Sheet metal forming turns a flat blank into a finished part by plastically deforming the material past its yield strength without removing any mass. On a press brake, that means the flat pattern has to account for how the metal stretches around each bend, how far the part springs back when the ram retracts, and how tight a radius the chosen alloy will tolerate before it cracks. Get those three variables right on the print and a part runs clean the first time. Get them wrong and the shop discovers it at the brake, after the blank is already cut.
This guide covers the working numbers a designer needs to dimension a bent part: K-factor ranges and what drives them, the bend allowance and bend deduction math behind a correct flat pattern, minimum inside bend radius by alloy and thickness, springback by material, and the practical geometry rules (minimum flange, hole-to-bend distance, die selection) that decide whether a feature is formable at all. Every figure below is tied to a published source.
Bending Methods: Air Bending, Bottoming, and Coining
Nearly every flange on a precision part is produced by one of three press-brake methods. The method sets the achievable radius, the tonnage required, and how much the part springs back.
- Air bending presses the punch into the sheet only partway into the V-die, so the material never touches the bottom of the cavity. The inside radius is set by the die opening, not the punch tip, which is why one punch and one die can produce a range of angles and radii. It uses the least tonnage and is the dominant method in modern fabrication, but it has the most springback. (RapidDirect, Bend Radius Chart)
- Bottoming drives the sheet to the bottom of the V-die. The die angle controls the final angle, springback is small and repeatable, and the radius is tighter than air bending, at the cost of higher tonnage and a dedicated die per angle.
- Coining forces the punch tip into the material under very high tonnage (often several times that of bottoming), plastically setting the radius and nearly eliminating springback. It produces the most accurate, most repeatable radius but is reserved for cases that justify the tooling load. (The Fabricator, Springback and Springforward)
For air bending, a common shop rule is to size the V-die opening at roughly 8 times the material thickness, which in turn produces an inside radius near 16 percent of the die opening for mild steel. Wider die openings spread the bending stress over more material, which raises the formed radius and increases springback. As thickness goes up, both the die opening and the minimum usable flange length go up with it. (RapidDirect)
Punch stops partway into the V. Three contact points, most springback.
The inside radius follows the die opening (about 16 percent of it for mild steel), not the punch tip. Least tonnage, and one punch and die cover a range of angles and radii.
Sheet is driven to the bottom of the V. Small, repeatable springback.
The die angle controls the final angle, at a tighter radius than air bending gives. Costs more tonnage than air bending and needs a dedicated die per angle.
Punch tip is forced into the material. Springback nearly eliminated.
Very high tonnage, often several times that of bottoming, plastically sets the radius. The most accurate and repeatable bend, reserved for parts that justify the tooling load.
– – – marks the unloaded position after springback. For air bending, a common shop rule sizes the V opening at about 8 times material thickness.
Air bending, bottoming, and coining compared by punch penetration, die contact, and springback tendency; hover or tap a panel for detail.
The K-Factor: Why the Flat Pattern Is Not the Sum of the Flanges
When a sheet is bent, the inside surface compresses and the outside surface stretches. Somewhere between them is the neutral axis, a layer that neither stretches nor compresses. In the flat blank the neutral axis sits at the center of the material, 50 percent of the thickness. As the bend forms, the neutral axis shifts toward the inside surface. The K-factor is the ratio of that shifted location to the material thickness:
K-factor = t / T, where t is the distance from the inside surface to the neutral axis and T is the material thickness.
Because the neutral axis only ever moves inward from center, the K-factor is always 0.50 or less. In practice it falls between 0.3 and 0.5, with 0.33 a common starting value and 0.4468 cited as the average across most applications in Machinery's Handbook. The exact value is driven by the tightness of the bend relative to thickness (sharper inside radius shifts the neutral axis further inward, lowering K), the forming method, and the alloy. (The Fabricator, Analyzing the K-Factor; Firgelli, Bend Allowance Calculator)
| K-factor value | Where it applies | Source |
|---|---|---|
| 0.33 | Common default; tighter bends where inside radius is less than ~1x thickness | Firgelli / common shop practice |
| 0.3 – 0.5 | Working range for most materials and radii | Firgelli |
| ~0.4468 | Average value used for most bending applications | Machinery's Handbook (via The Fabricator) |
| Approaches 0.5 | Generous inside radii relative to thickness; neutral axis stays near center | The Fabricator |
Springback: expect 0.75 to 1.0 degree on a 90 degree air bend at 1:1 R:T. The shop overbends to compensate; springback grows with wider die openings and larger R:T.
