Quick answer
Choosing a sheet metal bend radius starts with the material grade and condition, thickness, tooling, and finished-part requirements. Specify the inside radius and critical formed dimensions on the drawing. Calculate the flat blank using bend allowance or bend deduction based on a bend table or K-factor appropriate to the actual process, then check the result with a trial bend.
Checking a formed corner: evaluate the specified radius and angle on the actual part, not just the CAD flat.
In this guide
01What Is the Inside Sheet Metal Bend Radius?
02How Do You Choose a Bend Radius for Sheet Metal?
03Bend Allowance, Bend Deduction, and K-Factor
04Worked Example: A 90° Bend
05Common Drawing Mistakes—and Better Callouts
06Five Checks Before Releasing a Bent-Part Drawing
07Frequently Asked Questions
08References
What Is the Inside Sheet Metal Bend Radius?
You measure the inside bend radius, R, on the concave, inner surface of a formed bend. The nominal sheet thickness is t; use the appropriate actual stock thickness when calibrating the process. The outside radius is approximately R + t if thickness remains approximately uniform through the bend. In the equations below, θ is the amount of material turned from flat, in degrees: a right-angle bend is 90°. However, the included opening angle between the finished legs is 180° − θ. At 90°, both angles happen to have the same value.
During bending, the inside compresses and the outside stretches. A neutral region lies between them. In a simplified model, K × t locates the neutral axis from the inside surface. K-factor is a flat-pattern model input, not a universal material property.
Why formed dimensions matter: An unfolding rule calculates the flat pattern. If its K-factor or bend table does not match the actual material and tooling, the finished flanges may miss assembly dimensions. Therefore, state critical formed dimensions and datums explicitly, and clarify whether a supplied flat is contractual or for reference. Do not silently treat an unverified flat and formed drawing as independently governing when they disagree.
How Do You Choose a Bend Radius for Sheet Metal?
Check the following before specifying a radius:
- Material and condition: alloy, temper or hardness, and grain direction can affect formability. Do not transfer a setting from one material to another without checking.
- Actual thickness: confirm the stock specification and actual sheet-thickness considerations.
- Tooling and method: punch, die opening, and forming method can affect the radius produced. Confirm the available tooling rather than assuming CAD defines the actual radius.
- Geometry and sequence: short flanges, nearby holes, and previously bent walls can interfere with tools or backgauges.
- Function: specify critical mating dimensions and visible surfaces so you can check them on the formed part.
A tighter radius can increase cracking risk; a larger radius changes flange geometry and the calculated blank. See common causes of cracking during sheet metal bending for the separate failure-analysis discussion.
What is a minimum bend radius?
The minimum bend radius is the smallest inside radius that the material and process can hold without cracking or unacceptable thinning under the specified material and process conditions. Grade, temper, thickness, bend-line orientation, and tooling all matter. Consult material data and qualified process records for a starting point, then confirm critical bends with the intended material and setup.
Material condition, rolling direction, and surface quality
Two sheets bearing a similar broad material name can behave differently. Specify the actual grade and temper/condition rather than assuming, for example, that all aluminum bends like 5052-H32 or 6061-T6. For a tight or crack-sensitive bend, ask the fabricator whether to control the bend-line orientation relative to rolling direction on the blank. The outer surface of the bend is in tension, so direction and condition can affect cracking risk. Do not publish a universal minimum-radius multiplier for a material without a qualified source and process.
If a flange is cosmetic, identify the visible face and acceptable marking. In addition, discuss tool contact and surface protection along with the bend sequence; a finish applied after forming can also affect fit or appearance. These are project decisions, not a promise that every tool and finish combination is available.
Tooling, bend sequence, and springback
In air bending, the formed inside radius depends on the material, thickness, die opening, and punch/die combination. However, it does not necessarily match the punch-tip radius or the value drawn in CAD. Check short-flange support and tool clearance against the actual part and selected tooling rather than relying on a universal minimum.
| Sheet thickness t | Typical die opening V ≈ 6t | Air-bend inside radius ≈ V/6 | Minimum supported flange ≈ V/2 + t |
|---|
| 0.8 mm | 5 mm | ≈ 0.8 mm | ≈ 3.3 mm |
| 1.0 mm | 6 mm | ≈ 1.0 mm | ≈ 4.0 mm |
| 1.5 mm | 9 mm | ≈ 1.5 mm | ≈ 6.0 mm (6.3 mm in our shop practice) |
| 2.0 mm | 12 mm | ≈ 2.0 mm | ≈ 8.0 mm |
| 3.0 mm | 18 mm | ≈ 3.0 mm | ≈ 12.0 mm |
Typical starting values — confirm with a trial bend on the actual material and tooling.
Springback can change the released angle. A trial bend helps establish any angle correction needed for the specific material and setup.
