Press Brake Forming
Also: press brake bending, sheet metal bending, air bending, bottom bending, coining, brake forming, CNC bending, brake press
Press brake forming bends sheet and plate between a punch and a V-die; bend radius, tonnage and springback follow from the die opening and the material.
1,699 sheet metal fabrication companies in the Noramark directory
A press brake holds a long punch in a ram and a V-die on the bed; the sheet is pushed into the die to form a bend along a straight line. Nearly all job-shop work is air bending: the punch drives the sheet only part way into the V, and the angle is set by ram depth, so one punch and die make any angle. The inside radius is not the punch tip but roughly one sixth to one eighth of the die opening, which is why shops bend 1.5 mm (0.060") steel over a 12 mm (0.5") V and get a radius near the thickness. Bottoming and coining force the sheet fully into the die for a fixed radius and less springback, at several times the tonnage.
Tonnage scales with thickness squared and inversely with the die opening. For 60 ksi mild steel the rule of thumb is about 575 x t² / V tons per foot with t and V in inches: 1.5 mm (0.060") steel over a 12 mm (0.5") V needs about 4 tons per foot (12 t/m). Stainless needs roughly 1.5 times that, 5052 aluminum about half. Springback runs 0.5-2° for mild steel, 2-4° for stainless and hard aluminum, and more for high-strength steel; the operator overbends to compensate, and a CNC brake with angle measurement corrects it per hit.
The flat pattern is developed with a K-factor (the position of the neutral axis, 0.33-0.5 of the thickness, typically 0.42-0.45 for air-bent mild steel at a 1t radius) or the bend deduction the shop has measured on its own tooling. This is why shops prefer a 3D model with bends over a customer flat pattern: the flat only comes out right with the tooling it was developed for.
At a glance
| Typical tolerances | Bend angle ±1° standard, ±0.5° with care (angle-measuring brake, crowning, consistent material lot). Flange length ±0.25 mm (±0.010") standard, ±0.13 mm (±0.005") with care, per bend; tolerances stack across bends. Inside radius ±0.25 mm (±0.010") in air bending, since it follows the die and the material. Mill thickness variation shifts both the radius and the flange length. |
|---|---|
| Size limits | Job-shop brakes run 1.2-6 m (4-20 ft) beds at 40-1,000 tons; 3 m (10 ft) at 100-200 tons is the typical machine. Thickness 0.5-25 mm (0.020-1") and beyond, though above 6 mm (0.25") the work is plate forming with large radii. Minimum flange length is about half the die opening plus the radius, roughly 4t. Box depth is limited by the punch height and the ram clearance, about 150-300 mm (6-12") with standard tooling. |
| Surface finish | The V-die shoulders leave witness marks on the outside of the bend, more visible on soft aluminum and polished stainless; urethane pads, polished radius dies and protective film reduce them. Tight radii show orange peel on the outside of the bend. The inside of the bend is untouched. Finishing is whatever the part gets afterwards: powder coat hides die marks, anodize does not. |
| Lead time | Prototypes in 3-7 business days once the flats are cut; production in 1-3 weeks. Special tooling (large radius, hemming, gooseneck) adds 1-3 weeks if not on the shelf. |
Typical of U.S. job shops; confirm with the shop for your part.
Materials
Mild steel (CRS, HRPO, galvanized) bends best. 5052-H32 is the aluminum of choice; 6061-T6 needs a 1.5-2.5t radius and cracks below that, so tight bends in 6061 are done in the O or T4 temper and aged afterwards. 5083 bends at 2-3t. Stainless 304 and 316 bend well but spring back more and need more tonnage; A572 Grade 50 and other high-strength plate need larger radii and larger dies. Copper and half-hard brass form easily. Grade 2 titanium bends cold at 2.5-3t radius; Ti-6Al-4V is hot formed. 7075-T6, spring-temper 1095 and hardened steels are not bent on a brake.
What drives the cost
- Number of bends per part: each is a hit and, for different angles or radii, a tool change
- Special tooling: large radii, hems, offsets, goosenecks and box-forming punches
- Tolerances tighter than ±1° and ±0.25 mm (±0.010") that need angle measurement and test bends
- Material: stainless and high-strength steel need larger dies, more tonnage and more overbend
- Cosmetic requirements: no die marks means film, urethane tooling and slower handling
- Quantity: setup dominates singles; hundreds run at seconds per bend
When to use it
- Any straight bend in sheet or plate, from one piece to tens of thousands
- Brackets, channels, enclosures, boxes and pans with flanges
- Parts whose bend radius and angle can live with ±1° and ±0.25 mm (±0.010")
- Hemmed edges and offsets that stiffen sheet without adding thickness
When not to
- Curved bends or compound curves: roll bending, deep drawing or stamping
- Hundreds of thousands of a small part: a progressive die forms it in one stroke
- Long runs of one profile: roll forming is faster and straighter per foot
- Materials that crack cold: 7075-T6, hardened steel, thick titanium alloys
- Bends deeper than the tooling can reach, such as a tall narrow box
Design tips
- Use an inside radius equal to the thickness (1t) for steel and 5052; 1.5-2.5t for 6061-T6 and stainless at heavy gauges.
- Keep one radius and, where possible, one thickness per part so the whole job runs on one punch and die.
- Make flanges at least 4t long and keep holes 2t plus the radius from the bend line, or slot them.
- Orient tight bends across the grain (perpendicular to the rolling direction) where the drawing lets you.
- Model the bends in 3D and let the shop develop the flat with its own K-factor; if you supply a flat, say what K-factor and radius it assumes.
- Dimension bent parts to the outside mold line or to a face the inspector can touch, not to a bend tangent line.
- Add bend relief at least 1t wide and 1t past the bend line where a bend ends inside the blank.
- Check that a tall box or a return flange leaves room for the punch and ram; a quick call to the shop saves a redesign.
Press Brake Forming by material
Frequently asked questions
- What is the K-factor for sheet metal bending?
- The K-factor is the position of the neutral axis as a fraction of the thickness, between 0.33 and 0.5. Air-bent mild steel at a 1t radius runs about 0.42-0.45; harder materials and tighter radii push it lower. Every shop measures its own with its tooling, which is why a customer flat pattern often comes out a little long or short.
- How much tonnage does a press brake need?
- For mild steel in air bending, about 575 x t² / V tons per foot of bend, with thickness t and die opening V in inches. 3 mm (0.120") steel over a 25 mm (1") V takes about 8 tons per foot, so a 3 m (10 ft) bend needs an 80-ton brake. Stainless needs about 1.5 times that, 5052 aluminum about half, and bottoming or coining several times more.
- What is springback in bending?
- When the punch lifts, the elastic part of the bend recovers and the angle opens: 0.5-2° for mild steel, 2-4° for stainless and hard aluminum, more for high-strength steel and large radii. The brake overbends to compensate, and angle-measuring brakes correct each hit.
- Can 6061-T6 aluminum be bent?
- Yes, with an inside radius of 1.5-2.5 times the thickness and some orange peel on the outside of the bend. For tighter radii, bend in the O or T4 temper and age to T6 afterwards, or switch to 5052-H32, which bends at 1t.
- What is the difference between air bending and bottoming?
- Air bending presses the sheet part way into the V, so the angle comes from ram depth and one tool set makes any angle; it uses the least tonnage and has the most springback. Bottoming pushes the sheet fully into the die for a fixed angle and radius with less springback at three to five times the tonnage; coining goes further and stamps the radius into the sheet.
