Sheet Metal Bend Allowance and Bend Deduction Chart

Q: What is the bend allowance formula for a 90 degree bend?

Using the angle convention on this page, BA = (pi / 2) x (R + K x T). You still need the formed inside radius, thickness, and a validated K-factor for the intended process.

Q: How do I calculate bend deduction for a 90 degree bend?

For a right-angle bend, OSSB = R + T, so BD = 2 x (R + T) - BA. Subtract that value once from the sum of the two outside flange dimensions.

Q: Is 0.33 the correct K-factor for all sheet metal?

No. 0.33 is the explicit example assumption used in this chart. K-factor can change with material condition, thickness, bend angle, radius, tooling, and forming method. Use measured or supplier-validated data for production.

Sheet Metal Bend Allowance and Bend Deduction Formulas

For this page, the bend angle A is the angle through which the flat sheet is bent: 0 degrees is flat and 90 degrees produces a right-angle bend. Dimensions L1 and L2 are finished outside flange dimensions measured to the virtual sharp intersection.

Bend allowance

BA = (pi / 180) x A x (R + K x T)

Outside setback

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

Bend deduction

BD = 2 x OSSB - BA

Flat length for one bend, using outside dimensions

Flat length = L1 + L2 - BD

Where:

BA = bend allowance, the neutral-axis arc length through the bend
BD = bend deduction from the sum of the two outside flange dimensions
OSSB = outside setback from the bend tangent to the virtual sharp
A = bend angle in degrees, using the convention defined above
R = formed inside bend radius
K = K-factor, equal to the neutral-axis location from the inside surface divided by T
T = material thickness

Use one unit system throughout a calculation, keeping R, T, BA, BD, OSSB, L1, and L2 in the same unit.

90 Degree Bend Allowance and Bend Deduction Chart

This quick chart assumes one 90-degree bend, R = T, and K = 0.33. Under those assumptions, BA = 2.089T and BD = 1.911T. Metric values control; inch equivalents are metric results divided by 25.4 and rounded to four decimal places.

Thickness T (mm)	Inside Radius R (mm)	Bend Allowance BA (mm)	Bend Deduction BD (mm)	BA (in)	BD (in)
0.5	0.5	1.045	0.955	0.0411	0.0376
0.8	0.8	1.671	1.529	0.0658	0.0602
1.0	1.0	2.089	1.911	0.0823	0.0752
1.2	1.2	2.507	2.293	0.0987	0.0903
1.5	1.5	3.134	2.866	0.1234	0.1128
2.0	2.0	4.178	3.822	0.1645	0.1505
2.5	2.5	5.223	4.777	0.2056	0.1881
3.0	3.0	6.267	5.733	0.2468	0.2257
4.0	4.0	8.357	7.643	0.3290	0.3009
5.0	5.0	10.446	9.554	0.4113	0.3761
6.0	6.0	12.535	11.465	0.4935	0.4514

Do not select a production bend deduction from thickness alone. If the actual radius or K-factor differs from this chart, recalculate the row or use a validated bend table. Check the proposed inside radius against the material-specific minimum bend radius chart before treating R = T as feasible.

Bend-Angle Multipliers for R = T and K = 0.33

The following dimensionless multipliers let you estimate BA and BD for several bend angles. Multiply the relevant coefficient by material thickness T. The same scope limits apply: these are calculated values for R/T = 1.00 and K = 0.33, not measured shop data.

Bend Angle A	BA/T	BD/T
30 degrees	0.696	0.375
45 degrees	1.045	0.612
60 degrees	1.393	0.917
90 degrees	2.089	1.911
120 degrees	2.786	4.143
135 degrees	3.134	6.523

Large-angle bend deductions grow quickly because the virtual-sharp intersection moves farther from the tangent points. Hems, curls, closed bends, and geometries approaching 180 degrees need process-specific rules rather than extrapolation from this table.

How to Use This Bend Deduction Chart

Confirm the finished part’s material specification, actual thickness, bend angle, intended inside radius, and forming process.
Use the chart only when the bend is 90 degrees, R = T, and the validated K-factor is 0.33. Otherwise, use the formulas.
Measure both outside flange dimensions to the same virtual sharp convention used by the formula.
Subtract one BD for each bend from the sum of the corresponding finished outside dimensions.
For multiple bends, calculate each bend separately. Do not reuse one value when radius, angle, material orientation, or tooling changes.
Compare the result with the CAD flat pattern and the fabricator’s bend table before cutting production blanks.