Forming a perforated component at the press brake. Check hole-to-bend clearance, flange support, and bend sequence together for the specific part.
Check whether a short flange has adequate support on the selected die and whether a previously formed wall collides with the punch, die, or backgauge. For example, in some parts the preferred order is to form obstructed internal features before closing larger outer walls; therefore, check the actual sequence against the specific geometry. A larger specified radius also changes tangent points, clearances, and the flat pattern: it is not a free cure for cracking.
What about minimum flange length and holes near a bend?
There is no universal flange-height or hole-to-bend rule for every tool and part. A short flange needs adequate support in the die, while a hole crossing the deformation zone may distort. Show the measurement datum and important features on the drawing. Our sheet metal drawing and DFM checklist helps collect these details.
Bend Allowance, Bend Deduction, and K-Factor
Bend allowance (BA) estimates the neutral-axis length of the bent region. Outside setback (OSSB) relates the theoretical outside apex to each tangent point. You subtract bend deduction (BD) from the sum of the outside-apex leg dimensions to estimate the blank length. They are related, but not interchangeable.
| Parameter | Symbol | Meaning | Role in the flat pattern |
|---|
| Inside bend radius | R | Radius on the inner surface | Sets the modeled inner bend geometry |
| K-factor | K | Neutral-axis offset divided by thickness | Locates the modeled neutral-axis radius, R + K × t |
| Bend allowance | BA | Modeled neutral-axis arc length through the bend | Added to tangent-to-tangent straight lengths |
| Outside setback | OSSB | Distance from the outside virtual apex to a bend tangent point | Relates outside-apex legs to the bend zone |
| Bend deduction | BD | 2 × OSSB − BA for the stated convention | Subtracted from the sum of outside-apex legs |
The K-factor expresses the neutral-axis offset from the inside surface as a fraction of thickness: K = neutral-axis offset / t. The modeled neutral-axis bend radius is therefore R + K × t. A CAD application’s default K-factor is a starting assumption, not proof that a particular shop’s formed part will match the flat. Use bend data qualified for the chosen material, thickness, angle, and tooling when the finished dimensions matter.
| Inside radius relative to thickness (R/t) | Typical K-factor used as a starting value (air bending) |
|---|
| ≈ 0.5 (near-sharp bend) | ≈ 0.33 |
| ≈ 1.0 | 0.40–0.45 |
| ≈ 2.0 | 0.45–0.48 |
| ≥ 3.0 | approaches 0.50 |
Typical published ranges for air bending — verify with your own bend data before releasing a drawing.
For a uniform bend, with θ defined as the bend angle in degrees:
BA = (π × θ / 180) × (R + K × t)
OSSB = (R + t) × tan(θ / 2)
BD = 2 × OSSB − BA
Flat length for one bend = outside leg A + outside leg B − BD
Use one angle convention and one system of units throughout. Inside-face lengths, tangent-to-tangent lengths, and outside-apex lengths do not fit the final equation directly; you must convert them first. With multiple bends, account for each bend and then inspect the finished part against functional datums. A calibrated bend table can incorporate measured results for specific thicknesses, radii, and angles rather than applying one linear K-factor everywhere. Our precision sheet metal tolerances primer provides related drawing context.
Worked Example: A 90° Bend
Hypothetical inputs, not production settings: thickness t = 2.0 mm; inside radius R = 2.0 mm; bend angle θ = 90°; assumed K = 0.42 for this calculation only. The finished part has two outside-apex leg dimensions of 30.0 mm and 40.0 mm.
First locate the modeled neutral axis: K × t = 0.42 × 2.0 = 0.84 mm from the inside surface, giving a neutral-axis radius of R + K × t = 2.84 mm. Convert the bend angle to radians: 90 × π / 180 = π / 2. Now calculate:
BA = (π × 90 / 180) × (2.0 + 0.42 × 2.0) ≈ 4.461 mm
OSSB = (2.0 + 2.0) × tan(45°) = 4.000 mm
BD = 2 × 4.000 − 4.461 ≈ 3.539 mm
Estimated flat length = 30.0 + 40.0 − 3.539 ≈ 66.461 mm
This is therefore a calculated starting blank, not a guaranteed formed dimension or a qualified bend setting. Measure a trial bend under the selected material and tooling conditions; update the bend table or K-factor if the result differs. Do not reuse the example’s 0.42 for every material, thickness, tool, and angle.
Check the result on a formed trial part
Record the material and tooling used for the trial, then check the released angle, inside radius, and the formed dimensions that matter to assembly. A protractor can check angle; a radius gauge can help compare the corner profile. Check the measured dimensions against the drawing requirements. If the measured result differs from the CAD prediction, revise the applicable bend data before approving a production flat.
Examples of dimensional inspection equipment. For a trial bend, check the released angle, inside radius, and critical dimensions on the formed part against its drawing.
