---
type: process
name: "Metal Stamping"
category: "Forming"
subcategory: "Metal"
materials: ["Metal"]
tolerances: "±0.005 in (±0.13 mm) typical on blanked and pierced features; ±0.001–0.002 in (±0.025–0.05 mm) achievable in precision dies. Formed dimensions spanning several stations hold looser than single-station features"
volumes: "25,000–10,000,000+ parts per year; below about 10,000 laser cutting and press braking usually win"
lead_time: "10–20 weeks for progressive die design, build, and tryout; 1–3 weeks per production release thereafter"
url: https://manufacturingprocesses.org/processes/forming/metal-stamping
---

# Metal Stamping

Metal stamping shears and forms sheet metal between matched dies in a press, producing flat and shallow-formed parts at very high rates.

- **Category**: [Forming](https://manufacturingprocesses.org/processes/forming.md)
- **Family**: Metal
- **Materials**: Metal
- **Typical tolerances**: ±0.005 in (±0.13 mm) typical on blanked and pierced features; ±0.001–0.002 in (±0.025–0.05 mm) achievable in precision dies. Formed dimensions spanning several stations hold looser than single-station features
- **Surface finish**: Inherits the coil finish, typically 16–63 µin Ra (0.4–1.6 µm); sheared edges carry a burr up to about 10% of thickness
- **Typical volumes**: 25,000–10,000,000+ parts per year; below about 10,000 laser cutting and press braking usually win
- **Lead time**: 10–20 weeks for progressive die design, build, and tryout; 1–3 weeks per production release thereafter

## Overview

Metal stamping shears and forms sheet metal between matched punch-and-die sets in a mechanical or servo press, producing flat blanks and shallow-formed parts at rates no other metal process approaches. A progressive die running at 200 strokes per minute makes 12,000 parts an hour from a single coil, and high-speed lines for terminals and lead frames exceed 1,000 strokes per minute.

Operations combine freely in one die: blanking, piercing, notching, bending, coining, embossing, lancing, and drawing. Typical parts are brackets, clips, contacts, shielding cans, hinges, lamination stacks, and structural body panels, in low-carbon steel, high-strength steel, stainless, aluminum, copper, and brass from about 0.005 to 0.250 in (0.13 to 6 mm).

The economics are tooling-driven. A progressive die is a substantial investment with a multi-month build, so stamping is a high-volume answer — generally above 25,000–50,000 parts a year.

## How it works

### How does the cut actually happen?

Shearing is fracture, not cutting. The punch first pushes the sheet down (rollover), then penetrates and burnishes a smooth band, and then a crack initiates from the punch and die edges and runs through the remaining thickness. A correctly clearanced cut has the two cracks meet, giving a clean break; wrong clearance makes them miss, leaving a secondary shear band and a heavy burr. Die clearance is roughly 5–10% of material thickness per side — toward the low end for soft aluminum, the high end for high-strength steel.

### The die types

- **Progressive dies** carry the strip through a series of stations on a carrier web, adding one operation per stroke, and cut the part free at the last station. This is the high-volume standard.
- **Transfer dies** cut the blank free first and move it mechanically between stations, which allows deeper forms than a carrier strip can support.
- **Compound dies** do several operations in a single stroke at one station, giving excellent flatness and concentricity for simple parts.

### The cycle

1. **Coil feed.** Stock is uncoiled, straightened through a leveler, and fed by a servo roll feed to a pitch accuracy typically within a few thousandths of an inch.
2. **Pilot.** Pilot pins enter pre-pierced holes to register the strip precisely before any station works it.
3. **Stroke.** All stations act simultaneously. Tonnage required is approximately cut perimeter × thickness × material shear strength; shear strength runs roughly 70–80% of tensile strength for common steels.
4. **Form.** Bending, drawing, and coining stations shape the part while it is still attached to the carrier.
5. **Cutoff.** The final station separates the part; the skeleton scrap is chopped and recycled.
6. **Secondary.** Deburring, tumbling, tapping, plating, or heat treatment as required.

Press selection follows tonnage and speed. Servo presses allow the slide velocity to be programmed within the stroke, which is what makes high-strength steels and deep forms viable at rate.

## Design guidelines

### Hole size and spacing

Minimum punched hole diameter is about 1× material thickness in mild steel and 1.5–2× in stainless and high-strength grades — below that, punches break. Keep holes at least 2× thickness from any edge and 2× thickness from each other, and make slots at least 1.5× thickness wide.

### Distance from a hole to a bend

Keep the edge of a hole at least 2.5× material thickness plus the bend radius away from the bend line. Closer and the hole distorts into an oval as the metal stretches around the bend.

### Bend radius and grain direction

Inside bend radius should be at least 1× material thickness for mild steel and more for high-strength or hardened tempers. Bend across the rolling direction where possible; bending parallel to the grain cracks the outer fiber, which is a routine failure in 5000- and 6000-series aluminum. Flat patterns come from the [bend radius and K-factor chart](/charts/sheet-metal-bend-radius-k-factor), and stock thickness from the [sheet metal gauge chart](/charts/sheet-metal-gauge-chart).

### Bend relief

Where a bend ends at a formed edge, add a relief notch at least as wide as the material thickness and deeper than the bend radius plus thickness. Without relief the material tears at the bend end.

### Edge condition and burr

Every sheared edge has a burr on the die side. Specify the burr side on the drawing if it matters; a common acceptance limit is 10% of material thickness. Call out deburring or tumbling explicitly rather than assuming it.

### Flatness

Blanking induces stress and parts come out with some bow and camber. If flatness is functional, specify it — restrike or a leveling operation adds cost but is the only way to get it.