Set thickness, inside radius, bend angle, and alloy to see the neutral axis shift and the flat-pattern numbers update, using the K-factor, minimum-radius, and springback ranges cited in this article.
Bend Allowance, Bend Deduction, and the Flat Pattern
The K-factor exists to feed two calculations that produce a correct flat blank length. Cut the blank to the simple sum of the flange dimensions and the finished part will be oversized, because the metal elongates as it wraps the bend.
Bend Allowance (BA) is the arc length of the neutral axis through the bend. It is the amount of material consumed by the bend:
BA = (π / 180) × (R + K × T) × A
where R is the inside bend radius, K is the K-factor, T is the material thickness, and A is the bend angle in degrees. (ArcCaptain, Bend Allowance Formula; Firgelli)
Outside Setback (OSSB) is the distance from the bend tangent line to the apex where the two outside flange faces would intersect:
OSSB = tan(A / 2) × (R + T)
Bend Deduction (BD) is the amount subtracted from the sum of the outside flange dimensions to get the flat length:
BD = 2 × OSSB − BA
Flat length then equals the sum of the outside dimensions minus the bend deduction for each bend. (Firgelli, Bend Deduction) The practical takeaway for a designer: dimension the print to the feature that matters (inside, outside, or hole-to-edge), specify the inside radius explicitly, and let the shop compute the flat from a K-factor verified for the actual tooling.
Minimum Inside Bend Radius by Material and Thickness
The single most common drawing error is calling out an inside radius tighter than the alloy can take. A bend made too sharp pushes the outside fibers past their elongation limit and cracks. The minimum bend radius is a property of the material and its temper, not of the sharpest punch on the rack. (The Fabricator)
Minimum radius is usually expressed as a multiple of thickness, written "T." The table below is a baseline for standard air bending. Temper matters as much as alloy: soft 5052-H32 aluminum follows roughly a 1T rule, while harder 6061-T6 is prone to cracking and typically needs 3T to 6T unless the bend zone is locally annealed first.
| Material | 1–6 mm thick | 6–12 mm thick | 12–25 mm thick |
|---|---|---|---|
| Aluminum (general) | 1.0 × T | 1.5 × T | 2 – 3 × T |
| Mild / cold-rolled steel | 0.8 × T | 1.2 × T | 1.5 – 2.5 × T |
| Stainless steel (304) | 2.0 × T | 2.5 × T | 3 – 4 × T |
| Alloy / temper | Formability and radius behavior |
|---|---|
| 5052-H32 aluminum | Excellent formability, generally follows a ~1T rule |
| 6061-T6 aluminum | Prone to cracking; typically 3T – 6T, or locally anneal the bend zone for tighter radii |
| 304 stainless steel (annealed) | ~1T to 2T minimum; work-hardens and springs back significantly, so overbending is required |
| C110 copper / C260 brass (soft) | 0T to 1T; can sometimes be bent flat on itself; half-hard tempers need roughly double the soft-state radius |
When supplier data is not on hand, there is a documented rule of thumb for the minimum inside bend radius of steel (and it generally works for aluminum): divide 50 by the material's tensile reduction percentage, subtract 1, and multiply by thickness. For a steel with 10 percent tensile reduction: (50 / 10) − 1 = 4, so the minimum inside radius is about 4 × T. This is a screening number, not a substitute for mill data or a test bend. (The Fabricator, Bending Basics: Heavy Bending)
Springback: Designing for the Angle You Actually Get
When the ram retracts, the elastic portion of the strain releases and the bend opens up slightly. That recovery is springback, and it is governed mostly by yield strength: the higher the yield strength, the more the part springs back. Springback also grows as the inside radius grows relative to thickness, and as the die opening widens in air forming. (The Fabricator, Springback and Springforward)
For a 90-degree air bend with a roughly 1-to-1 ratio of inside radius to thickness, expect approximately:
| Material | Typical springback at 1:1 radius-to-thickness |
|---|---|
| 304 stainless steel | 2 to 3 degrees |
| Mild aluminum | 1.5 to 2 degrees |
| Cold-rolled steel | 0.75 to 1.0 degree |
| Hot-rolled steel | 0.5 to 1.0 degree |
| Copper and brass | 0.0 to 0.5 degree |
The shop compensates by overbending: forming to a sharper beginning angle so the part springs back to the target. The springback factor (Sf) relates the two angles, Sf = bending angle / bent angle. A 90-degree bend that relaxes to 88 degrees has Sf = 90 / 88 = 1.022. The same factor applies to the radius, which also opens slightly after forming, so the actual radius equals Sf times the formed radius. For profound-radius bends and high-strength steels, springback can exceed 40 degrees, which is why HSS parts need generous radii and heavy overbend allowances designed in from the start. (The Fabricator)
Geometry Rules That Decide Whether a Feature Is Formable
A few proximity rules govern whether features survive forming. They come from a single physical constraint: material inside the bend deformation zone distorts, so holes, slots, and short flanges placed inside that zone pull oval, tear, or fail to form.