Before using this method: Are both leg dimensions measured to the outside virtual sharp corner rather than to the inside faces or tangent points? Does θ mean the bend angle rather than the open angle? Are all lengths in millimeters? Was K derived from a qualified bend table, a trial bend, or an untested CAD default? A plausible numerical result is not enough if the dimension references are wrong.
Want a second pair of eyes?
Share the formed drawing so we can discuss its radius, flange, and flat-pattern requirements for your RFQ.
Get a bend DFM review ↗
Common Drawing Mistakes—and Better Callouts
No inside radius specified. The manufacturing team may choose a radius based on its available tooling. If the radius affects mating clearance, strength, or appearance, call it out explicitly. For other bends, agree a project-specific default radius with the fabricator; do not assume R = t will work for all materials or tooling.
A supplied flat conflicts with the formed drawing. Different unfolding rules may generate different blank lengths for the same modeled geometry. Identify the governing formed dimensions and tolerances, state the status of the flat pattern, and resolve conflicts before production rather than asking both drawings to govern independently.
Holes or slots intersect the bend zone. Holes can elongate or move relative to critical features as the bend forms. Dimension their location in the finished part and ask for a DFM review of the die opening, radius, and hole-to-bend relationship. If necessary, consider a validated change to feature placement or a secondary operation; do not prescribe a universal 2.5t + R clearance or promise post-bend machining for every part.
One K-factor is used for every material. The flat may be consistently wrong even when every arithmetic step is correct. Therefore, record the source of the unfolding rule and validate it against the actual material, thickness, radius, tooling, and measured bend result.
Five Checks Before Releasing a Bent-Part Drawing
- Identify material and condition. Include grade, temper/condition if relevant, and thickness.
- Define the bend. Indicate the inside radius and bend angle, clarify the angle convention, and identify visually critical surfaces.
- Prioritize formed dimensions. Highlight dimensions and datums important to assembly rather than treating an unverified flat as the sole authority.
- Review nearby features. Check holes, slots, short flanges, rolling direction where relevant, bend sequence, and tool clearance. See the hinge and radius-bend validation example.
- Validate the blank. If you provide a DXF or CAD flat, identify its bend-table assumptions. Discuss feasible tools and the sequence with the team responsible for CNC bending.
Frequently Asked Questions
Is an inside bend radius equal to the sheet thickness?
In practice, that may be a convenient initial drawing assumption for some designs, but it is not a universal minimum or a promise of the radius a tool will produce. Check the material condition, process, and finished-part requirements.
Does the punch-tip radius determine the formed inside radius?
Not by itself in air bending. The actual radius depends on the material and selected punch/die setup. For a radius that is critical to fit or performance, specify the acceptance requirement and ask whether the proposed tooling and forming method can achieve it.
How do you calculate the bend radius of sheet metal?
If you know the bend allowance, bend angle, thickness, and a process-appropriate K-factor, rearrange the bend-allowance formula: R = BA / θ(rad) − K × t. For the worked example above (BA 4.461 mm, 90° bend, t = 2.0 mm, K = 0.42), R = 4.461 / 1.5708 − 0.84 = 2.00 mm. In real production, confirm the formed radius by measurement and tune the flat-pattern rule to the actual bend rather than calculating a nominal radius in isolation.
Are bend allowance and bend deduction the same?
No. Bend allowance estimates the neutral-axis length through the bend; bend deduction converts the sum of two outside-apex leg dimensions into a flat length under the stated convention.
Can the same K-factor be used for every part?
No. It is a modeling assumption until checked against the relevant material, thickness, tooling, bend angle, and process. Keep qualified bend data when repeatability matters.
Why can a bend crack even when its flat pattern is correct?
Flat-pattern accuracy and material formability are different checks. Material condition, grain direction, radius, and tooling can contribute to cracking. Therefore, investigate the crack and test the intended setup rather than changing the flat pattern alone.
Should I send a formed drawing or a flat pattern?
Send the formed drawing with critical dimensions and datums. Include the CAD model and flat pattern when available, but identify the assumptions behind the flat. The manufacturer can then review the blank against the intended process.
References
- DIN 6935 — Cold bending of flat rolled steel products; determination of the unfolded (developed) length.
- ISO 7438 — Metallic materials; bend test.
- ASM Handbook, Volume 14B: Metalworking — Sheet Forming, ASM International.
Request a Bend DFM Review
Share your formed drawing, material grade and condition, thickness, bend radii, bend angles, critical assembly dimensions, relevant rolling-direction or finish requirements, expected quantity, and any existing flat pattern. Include the model or DXF if available and flag dimensions that require special attention. We can discuss project-specific manufacturability and quotation requirements; do not assume every requested radius or tolerance is feasible before review. .
Submit your drawing for an RFQ
Sheet Metal Bend Radius Guide: Choosing an Inside Radius and Calculating Bend Allowance
