Press Braking
Press braking bends sheet metal by driving a punch into a V-die, forming one straight-line bend at a time.
- Part
- Forming
- Revised
- 2026-08-11
At a glance
- Family
- Metal
- Typical tolerances
- ±0.010 in (±0.25 mm) on a single bend dimension, accumulating roughly ±0.010 in per additional bend; bend angle ±1°, or ±0.5° with in-process angle measurement
- Surface finish
- Inherits the incoming sheet finish; die shoulder marks on the outside of the bend are normal unless urethane or film-protected tooling is specified
- Typical volumes
- 1–25,000 parts; above about 25,000 identical parts, hard tooling usually wins
- Lead time
- 1–10 business days in a job shop; same-day for simple parts with material in stock. No tooling lead time
- Materials
- Metal
What it is
Press braking bends sheet metal by driving a punch into a V-shaped die, forming one straight-line bend per stroke. It is the universal sheet metal forming process: no part-specific tooling, a few standard punches and dies covering thousands of part numbers, and a CNC backgauge that positions the blank for each bend in sequence.
Typical work is enclosures, chassis, brackets, panels, and channels in 0.024–0.250 in (0.6–6 mm) steel, stainless, and aluminum, at anything from one piece to tens of thousands. Because the tooling is generic, cost per part is machine time and setup, which makes press braking the natural partner to laser cutting in job-shop fabrication.
The number to design around is the inside bend radius, which in air bending is not set by the punch but by the die opening — roughly 16% of the V-width for mild steel. Get that wrong and the flat pattern is wrong.
How it works
Air bending, bottoming, or coining?
Air bending stops the punch short of the die bottom, so the sheet touches at just three points and the bend angle is a function of ram depth. One die opening covers a range of angles and thicknesses, and tonnage is lowest. This is the default.
Bottoming presses the sheet fully into the V, so the die angle sets the part angle. It needs roughly three to five times the air-bend force, but springback is smaller and repeatability better.
Coining drives the punch nose into the material, plastically deforming through the full thickness. It eliminates springback almost entirely and needs on the order of five to ten times air-bend force, so it is reserved for small, precise bends.
The cycle
- Tool up. Punch and die are loaded and the die opening chosen — the standard starting point is a V-width of about 8× material thickness.
- Program. The CNC computes ram depth per bend from thickness, tooling, and target angle, and sets the backgauge positions for the bend sequence.
- Position. The operator or robot slides the blank against the backgauge fingers.
- Bend. The ram descends. Force for air bending mild steel follows the standard relation of roughly 575 × t² ÷ V tons per foot, with thickness t and die opening V in inches; stainless runs about 50% higher and aluminum roughly half.
- Springback. The part relaxes elastically when the ram lifts — about 1–3° for mild steel, more for stainless, aluminum, and high-strength grades. The CNC overbends to compensate, and in-process angle measurement systems close the loop automatically.
- Sequence. Bends are made in an order that never traps the part inside its own geometry. This is the real skill of press braking, and the reason bend sequence should be checked at design time.
Bend sequence and tool access explain most of the parts a fabricator says cannot be made: the geometry is fine, but the formed flange collides with the ram before the last bend can be reached.
Design guidelines
Inside bend radius
Use an inside radius of at least 1× material thickness for mild steel and annealed aluminum. Harder tempers need more: 6061-T6 commonly needs 2–4× thickness across the grain and more parallel to it. In air bending, the achieved radius follows the die opening — approximately 16% of the V-width — not the punch tip, so a sharp punch in a wide die still produces a large radius.
One radius throughout
Keep every bend on the part at the same inside radius if you can. Each different radius is another tool change and another setup, and setup is most of the cost on short runs.
Minimum flange length
A flange must be long enough to sit on both shoulders of the V-die: figure roughly 4× material thickness as a working minimum, or half the die opening plus the thickness. Shorter flanges slip into the die and form inconsistently, requiring special tooling.
Hole and feature distance from a bend
Hold holes at least 2.5× material thickness plus the bend radius from the bend line. Closer holes distort. If the hole must be closer, either pierce it after bending or extend it into a slot that crosses the bend line entirely.
Bend relief
Where a bend terminates at an edge, provide a relief notch at least as wide as the material thickness and deeper than the bend radius plus thickness. Without it the material tears at the end of the bend.