- Minimum flange length. A flange has to be long enough to span the die opening or it slips into the V and never forms cleanly. Minimum flange grows with thickness because thicker stock needs a wider die. As a representative figure, 16 GA (0.051 in.) 5052-H32 aluminum carries a minimum flange around 0.20 in., rising to roughly 0.375 in. at 11 GA (0.091 in.). (RapidDirect)
- Hole-to-bend distance. Keep holes outside the bend deformation zone. A widely used guideline is to hold a hole edge at least 2.5 times material thickness plus the bend radius away from the bend tangent line. Closer than that and the hole deforms during forming.
- Single radius across the part. Designing every flange to the same inside radius lets the operator form the whole part on one punch-and-die setup instead of changing tooling between bends, which lowers cost and improves repeatability. (RapidDirect)
- Bend relief. Where a bend ends at the edge of a flange, a small relief notch prevents tearing at the corner.
Tonnage and Material Differences at the Brake
Forming force scales with yield strength, thickness, and bend length, and inversely with die opening. As a quick relative baseline against mild steel of the same thickness, aluminum takes roughly half the bending force, while stainless steel takes about 1.5 times the force. (RapidDirect) Stainless also work-hardens during forming, which is why it both springs back more and demands more tonnage and harder, polished tooling than the same gauge of mild steel.
Material Selection for Formed Parts
Material choice for a formed part balances formability, strength-to-weight, corrosion resistance, weldability, and cost. The forming-specific tradeoffs:
- Aluminum (5052, 6061). Light and corrosion-resistant. 5052 forms readily at tight radii; 6061-T6 trades formability for higher strength and needs generous radii or local annealing at the bend.
- Cold-rolled and mild steel. The most forgiving at the brake: low springback, tight achievable radii, and lower tonnage than stainless. Requires a finish or coating for corrosion resistance.
- Stainless steel (304, 316). Strong and corrosion-resistant, but work-hardens, springs back 2 to 3 degrees at a 1:1 radius, and needs about 1.5 times the tonnage of mild steel. Design in larger radii and overbend allowances.
For deeper alloy-by-alloy property and specification data, consult mill data sheets and the relevant ASTM specifications (for example, ASTM A1008 for cold-rolled carbon steel sheet, ASTM A240 for stainless steel sheet and plate, and ASTM B209 for aluminum sheet and plate), alongside the ASM Metals Handbook volume on forming and forging.
Other Forming Operations Beyond the Press Brake
Bending on a press brake is the workhorse, but several other operations shape sheet metal for specific geometries.
Punching
Punching shears holes and shapes through the sheet using a punch and die. It is fast and well suited to high-volume hole patterns. The cut edge shows a characteristic profile: a rounded rollover and burnished band where the punch enters, and a fracture zone and burr on the die side. A general guideline is to keep the smallest punched hole diameter at or above the material thickness; smaller holes risk punch breakage and excessive edge deformation. Punch-to-die clearance, tooling sharpness, and alignment control edge quality. Atlas runs punching machines with a linear tool changer (not a turret) rated to 25 tons, holding ±0.004 in. positioning accuracy and ±0.001 in. repeatability.
