Sheet Metal Gauge Chart.
Convert gauge number to thickness in millimetres and inches for standard steel, galvanised steel, stainless steel and aluminium. Includes sheet weight, minimum bend radius and the nearest metric stock size.
Look Up
Sheet and Bending
Min inside radius ≈ 1 × t mild steel, 3 × t for 6061-T6
Min punched hole dia ≈ 1 × t (mild steel), 2 × t (stainless)
Hole / bend edge distance ≈ 2.5 × t + inside radius
Why Gauge Numbers Are Not Interchangeable
Sheet metal gauge is a legacy scale from wire drawing, where the number counted how many times the material had been pulled through a die. More passes meant thinner material — which is why a higher gauge number means a thinner sheet, the opposite of every other size convention in engineering.
The important consequence: each material has its own gauge scale. 16 gauge is 1.52 mm in standard steel, 1.61 mm in galvanised steel, 1.59 mm in stainless, and 1.29 mm in aluminium. Ordering "16 gauge" without naming the material is how the wrong plate arrives.
| Gauge | Steel (mm) | Galvanised (mm) | Stainless (mm) | Aluminium (mm) |
|---|---|---|---|---|
| 7 | 4.55 | — | 4.76 | 3.67 |
| 8 | 4.18 | 4.27 | 4.37 | 3.26 |
| 10 | 3.42 | 3.51 | 3.57 | 2.59 |
| 11 | 3.04 | 3.13 | 3.18 | 2.30 |
| 12 | 2.66 | 2.75 | 2.78 | 2.05 |
| 13 | 2.28 | 2.37 | 2.38 | 1.83 |
| 14 | 1.90 | 1.99 | 1.98 | 1.63 |
| 16 | 1.52 | 1.61 | 1.59 | 1.29 |
| 18 | 1.21 | 1.31 | 1.27 | 1.02 |
| 20 | 0.91 | 1.01 | 0.95 | 0.81 |
| 22 | 0.76 | 0.85 | 0.79 | 0.64 |
| 24 | 0.61 | 0.70 | 0.64 | 0.51 |
| 26 | 0.45 | 0.55 | 0.48 | 0.40 |
| 28 | 0.38 | 0.47 | 0.40 | 0.32 |
Galvanised sheet is consistently thicker than the equivalent bare steel gauge because the scale includes the zinc coating — roughly 0.09 mm for a standard G90 coating.
Sheet Weight
kg/m² = thickness (mm) × density (g/cm³)
Steel has a density of 7.85 g/cm³, so a convenient shop rule is 7.85 kg per m² per mm of thickness. A 2500 × 1250 mm sheet of 1.5 mm mild steel is 3.125 m² × 1.5 × 7.85 = 36.8 kg. Stainless is about 1% heavier, aluminium about a third of the weight at 2.70 g/cm³.
Minimum Bend Radius
Bend an inside radius tighter than the material can take and the outer fibre cracks. The limit scales with thickness and with how much cold work the alloy already carries:
| Material | Min inside radius | Notes |
|---|---|---|
| Cold rolled mild steel | 1.0 × t | Most forgiving common material |
| Hot rolled steel | 1.5 × t | Coarser grain, scale on surface |
| Stainless 304 annealed | 1.5 × t | Springback is significant |
| Aluminium 5052-H32 | 1.0 × t | Good general forming alloy |
| Aluminium 6061-T6 | 3.0 × t | Cracks readily — bend in T4 and age after |
Always bend across the grain where possible. Bending parallel to the rolling direction can halve the achievable radius before cracking, and 6061-T6 in particular is unforgiving.
V-Die Selection and Bend Deduction
In air bending the die opening controls both the achievable inside radius and the force required. The standard starting point is a V opening of 8 × material thickness, which naturally produces an inside radius of roughly 0.16 × the opening — close to 1.3 × t.
Bigger die openings need less tonnage and give a larger radius; smaller openings mark the surface and can crack the outer fibre. For thickness above about 3 mm, 10 × t is common practice.
The flat pattern is shorter than the sum of the outside dimensions because material stretches around the bend. That difference is the bend deduction, and it depends on the neutral axis position through the K-factor — typically 0.33 to 0.45 for common sheet operations. For the full worked calculation, see the Bend Allowance and K-Factor Calculator.
Design Rules for Punched Features
- Minimum hole diameter — 1 × t in mild steel, 1.5 × t in aluminium, 2 × t in stainless. Below that the punch breaks before the slug does.
- Hole to bend distance — at least 2.5 × t plus the inside bend radius, measured from the hole edge to the bend line. Closer and the hole distorts into an oval.
- Hole to edge — at least 2 × t, or the edge bulges.
- Slot width — at least 1 × t; slot length no more than 5 × width for tool life.
- Relief notches — at intersecting bends, at least 1 × t wide and extending past the bend line, or the corner tears.
- Minimum flange length — 4 × t plus the bend radius, so the flange clears the die shoulder.
Metric Stock Sizes
Outside North America, sheet is ordered in millimetres and gauge numbers are only used to interpret legacy drawings. Common metric stock runs 0.5, 0.6, 0.8, 1.0, 1.2, 1.5, 2.0, 2.5, 3.0, 4.0, 5.0 and 6.0 mm. Where a drawing specifies a gauge, quote the nearest metric stock rather than asking a supplier to match the imperial figure — the price difference on a non-stock thickness is rarely worth it.
Related Tools
For the flat pattern, use the Bend Allowance / K-Factor Calculator. For total part weight and material cost, see Material Weight. For hole positional callouts see Position Tolerance, and for general tolerances on fabricated parts see ISO 2768.