Sheet Metal Design Guide

Design to the process, not around it

Sheet metal parts are developed as a flat pattern that is then folded. Every bend removes material from the flat, adds springback and requires tool access. The fewer bends and the more uniform their direction, the lower the cost and the better the repeatability.

Aim for one bend direction per setup wherever the geometry allows.

Keep wall thickness uniform

A single part should use one material thickness. Mixing thicknesses in one formed part forces multiple blanks, multiple programs and additional assembly, and creates stiff-to-flexible transitions that concentrate stress.

If different stiffness is needed, add formed ribs rather than changing gauge.

Specify only the tolerances that matter

General dimensions can be held to ISO 2768-m. Tight callouts should be reserved for functional features: locating hole positions, mounting-face flatness, and bores that receive a bush or bearing. Every tight tolerance adds inspection time and cost.

Provide both 3D and 2D

A 3D model (STEP or IGES) drives programming; a 2D drawing carries the tolerances, finish specification, weld symbols and critical dimensions. Supplying only one of the two is the most common cause of quotation delays.

K-Factor

The K-factor is the ratio between the position of the neutral axis and the material thickness. It determines how much the flat pattern must be shortened or lengthened at each bend. Typical values run from 0.3 to 0.5 depending on material, thickness, tooling and bend angle.

Bend Allowance = (π / 180) × Bend Angle × (Inside Radius + K-Factor × Thickness)

Send us your assumed K-factor if your CAD model already unfolds the part, so our flat pattern matches yours.

Wall Thickness Range

We form sheet from 0.9 mm up to 20 mm. Material below about 3 mm is processed as sheet, above that as plate, and the tooling, bend radius and springback behaviour differ between the two. Very thin material below 0.9 mm is better suited to stamping or photo-etching.

Bend Radius

Use one inside bend radius across the entire part so a single tool set can form it. The practical minimum is one material thickness; going below that risks cracking on the outer fibre, particularly on aluminum and high-strength steel.

Minimum Inside Radius = 1 × Material Thickness

Radii below 1t require special tooling and are quoted separately.

Consistent Bend Orientation

When all bends run in the same direction the part can be formed in one setup without re-orientation. Mixed orientation means the operator must flip the part, which adds handling time, introduces a second source of error and can make some bends unreachable with standard tooling.

Minimum Flange Length

The flange must be long enough to rest on the die shoulder until the bend is complete. A flange shorter than this will slip into the die opening and produce an inconsistent angle or a rounded edge.

Minimum Flange = Inside Radius + Thickness + Die Shoulder Allowance (≈ 3 × Thickness)

Bend Relief

Where a bend runs into an existing edge or a cutout, the material can tear. Adding a relief notch, a tear relief slot or a rectangular relief cut prevents this. Relief width should be at least the material thickness, and relief depth should extend slightly past the bend line.

If you omit relief, we will add it during programming and flag it on the returned drawing.

Bend Height

The height of a formed flange must be sufficient to be held by the tooling. A flange shorter than twice the thickness plus the bend radius cannot be formed reliably.

H ≥ 2t + r

Forming Near Holes

A bend placed too close to a hole distorts it into a teardrop. Keep holes at least 2.5 times the material thickness plus the bend radius away from the bend line. Where that is not possible, add relief cuts around the hole or machine the hole after forming.

Distance from Bend Line ≥ 2.5t + r

Minimum Hole Diameter

Pierced and laser-cut holes should not be smaller than the material thickness. Smaller punches deflect and break, and laser-cut micro holes leave excessive dross. For holes below 1t, specify a drilled or machined operation instead.

Minimum Hole Diameter ≥ 1 × Thickness

Extruded Holes and Edge Distance

Extruding a hole is one of the highest-pressure operations in press working and generates significant friction and heat. Keep extruded holes well away from part edges and from other extrusions, otherwise the material between them thins and the extrusion collapses.

General Tolerances

Where a drawing does not specify otherwise, we manufacture to the model with general tolerances per ISO 2768-m. This covers cut profile, bend angles and overall size for the majority of industrial parts.

Typical Achievable Values

Cut profile ±0.1 to ±0.2 mm depending on thickness; bend angle ±0.5 to ±1 degree; hole position ±0.15 mm; flatness of a mounting face 0.2 to 0.5 mm per 100 mm. Tighter values are achievable on machined features and are quoted separately.

Laser Kerf

Laser cutting burns away a narrow band of material, leaving a gap known as the kerf. It typically ranges from 0.08 to 0.45 mm depending on material, thickness, laser power and cutting speed. Kerf is compensated in the nesting program, but it matters when two parts must fit together from the same sheet.

