Introduction
Sheet metal is one of the most cost-effective manufacturing processes available to mechanical designers — but only when the design respects the process constraints. Parts that ignore bend radii minimums, punch-to-edge distances, or corner relief requirements will either crack during forming, require expensive secondary operations, or come back from the shop with a call asking “is this really what you meant?”
This article covers the fundamental design rules for sheet metal parts: what they are, why they exist in terms of the underlying physics, and how to apply them in practical drawing callouts. These rules apply broadly across mild steel, stainless steel, and aluminum sheet, with notes on where material type requires adjustment.
Bend Radius: The Most Impactful Single Parameter
The inside bend radius is the smallest radius at which a given material and thickness can be bent without cracking on the outer surface. The outer fibers of the material are in tension during bending; if the radius is too small relative to the material thickness, the tensile strain exceeds the material’s elongation limit and cracks form.
Minimum inside bend radius by material
As a general starting point:
- Mild steel (low carbon): 0.5× to 1× material thickness (t)
- Stainless steel (304): 1× to 1.5× t — work-hardens more than mild steel
- Aluminum (6061-T6): 1.5× to 3× t — lower ductility, particularly in T6 temper
- Aluminum (5052-H32): 0.5× to 1× t — better formability than 6061-T6
These are guidelines, not absolutes. Your actual minimum radius depends on the specific alloy, temper, sheet direction relative to rolling direction, and the bending process. Consult your fabrication shop’s capability documentation for confirmed minimums on their equipment.
Design practice: Unless you have a specific geometric reason for tight bends, design to 1× material thickness as your standard inside radius. This is achievable on virtually all sheet metal materials and equipment without risk. Going tighter saves very little space but introduces quality risk.
K-Factor: Understanding the Flat Pattern
When sheet metal is bent, the outer surface stretches and the inner surface compresses. Somewhere in the thickness of the sheet there is a neutral axis — the line that neither stretches nor compresses. The K-factor defines the position of this neutral axis as a fraction of the material thickness:
K = t_neutral / t
where t_neutral is the distance from the inner surface to the neutral axis, and t is the total material thickness.
K-factor affects flat pattern development: a higher K-factor means more material stretches in the bend zone, which means a shorter flat blank is needed to produce a given bent geometry. Typical K-factor values:
- Air bending (most common process): K ≈ 0.33 to 0.42
- Bottom bending (coining): K ≈ 0.45 to 0.50
- Soft materials (copper, soft aluminum): K approaches 0.50
In practice, CAD software handles K-factor calculations automatically when you configure the sheet metal parameters correctly. The critical step is to verify that your CAD software’s K-factor setting matches your fabricator’s actual process — otherwise your flat patterns will be systematically off, causing assembly fit problems.
Hole and Feature Placement Rules
Punching holes too close to edges or bends creates tearing, distortion, or punch breakage. These are not conservative rules — they’re based on the physical mechanics of punching and bending.
Minimum hole-to-edge distance
The minimum distance from the edge of a punched hole to the edge of the sheet (or to another hole) is typically:
- To the sheet edge: ≥ 1.5× material thickness + bend allowance
- Hole-to-hole: ≥ 2× material thickness (center-to-center minus diameter, expressed as edge-to-edge)
For thin materials (below 1.5mm), the edge distance rules become even more critical. A small notch or tear at a hole edge in thin sheet can propagate under service loading.
Minimum hole-to-bend distance
Holes punched close to a bend line distort during bending — the hole elongates into an oval and the edge tears. The minimum safe distance from the edge of a hole to the inside of a bend is approximately:
d_min = t + r + k
where t is thickness, r is inside bend radius, and k is a material factor (typically 0 for mild steel, up to 0.5t for springback-prone materials). A conservative practical rule: keep holes at least 2× material thickness from the bend tangent line.