Worked Example: 1.5 mm Sheet, 90 Degree Bend

Assume T = 1.5 mm, R = 1.5 mm, K = 0.33, A = 90 degrees, and finished outside flange dimensions of 40 mm and 60 mm.

BA = (pi / 180) x 90 x (1.5 + 0.33 x 1.5) = 3.134 mm

OSSB = tan(45 degrees) x (1.5 + 1.5) = 3.000 mm

BD = 2 x 3.000 - 3.134 = 2.866 mm

Flat length = 40 + 60 - 2.866 = 97.134 mm

This result matches the 1.5 mm row after rounding. It remains a first-pass estimate until the radius and K-factor are confirmed for the production setup.

How K-Factor Changes Bend Allowance

The K-factor locates the neutral axis within the sheet thickness. A larger K-factor increases bend allowance and therefore reduces bend deduction when angle, radius, and thickness stay constant. It is not a material constant: Autodesk notes that bend angle, material, thickness, and production conditions can affect the value. For a 90-degree bend with R = T, the calculated sensitivity is:

K-Factor	BA/T	BD/T	Interpretation
0.30	2.042	1.958	Smaller neutral-axis offset; shorter bend allowance
0.33	2.089	1.911	Assumption used in this page's quick charts
0.40	2.199	1.801	Larger neutral-axis offset; longer bend allowance
0.45	2.278	1.722	Sensitivity case, not a material recommendation
0.50	2.356	1.644	Mid-thickness neutral-axis limit in the geometric model

This table shows mathematical sensitivity only. It does not assign K-factor values to aluminum, steel, or stainless steel. Production K-factor should come from a supplier-specific bend table or from test coupons formed with the intended material, grain direction, radius, die opening, punch, and method.

How to Determine K-Factor From a Trial Bend

A trial bend is the most defensible way to connect a CAD flat pattern with a specific process setup.

Record the coupon’s material grade and temper, thickness, rolling direction, punch and die, programmed angle, and forming method.
Measure the original flat length and the two finished straight flange lengths using a documented tangent or virtual-sharp convention.
Derive the measured bend allowance as BA = flat length - straight length 1 - straight length 2 when the straight lengths are measured to the bend tangency points.
Rearrange the bend allowance formula: K = {[(BA x 180) / (pi x A)] - R} / T.
Repeat the bend and measurement. Use the mean only if the samples and measurement method are stable.
Store the resulting value in a bend table tied to the exact material and tooling conditions.

If the flange measurements are taken to a virtual sharp instead of tangent points, derive BD first and convert it using BA = 2 x OSSB - BD. Mixing tangent and virtual-sharp measurements is a common source of incorrect K-factor results.

Bend Allowance, Bend Deduction, and K-Factor Compared

Term	What It Represents	Where It Is Used	Main Input Risk
Bend allowance	Neutral-axis arc length through the bend	Building the flat from tangent-length dimensions	Wrong K-factor or formed radius
Bend deduction	Amount removed from summed outside dimensions	Building the flat from outside flange dimensions	Ambiguous virtual-sharp measurement
K-factor	Neutral-axis offset divided by thickness	Calculating bend allowance	Treating a setup-dependent value as universal
Outside setback	Tangent-to-virtual-sharp distance	Converting between BA and BD	Using the wrong angle convention

Bend allowance and bend deduction are two routes to the same developed length when dimensions and conventions are consistent. Do not add bend allowance and subtract bend deduction in the same bend calculation.

Design Checks Before Releasing a Drawing

Specify material grade, alloy, temper, and nominal thickness rather than relying only on gauge; use the sheet metal gauge thickness chart when translating legacy gauge callouts.
Define the finished inside radius and bend angle, and state whether the angle is included angle or bend rotation.
Identify critical finished dimensions, datums, and whether dimensions apply before or after coating.
Confirm minimum flange support against the intended tooling; review the minimum flange length chart for early layout checks.
Check holes, slots, hardware, embosses, and cosmetic surfaces near the bend for distortion or tool contact.
Mark rolling direction where cracking, springback, or appearance makes orientation important.
Ask which bend table or K-factor the fabricator will use before sending a manufacturing flat pattern.
Keep the formed model as the design authority unless the fabricator explicitly requests a controlled flat pattern.