Tell us if a cutout and its matching insert come from the same blank; we will adjust the compensation.

Springback and First-Off Approval

Every material and thickness combination springs back differently, and high-strength grades spring back more. We establish the correct overbend on the first part and record it in the program. For series production we recommend a first-off approval before the batch runs.

Minimum Diameter and Width

Keep hole diameters and slot widths at least equal to the material thickness. Higher-strength materials need larger minimums because the punch experiences greater lateral load.

Diameter or Slot Width ≥ 1 × Thickness

Edge Clearance

Holes too close to an edge cause the material to bulge or tear during cutting. Keep the distance from hole edge to part edge at least one material thickness, and preferably two for thin gauges.

Hole Edge to Part Edge ≥ 1 × Thickness

Hole-to-Hole Spacing

Adjacent holes need enough material between them to stay round. Minimum centre-to-centre distance is normally twice the thickness, or one hole diameter plus the thickness, whichever is greater.

Slots and Elongated Holes

Corner radii on slots should be at least half the material thickness. Sharp internal corners concentrate stress, slow the laser down and leave a rougher edge. Slots used for adjustment should be dimensioned with the fastener head and washer in mind, not just the shank.

Threaded Holes in Thin Sheet

Tapping sheet thinner than about 1.5 mm produces very few engaged threads. Use pressed-in threaded inserts, welded nuts or clinch standoffs instead; they hold far better under repeated assembly and do not strip.

Notch Sizing

A notch must be at least as wide as the material thickness and should not be longer than five times its width. Long narrow notches are difficult to cut cleanly and leave a weak section that can tear during handling.

Notch Width ≥ t; Notch Length ≤ 5 × Width

Tab Sizing

Tabs must be at least twice the material thickness wide. Narrow tabs bend or break during forming, welding and packing, and they are a common source of scrap on parts that otherwise measure correctly.

Tab Width ≥ 2 × Thickness

Spacing Between Features

Keep at least one material thickness between a notch or tab and any other cutout, hole or bend line. Features closer than this merge during cutting and produce an unintended profile.

External Corners

A radius of at least half the material thickness is recommended on external corners. Fully square external corners are possible but leave a sharp edge that can cut an assembler and that chips paint more easily.

External Corner Radius ≥ 0.5 × Thickness

Internal Corners

Internal corners should carry a radius of at least one material thickness. A true sharp internal corner is a stress raiser and a crack initiation point, particularly on aluminum and on parts that see cyclic loading.

Consistency

Use the same fillet radius across the part where possible. Mixed radii require multiple tools and increase the chance of a programming error on a nested batch.

Open and Closed Hems

Both types can be formed. An open hem leaves a visible gap and is easier to produce; a closed hem is fully flattened and gives the best edge stiffness and appearance, at the cost of an additional forming stage.

Hem Guidelines

The hem radius should be at least the material thickness, and the hemmed edge should be at least four times the thickness long. Hems placed too close to holes, slots or other bends will distort those features during flattening.

Keep a clearance of at least 2.5 times the thickness between a hem and any other feature.

Hem Tolerance

Hem tolerance depends on the hem radius, material thickness and the features near the hem. Expect ±0.3 to ±0.5 mm on hem height for standard production; tighter values require a coining stage in a press.

Curl Feature Guidelines

The internal radius of a curl should be at least the material thickness. Material between the curl and any other feature must be sufficient to avoid distortion, so keep at least the curl radius plus one thickness of clear material before the next bend or cutout.

Curl Internal Radius ≥ 1 × Thickness

Curl Direction

Curls formed away from the part body are easier to produce and give a cleaner result. Curls formed toward the body can trap material and require an additional stage.

Hinge and Pin Applications

Where a curl carries a hinge pin, specify the pin diameter and the required clearance. We will size the curl inner diameter to give the running fit you need, and leave the ends of the curl open or closed according to the assembly.

Machined vs Formed

Machined countersinks are cut after laser forming and suit small quantities and thick material. Formed countersinks are extruded with a punch, which displaces rather than removes material, giving better thread engagement in thin sheet and lower unit cost at volume.

Countersink Tolerance

Standard countersink angle tolerance is ±1 degree, with diameter tolerance of ±0.2 mm for machined and ±0.3 mm for formed features. Depth is normally controlled by the angle and diameter rather than called separately.

