that is the rotation from the flat state.

Use a value from the material supplier, your CAD bend table, or a controlled test bend that matches the thickness, radius, material condition, grain direction, and bend method. The default 0.330 is only a worked example.

CAD may use an empirical bend table, a different angle or flange datum, bend-specific K-factors, or springback compensation. Compare the definitions and intermediate BA/OSSB values before changing the input.

You can sum individual deductions only when each bend uses consistently defined dimensions and validated bend data. This calculator is single-bend only and does not check bend sequence, bend interaction, reliefs, or proximity interference.

Need a Production-Ready Flat Pattern?

A drawing-specific DFM review can reconcile the generic formula with your material, tooling, dimension datums, bend sequence, and inspection requirements. Contact ShincoFab with a drawing or model, material and thickness, target inside radius and angle, quantities, and any known bend-table or test-bend data.

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