Flat pattern and K-factor
Bend allowance depends on the K-factor — the position of the neutral axis as a fraction of thickness — which typically runs 0.33 for tight radii and approaches 0.5 for generous ones, with 0.42–0.45 a common working value for air-bent mild steel. Use the shop's actual bend deduction table rather than a nominal value; see the bend radius and K-factor chart and the sheet metal gauge chart.
Grain direction
Bend across the rolling direction wherever possible. Bends parallel to the grain crack at the outer fiber, most notably in 5000- and 6000-series aluminum and in high-strength steels.
| Feature | Recommended | Limit | Why |
|---|---|---|---|
| Inside bend radius, mild steel | 1× thickness | 0.5× thickness with coining | Outer fiber cracks at tighter radii |
| Inside bend radius, 6061-T6 | 3–4× thickness | 2× thickness across grain | Hard tempers have little outer-fiber ductility |
| V-die opening | 8× thickness | 6–12× thickness | Sets achieved radius and required tonnage |
| Minimum flange length | 4× thickness | Half the V-width plus thickness | Flange must span both die shoulders |
| Hole to bend line | ≥ 2.5× thickness + radius | — | Stretching around the bend distorts the hole |
| Bend relief | Width ≥ thickness, depth > radius + thickness | — | Prevents tearing at the bend end |
| Same radius on all bends | Yes | — | Every distinct radius is another setup |
| Bend angle tolerance | ±1° | ±0.5° with angle measurement | Springback varies with coil lot and thickness |
Cost drivers
Press braking has effectively no part-specific tooling cost, so the entire bill is setup plus cycle time plus handling. Setup dominates short runs: loading and aligning tooling, programming the sequence, and bending a first article can take longer than running fifty parts. Cycle time scales with the number of bends and with part size — a large panel needs two operators or a robot, which doubles the labor rate.
Volume breakpoints: 1–100 parts is where press braking is unbeatable, since a stamping die would never amortize. From 1,000 to 10,000 it is still usually competitive with hard tooling. Above roughly 25,000 identical parts a year, a progressive die or a roll-formed profile beats it on cycle time.
- Reduce the number of bends. Each bend is a handling cycle. Two bends removed from a bracket is a real percentage of its cost.
- Use one bend radius and one material thickness across the whole assembly. This lets the shop run multiple part numbers on a single setup.
- Keep flanges long enough to gauge on. Flanges shorter than about 4× thickness force special tooling or a hand-held first article.
- Avoid bends that require the part to be reoriented repeatedly. A sequence that can be run with one backgauge setup runs far faster.
- Design so no bend traps the part. Check that the last bend can still be reached without the formed geometry hitting the ram — this is the most common cause of a redesign request from the shop floor.
Questions
6 questionsWhat is the minimum bend radius for press braking?
About 1× material thickness for mild steel and annealed aluminum. Hard tempers need more — 6061-T6 typically wants 2–4× thickness, and more if the bend runs parallel to the rolling direction. Coining can go tighter but requires roughly five to ten times the air-bend force.
What die opening should I use on a press brake?
Start at about 8× material thickness. The die opening, not the punch tip, controls the achieved inside radius in air bending — roughly 16% of the V-width for mild steel — and it also sets the tonnage, which falls as the opening widens.
What is the minimum flange length on a press brake?
Roughly 4× material thickness, or half the die opening plus one thickness, whichever is larger. The flange has to rest on both shoulders of the V-die. Shorter flanges slide into the die and form inconsistently, and require special tooling to make repeatably.
How much springback should I expect?
About 1–3° for mild steel, more for stainless, aluminum, and high-strength grades. The CNC compensates by overbending, and angle-measurement systems correct in process, but springback varies between coil lots, which is why bend angles are typically toleranced at ±1°.
What K-factor should I use for a flat pattern?
K-factor runs from about 0.33 at tight radii toward 0.5 at generous ones, with 0.42–0.45 common for air-bent mild steel. Use the fabricator's measured bend deduction table rather than a nominal figure, since it is specific to their tooling and material.
Press braking or roll forming?
Press braking for varied parts, short runs, and anything under roughly 25,000 pieces, since it needs no dedicated tooling. Roll forming for long constant cross-section profiles at high volume, where its continuous line produces hundreds of feet per minute against one bend per stroke on a brake.