Countersink Dimensions and Spacing

Keep the distance between countersink centres at least eight times the material thickness, and the distance from a bend line to the countersink centre at least three times the thickness plus the bend radius. Closer than this, the forming operation distorts the countersink.

Centre to Centre ≥ 8t; Bend Line to Centre ≥ 3t + r

Minimum Material Thickness

A countersink needs enough material to form a usable cone. As a rule, the sheet should be at least as thick as the countersink depth required by the fastener head. On very thin sheet, use a clinch nut or a bonded stud instead.

Stainless Steel 304 / 316L

The default for washdown, food, pharmaceutical, marine-adjacent and semiconductor equipment. Good corrosion resistance, weldable, and accepts brushed, bead-blasted or passivated finishes. 316L is specified where chlorides or acids are present. Heavier and more expensive than mild steel, with higher springback.

Aluminum 5052 / 6061

Chosen for weight-sensitive and mobile equipment, roughly one third the density of steel. 5052 forms well and is the standard for enclosures and brackets; 6061 is stronger and suits machined features but cracks more readily on tight bends. Both need larger inside radii than steel and are vulnerable to galvanic corrosion against steel.

Cold-Rolled and Galvanized Steel

The economical option for indoor machinery guards, control cabinets and structural brackets where corrosion exposure is limited. Galvanized stock carries a zinc coating for basic protection; note that welding burns off zinc locally and the affected area needs touch-up or a coating specification.

HSLA and High-Strength Steel

Used where stiffness per millimetre of thickness matters, particularly automotive brackets and structural frames. Higher yield strength means greater springback and a larger minimum bend radius; both must be reflected in the flat pattern.

Copper and Brass

Selected for electrical conductivity, thermal performance or appearance. Both are soft and mark easily, so protective film and careful handling are specified through the routing. Copper work-hardens quickly and needs generous bend radii.

Weld Access and Joint Design

The torch must reach the joint. Leave clearance for the welding head and for the fixture that holds the part, and avoid placing welds inside narrow channels. Lap joints and fillet welds are the most economical; full-penetration butt welds cost more and distort more.

Distortion Control

Thin sheet moves when heated. We control distortion through weld sequencing, tack-and-verify practice, fixture restraint and post-weld flattening on sealing and mounting faces. Designing a stiffening flange near a long weld reduces the problem at source.

Flag any face that must stay flat after welding; we will plan the sequence around it.

Weld Finish

Decide early whether welds are structural and left visible, ground smooth, or ground and blended for a cosmetic surface. Each step adds labour, and a cosmetic weld on a hidden joint is unnecessary cost.

Fastening Alternatives

Pressed inserts, clinch nuts, welded studs and riveted joints often replace a welded sub-assembly. Removing a weld removes a fixture, an inspection step and a distortion source, which frequently reduces unit cost more than any material saving.

Powder Coating

The most common finish for industrial enclosures and machinery panels, offering good durability and consistent colour for branding. Adds roughly 60 to 120 microns per side, which must be accounted for on mating features and threaded holes.

Anodizing

A hard, non-chipping surface for aluminum. Standard anodize is electrically insulating, so conductive anodize, chemical film or masked bare areas are required wherever a grounding path is needed.

Passivation, Brushing and Bead Blasting

Typical routes for stainless steel. Passivation restores the corrosion-resistant surface after welding; brushing gives a directional cosmetic grain; bead blasting produces a uniform matte texture. Define the grain direction on the drawing if appearance matters.

Masking and Cosmetic Class

Specify which areas stay uncoated: threaded holes, grounding points, sealing faces and bearing surfaces. Masking tolerance is normally ±0.5 mm, and the mask boundary should sit under a fastener head or gasket compression area so it is never exposed. Also state the cosmetic class, since visible panels require more handling protection than internal structure.

Geometry

Uniform wall thickness; single inside bend radius where possible; bend relief added near edges and cutouts; holes at least one thickness in diameter and kept away from bends; corner fillets applied; notches, tabs and hems sized per the rules above.

Documentation

3D model in STEP or IGES plus a 2D drawing marking critical dimensions, tolerances, weld symbols, material grade, finish specification and cosmetic class. Include the assembly context so we can see what the part mates to.

Commercial Information

Target quantity for the first order, expected annual volume and release pattern, required delivery date, destination for freight evaluation, and a target price if one exists. With these we can advise whether laser cutting or stamping tooling is the better route.

Next Step

Send the package to our engineering team. We review every drawing for manufacturability before quotation and return both an itemized price and DFM feedback on the features that will most affect cost, lead time and fit.