Punching and Blanking
Punching and blanking shear sheet metal between a punch and a die, producing holes and flat outlines at very high speed.
- Part
- Cutting
- Revised
- 2026-08-11
At a glance
- Family
- Mechanical
- Typical tolerances
- ±0.003–0.010 in (±0.08–0.25 mm) on punched features; ±0.002 in (±0.05 mm) achievable in a well-maintained progressive die; features punched in one station relate to each other more tightly than features across stations
- Surface finish
- A sheared edge shows four zones: rollover of 10–20% of thickness, a burnished band of about one third of thickness, a fracture zone, and a burr normally held under 10% of material thickness
- Typical volumes
- Turret punching 1–5,000; progressive dies 10,000–10,000,000+
- Lead time
- Turret punching 1–5 business days; hard tooling 4–12 weeks, then production in hours per thousand
- Materials
- Metal, Plastic
What it is
Punching and blanking shear sheet metal between a punch and a die. The difference is which piece you keep: in punching the slug that falls through is scrap and the sheet is the part; in blanking the slug is the part and the sheet becomes skeleton. Both are the fastest way to produce flat metal parts — a progressive die on a mechanical press runs hundreds of strokes per minute and holds ±0.003 in (±0.08 mm).
Press force comes straight out of the geometry: tonnage = cut perimeter (in) × thickness (in) × shear strength (tons/in²), and the shear strength of mild steel is about 25 tons/in² (50,000 psi, 345 MPa).
CNC turret punching produces the same sheared edge with standard stocked tools and no dedicated die, which makes it the low-volume route — no tooling cost, but one hit at a time.
How it works
- Clearance selection. The gap between punch and die per side is the single most important variable: roughly 5–10% of material thickness for mild steel, 3–6% for soft aluminum, and 10–12% for stainless and harder alloys. Everything about edge quality follows from getting this right.
- Rollover. The punch contacts and first deforms the sheet plastically, drawing the top edge down into a rounded rollover of roughly 10–20% of the material thickness.
- Penetration and burnish. The punch then shears into the material, producing a smooth burnished band that with correct clearance occupies about one third of the thickness. This band is the only part of the edge that is dimensionally reliable.
- Fracture. Cracks initiate at both the punch and die edges. With correct clearance they meet cleanly and the slug separates. With too little or too much clearance they miss, producing a secondary shear step or a ragged, tapered fracture zone.
- Breakthrough and stripping. The load releases suddenly at breakthrough — snap-through shock, which is why press and die design account for reverse tonnage. A stripper plate holds the sheet down as the punch withdraws.
- Progression. In a progressive die the strip advances through stations located by pilot holes, gaining holes, forms and coined features until the final station blanks the part free.
- Burr formation. The burr forms on the die side and grows as tooling dulls; 10% of material thickness is a common maximum acceptable burr height, and it is the practical indicator that punches need regrinding.
Design guidelines
Minimum hole diameter
Keep punched holes at least 1× material thickness in diameter in mild steel and 1.5× in stainless and harder alloys. Below that the punch is loaded in buckling rather than shear and breaks, and the hole comes out poorly formed.
Edge distance and hole spacing
Keep at least 2× material thickness between a hole and a formed or sheared edge, and the same between adjacent holes. Less than that and the material between them bulges or tears as the punch enters.
Slot proportions
Slot width should be at least 1× material thickness, and slot length should stay within about 10× the width per punch — longer slots are made in multiple hits or with a dedicated tool.
Blank corner radii
Give outside corners a radius of at least 0.5× material thickness. A sharp corner in a blanking die is a stress riser in the tool, wears fastest, and is the first place a die cracks.
Call out burr direction
The burr always forms on the die side of the cut. On a part where one face contacts a seal, a bearing or a user's hand, the drawing needs to state which face carries the burr — it is free to control and expensive to fix later.
Design the part around the press
Tonnage scales with cut perimeter, so a lace-like part with a huge perimeter can exceed the press before it exceeds any dimensional limit. Use the formula in the summary, or a shear angle ground into the punch face to spread the cut over the stroke.