Why Calculated and Measured Values Differ

The formulas model the neutral-axis arc, but the actual bend comes from a material-tooling system. Air bending can produce a radius influenced by the die opening and material response; bottoming, coining, wipe forming, and hemming impose different contact conditions. Springback, thickness tolerance, tensile properties, grain direction, punch radius, die wear, lubrication, and measurement technique can all shift the finished geometry.

The error becomes visible as flange-length drift, hole-position error after forming, cumulative mismatch across multiple bends, or poor assembly fit. Tight finished dimensions therefore need a drawing-specific tolerance strategy rather than extra decimal places in a generic chart. Review broader process assumptions with the sheet metal tolerance chart.

What to Do When the Flat Pattern Does Not Match

Option	When It Helps	Trade-Off
Verify angle and dimension conventions	CAD and manual results disagree by a large amount	Requires redimensioning to a common basis
Measure the formed inside radius	The assumed radius came from the drawing, not the part	Radius measurement can be method-sensitive
Run material-and-tooling coupons	Repeat production justifies calibrated data	Adds setup and inspection work
Adjust the K-factor or bend table	Error is repeatable for one controlled setup	The correction may not transfer to another material or tool
Change the radius or die opening	Cracking, marking, or flange support is unacceptable	Changes BA, BD, springback, and possibly the finished design
Dimension the formed part and let the shop unfold it	Supplier controls cutting and bending	Requires clear agreement on design authority and revision control

For production parts, use sheet metal bending services to review the bend sequence, tooling access, radius, flange support, and flat-pattern assumptions together.

Frequently Asked Questions

Review these common questions for quick clarifications on core bending concepts, K-factor assumptions, and best practices for preparing sheet metal flat patterns for fabrication.

What is the difference between bend allowance and bend deduction?

Bend allowance is the neutral-axis arc length within the bend. Bend deduction is the amount subtracted from the sum of finished outside flange dimensions to obtain the flat length. Both describe the same bend from different dimensioning approaches.

What is the bend allowance formula for a 90 degree bend?

Using the angle convention on this page, BA = (pi / 2) x (R + K x T). You still need the formed inside radius, thickness, and a validated K-factor for the intended process.

How do I calculate bend deduction for a 90 degree bend?

For a right-angle bend, OSSB = R + T, so BD = 2 x (R + T) - BA. Subtract that value once from the sum of the two outside flange dimensions.

Is 0.33 the correct K-factor for all sheet metal?

No. 0.33 is the explicit example assumption used in this chart. K-factor can change with material condition, thickness, bend angle, radius, tooling, and forming method. Use measured or supplier-validated data for production.

Can I use bend deduction without knowing K-factor?

Yes, if a validated bend-deduction table directly matches the material, thickness, angle, radius, tooling, and process. If you calculate BD from geometry, K-factor enters through the bend allowance term.

Should I send a flat pattern to a sheet metal fabricator?

Send the formed 3D model and dimensioned drawing first. A flat pattern is useful when its compensation data has been agreed with the fabricator; otherwise, the shop may need to regenerate it using its own bend table.

Does bend allowance change with grain direction?

It can. Rolling direction can affect material response, cracking risk, springback, and the stable process settings, especially for direction-sensitive alloys or tight radii. Preserve coupon orientation when calibrating production data.

Need Help With Bend Allowance and Bend Deduction?

Send ShincoFab your formed CAD model and drawing, material grade and temper, thickness, quantity, finish, inside radius, flange lengths, bend sequence, critical tolerances, and application requirements for a part-specific DFM review. Contact ShincoFab to confirm the production bend data before finalizing the flat pattern.

Capabilities

Fabrication

Value-Added

3D Printing

Material

Products

Sheet Metal Parts

Thermal & Electrical

Sheet Metal Enclosure

Energy & Infrastructure

Industries

Resource

Why Choose Us