Corner Relief: Preventing Tear-Out at Intersecting Bends
Where two bend lines intersect (as in a box corner), the material at the intersection is pulled in multiple directions simultaneously during forming. Without relief, the material tears. Corner relief is a cutout at the bend intersection that removes the over-constrained material and provides a controlled geometry for the forming process.
Three common corner relief types:
- Square relief: A square notch cut at the bend intersection. Simple and adequate for most applications. Size: at least (bend radius + material thickness) on each side.
- Round relief: A circular punch at the bend intersection. Better stress distribution than square; recommended for higher-strength materials or applications where the part will see repeated flexing.
- Bend relief slots: Narrow slots cut from the bend line inward at the ends of the bend. Used where a flange meets a non-bending adjacent surface. Prevents the flange from tearing or distorting the adjacent flat.
Always add corner relief to your CAD model before sending to fabrication. “The shop will figure it out” leads to inconsistent relief sizes, and inconsistent relief produces inconsistent corner geometry in the finished parts.
Key Sheet Metal Design Parameters Reference
| Parameter | Rule of Thumb | Notes |
|---|---|---|
| Minimum inside bend radius | 1× material thickness (mild steel) | Verify with fabricator for specific materials |
| Hole-to-edge distance | ≥ 1.5× thickness from sheet edge | More conservative for thin sheet (<1.5mm) |
| Hole-to-bend distance | ≥ 2× thickness from bend tangent | Closer holes distort during bending |
| Corner relief size | ≥ bend radius + thickness | Round relief preferred for fatigue-loaded parts |
| K-factor (air bend) | 0.33–0.42 | Confirm with fabricator for flat pattern accuracy |
| Minimum flange length | ≥ 2.5× thickness + bend radius | Shorter flanges are difficult to clamp in brake press |
Practical Drawing Notes for Sheet Metal Parts
Sheet metal drawings benefit from a few specific notes that reduce fabrication questions:
- State the material specification including thickness tolerance (e.g., “1.5mm ±0.1mm mild steel, CR4/DC01”)
- Specify inside bend radius in drawing or general notes
- Note which surfaces require finish (powder coat, anodize) and whether dimensions are before or after finish
- If hole diameters are tolerance-critical, specify whether the tolerance applies before or after powder coat (typical powder coat adds 0.05–0.1mm per surface)
- For precise assemblies, identify datum reference surfaces for inspection of bent features
FAQ
Q: Should sheet metal designs specify the bend radius on the drawing, or is it acceptable to leave it to the fabricator?
A: For non-critical geometry where any radius produced by standard tooling is acceptable, leaving it to the fabricator is reasonable and reduces drawing constraints. For parts where the bend geometry affects fit, clearance, or stress concentration (such as a bracket with tight space constraints or a part with repeated cycling loads), specify the inside bend radius explicitly. When in doubt, call it out — it takes seconds to add and eliminates potential ambiguity.
Q: How do I handle sheet metal parts that need very tight positional tolerances on bent features?
A: Tight positional tolerances on bent features are expensive because bend position accuracy depends on springback, material variation, and tooling condition. Before specifying tight tolerances, ask whether the tolerance is driven by a real functional requirement or by design habit. If the tolerance is genuinely required, design in a post-bend machining or restrike operation on the critical features, and add machining stock accordingly. Alternatively, redesign the interface to reduce the sensitivity to bend position accuracy.
Q: How does grain direction in sheet metal affect bend quality, and do I need to specify it on the drawing?
A: Rolling direction (grain direction) in sheet metal affects ductility — bending perpendicular to the rolling direction (across the grain) typically allows tighter radii than bending parallel to it (with the grain). For most mild steel and general-purpose aluminum sheet, grain direction is not specified on drawings and the fabricator optimizes nesting for material efficiency. For high-strength alloys, large radii relative to thickness, or parts near the minimum bend radius limit, specifying bend direction relative to grain can prevent cracking. Add a note: “Bend perpendicular to rolling direction” when required.
コメント