Plan for what happens next
If the part will be bent, keep holes at least 1.5× thickness plus the bend radius from the bend line, and consider grain direction — bending across the rolling direction cracks less. See the bend radius and K-factor chart and specify stock from the sheet metal gauge chart.
| Material | Punchability | Notes |
|---|---|---|
| Mild steel (CRS, HRPO) | Excellent | The reference material; ~25 tons/in² shear strength |
| Aluminum 5052, 3003 | Excellent | Lower tonnage; use tighter clearance, 3–6% per side |
| 304 / 316 stainless | Moderate | Higher tonnage, work hardens, wider clearance, faster tool wear |
| Galvanized steel | Good | Zinc pickup on tooling; needs frequent cleaning |
| Copper, brass | Excellent | Low tonnage, clean edges |
| Spring steel, hardened stock | Difficult | Cracks at the fracture zone; consider etching or wire EDM |
| Plastic sheet | Situational | Cracks when cold; larger clearance and warm stock help |
| Feature | Recommended | Limit | Why |
|---|---|---|---|
| Hole diameter | ≥ 1.5× thickness | 1× thickness (mild steel) | Punch buckles below this |
| Hole to edge | ≥ 2× thickness | 1.5× thickness | Material bulges or tears |
| Hole to hole | ≥ 2× thickness | 1.5× thickness | Web collapses between holes |
| Slot width | ≥ 1× thickness | 0.8× thickness | Punch strength |
| Blank corner radius | ≥ 0.5× thickness | Sharp | Die corners crack and wear |
| Punch-die clearance | 5–10% of t per side (steel) | 3–12% by material | Sets edge quality and burr |
| Burr height | ≤ 10% of thickness | — | Grows as tooling dulls |
Cost drivers
The economics split cleanly between hard tooling and turret punching, and the crossover is driven entirely by volume.
Tooling. A progressive die is a substantial one-time investment with a lead time of weeks; after that, per-part cost is dominated by press time measured in strokes per minute. Turret punching has no tooling charge but hits one feature at a time.
Part perimeter drives tonnage. Tonnage sets which press the job runs on, and press size is a rate. A part that just exceeds a press's capacity moves to a bigger machine and a higher rate for no functional gain.
Number of stations. Each hole, form and coin in a progressive die is a station, and stations are die cost.
Material utilization. Strip layout, web width and part nesting decide how much of the coil becomes part rather than skeleton. On a high-volume part, a few percent of yield outweighs almost everything else.
Tool maintenance. Punches dull, burrs grow, and dies come out for regrinding on a schedule. Stainless and galvanized shorten that interval.
Four ways to take cost out:
- Below about 5,000–10,000 parts, use turret punching or laser cutting and skip the die entirely.
- Design the strip layout with the toolmaker; web and pitch decisions set material yield for the life of the part.
- Keep holes at 1× thickness or larger and 2× thickness from edges so standard punches survive.
- Consolidate features so fewer die stations are needed.
Questions
6 questionsWhat is the difference between punching and blanking?
The tooling is the same; the difference is which piece you keep. In punching, the slug pushed through the die is scrap and the remaining sheet is the part. In blanking, the slug is the part and the sheet becomes skeleton scrap. Because the burnished band and burr form the same way in both, the edge quality rules are identical.
How do I calculate press tonnage for punching?
Tonnage equals cut perimeter in inches multiplied by material thickness in inches multiplied by the material's shear strength in tons per square inch. Mild steel is about 25 tons/in² (50,000 psi, 345 MPa). A 4 in perimeter in 0.125 in mild steel therefore needs about 12.5 tons. Grinding a shear angle into the punch face spreads the cut over the stroke and reduces peak tonnage.
What is the minimum hole size for punching?
About 1× material thickness in mild steel and 1.5× thickness in stainless and harder alloys. Below that the punch is loaded in buckling rather than shear and breaks quickly. Keep holes at least 2× thickness from any edge or from each other, or the material between them bulges and tears.
What punch to die clearance should I use?
Roughly 5–10% of material thickness per side for mild steel, 3–6% for soft aluminum, and 10–12% for stainless and harder alloys. Correct clearance makes the cracks from the punch and die edges meet cleanly, producing a burnished band of about one third of the thickness. Wrong clearance produces a secondary shear step or a ragged, tapered fracture zone.
Which side of a punched part has the burr?
The die side — the side the slug exits. Burr height grows as the punch dulls, and 10% of material thickness is a common maximum acceptable value and the usual trigger for regrinding tooling. If one face of the part must be burr-free for sealing, assembly or handling, state that on the drawing, since controlling burr direction is free at the die-design stage.
At what volume does a progressive die pay for itself?
Typically somewhere above 5,000–10,000 parts, though the exact point depends on die complexity and part cycle time. Below that, CNC turret punching or laser cutting produces the same part with no tooling investment and no multi-week tooling lead time. Above it, press strokes per minute make the die the clear low-cost route.