Roll Forming
Roll forming passes the strip through successive pairs of contoured rolls, each adding a small increment of bend, to produce a continuous engineered profile. It suits long, constant-cross-section parts run in volume.
Hydroforming
Hydroforming uses high-pressure fluid to press sheet (or tube) against a single die, distributing pressure evenly across the blank. It produces smooth, complex contours and a high strength-to-weight ratio with one die instead of a matched set, which is why it is common for automotive and aerospace structural parts. Setup and equipment costs are higher, so it favors complex geometries over simple bends.
Curling and Hemming
Curling rolls the edge of a sheet into a hollow ring to remove the sharp edge and stiffen the rim. Hemming folds the edge back flat on itself for the same reasons. Both improve edge safety and rigidity, and both depend on the same minimum-radius and springback behavior described above.
Deep Drawing and Ironing
Deep drawing pulls a blank into a die cavity to form a cup or box shape. Ironing then forces the drawn part through a tight die gap to even out the wall thickness, the operation behind aluminum cans and similar near-net-shape parts.
Custom Forming Tools: 3D-Printed Tooling at Atlas
Not every formed feature has an off-the-shelf die. For low-to-medium volume parts with unusual geometry, additively manufactured forming tools cut the lead time and tooling cost of conventional steel tooling. The gallery below shows a custom 3D-printed forming tool produced at Atlas Manufacturing for a bent and embossed part.
Forming at Atlas Manufacturing
Atlas Manufacturing runs precision sheet-metal forming out of facilities in Minneapolis, Minnesota and Chippewa Falls, Wisconsin, serving engineers and procurement teams across telecom, medical device, industrial, and OEM markets. The shop pairs CNC press brakes and panel benders with robotic bending for repeatable, high-mix work, and supports forming with laser cutting on 4 kW and 6 kW Bystronic machines (part dimensional tolerance ±0.005 to ±0.010 in.), 25-ton linear-tool-changer punching, welding, powder coating, hardware insertion, and assembly under one roof.
The practical value to a design team is catching the formability problems above before the blank is cut: confirming the inside radius is achievable for the chosen alloy and temper, setting flat patterns from a K-factor verified against the actual tooling, and designing in the right overbend for springback. Send a print and the forming group will flag the radius, flange, and hole-to-bend issues up front rather than at the brake.
Frequently Asked Questions
What is forming in sheet metal?
Sheet metal forming is the process of plastically deforming a flat blank into a desired shape without cutting or removing material. Force is applied to push the sheet past its yield strength so it takes a permanent set rather than springing back to flat.
What is a typical K-factor for sheet metal bending?
The K-factor is the ratio of the shifted neutral axis location to material thickness. It falls between 0.3 and 0.5, with 0.33 a common default and about 0.4468 cited as the average for most applications in Machinery's Handbook. Sharper bends relative to thickness lower the K-factor; the value should be confirmed against test bends for the actual alloy and tooling.
What is the minimum bend radius for sheet metal?
Minimum inside bend radius depends on the alloy and temper, not the punch. As a baseline for air bending, mild steel runs about 0.8T, general aluminum about 1T, and 304 stainless about 2T for thin gauges, where T is material thickness. Harder tempers like 6061-T6 need 3T to 6T. Always confirm against mill data or a test bend.
How much does sheet metal spring back when bent?
At a 1-to-1 inside-radius-to-thickness ratio on a 90-degree air bend, expect roughly 2 to 3 degrees for 304 stainless, 1.5 to 2 degrees for mild aluminum, 0.75 to 1 degree for cold-rolled steel, and near zero for soft copper and brass. Higher yield strength, larger radii, and wider die openings all increase springback.
How do you calculate bend allowance and bend deduction?
Bend allowance is the neutral-axis arc length: BA = (pi/180) x (R + K x T) x A, where R is inside radius, K is the K-factor, T is thickness, and A is the bend angle. Outside setback is OSSB = tan(A/2) x (R + T). Bend deduction is BD = 2 x OSSB - BA, and is subtracted from the sum of outside dimensions to get the flat length.