### Tolerances

Features made within one die station hold much better than features spanning several stations, because station-to-station accuracy depends on strip pitch and pilot registration. Group critical dimensions into the same station wherever the part permits.

| Feature | Recommended | Limit | Why |
| --- | --- | --- | --- |
| Punched hole diameter | ≥ 1.5× thickness | 1× thickness (mild steel) | Slender punches deflect and snap |
| Hole to edge | ≥ 2× thickness | 1.5× thickness | Thin webs bulge and tear during shearing |
| Slot width | ≥ 1.5× thickness | 1× thickness | Narrow punch sections lack column strength |
| Hole to bend line | ≥ 2.5× thickness + bend radius | — | Metal stretching around the bend ovals the hole |
| Inside bend radius | ≥ 1× thickness | Larger for high-strength grades | Outer fiber cracks below this |
| Bend relief | Width ≥ 1× thickness, depth > radius + thickness | — | Prevents tearing at the end of the bend |
| Die clearance | 5–8% of thickness per side | 10% for high-strength steel | Sets whether the shear cracks meet cleanly |
| Burr height | ≤ 10% of thickness | — | Sheared edges always carry a die-side burr |

## Variants

- Secondary Pressing

## Cost drivers

Tooling is the whole story at the front end. A progressive die's cost scales with station count, part size, tolerance, and die material, and it takes months to build and try out. Per-part cost is press seconds plus material, and material is usually the larger of the two: strip utilization on a typical part is 50–80%, meaning a fifth to a half of the purchased steel leaves as skeleton scrap.

Volume breakpoints: below roughly 10,000 parts, laser cutting plus press braking has no tooling cost and wins outright. From 25,000 to 250,000 a year, a simple progressive or compound die pays back. Above a million, high-speed dies, multi-out layouts, and material utilization improvements dominate the cost equation.

1. **Improve the nest.** Rotating the part on the strip or running a two-out layout can recover several percent of material on every stroke, forever.
2. **Reduce station count.** Each station is tooling, maintenance, and press length. Combining two bends into one station or dropping a non-functional feature is real money.
3. **Loosen non-critical tolerances.** Tolerances tighter than about ±0.002 in force precision die construction, harder die steel, and more frequent sharpening.
4. **Design for one grain direction.** Parts that require bends in two directions constrain the nest and can force a wider strip.
5. **Choose a common gauge and grade.** Standard coil widths and thicknesses avoid mill minimums and slitting charges.

## FAQ

### What is the minimum hole size for metal stamping?

About 1× material thickness in mild steel and 1.5–2× in stainless or high-strength grades. The limit is punch strength: a punch narrower than the sheet is thick lacks the column strength to survive repeated penetration and will break.

### How far should a hole be from a bend?

At least 2.5× material thickness plus the inside bend radius, measured from the edge of the hole to the bend line. Any closer and the metal stretching around the bend pulls the hole into an oval. If the hole must be closer, pierce it after forming.

### What die clearance should be used for stamping?

Roughly 5–10% of material thickness per side — nearer 5% for soft aluminum, 6–8% for mild steel, and up to 10% for high-strength steel. Correct clearance makes the cracks from the punch and die edges meet, which gives a clean fracture and a small burr.

### How much press tonnage does a stamping need?

Approximately the cut perimeter multiplied by material thickness and by material shear strength. Shear strength runs roughly 70–80% of tensile strength for common steels. Forming, coining, and drawing stations add their own force on top of the shearing requirement.

### Stamping or laser cutting and bending?

Laser cutting plus press braking has zero tooling cost and wins below roughly 10,000 parts a year or wherever the design is still changing. Stamping wins above 25,000–50,000, where the die amortizes and cycle time drops from minutes per part to a fraction of a second.

### Why are stamped parts not perfectly flat?

Shearing and forming leave residual stress that relaxes into bow and camber once the part is cut free. If flatness is functional, specify it on the drawing so the toolmaker can add a restrike station or a post-process leveling operation.

## Alternative processes

- [Laser Cutting](https://manufacturingprocesses.org/processes/cutting/laser-cutting.md): Laser cutting melts, burns or vaporises a narrow kerf through flat stock with a focused beam, producing profiles from a 2D file with no tooling.
- [Sheet Metal Fabrication](https://manufacturingprocesses.org/processes/forming/sheet-metal-fabrication.md): Sheet metal fabrication cuts, bends and joins flat stock into a finished assembly, typically laser cutting followed by press braking, hardware and welding.
- [Punching and Blanking](https://manufacturingprocesses.org/processes/cutting/punching-and-blanking.md): Punching and blanking shear sheet metal between a punch and a die, producing holes and flat outlines at very high speed.
- [Die Casting](https://manufacturingprocesses.org/processes/forming/die-casting.md): Die casting injects molten aluminum, zinc or magnesium into a hardened steel die under high pressure, producing thin-walled net-shape metal parts.

## Related processes

- [Press Braking](https://manufacturingprocesses.org/processes/forming/press-braking.md): Press braking bends sheet metal by driving a punch into a V-die, forming one straight-line bend at a time.
- [Deep Drawing](https://manufacturingprocesses.org/processes/forming/deep-drawing.md): Deep drawing pushes a sheet metal blank through a die with a punch so the metal flows into a seamless cup or box deeper than its own diameter.
- [Punching and Blanking](https://manufacturingprocesses.org/processes/cutting/punching-and-blanking.md): Punching and blanking shear sheet metal between a punch and a die, producing holes and flat outlines at very high speed.
- [Roll Forming](https://manufacturingprocesses.org/processes/forming/roll-forming.md): Roll forming passes coil stock through a sequence of contoured roller stands that bend it progressively into a constant cross-section profile.

---

*Source: [Manufacturing Processes](https://manufacturingprocesses.org/processes/forming/metal-stamping)*

*Last updated: August 11, 2026*