How do you design sheet metal parts for manufacturability?
- Share
- Issue Time
- Oct 19,2026
The short answer
Start with thickness: it sets every other limit. Keep holes at least one thickness across and 2.5 thicknesses plus the bend radius away from a bend line, keep the inside bend radius at one thickness for mild steel, and tolerance to ISO 2768-m except where a feature actually mates. That removes most avoidable cost before a quote is issued.
Thickness first, because it sets every limit
Sheet metal design for manufacturability is usually presented as a list of independent rules, which is misleading. The rules are all functions of one number. Material thickness sets the minimum hole diameter, the minimum inside bend radius, the minimum flange the press brake can grip, the distance a hole must stay clear of a bend, the tonnage needed to cut and form, and the tolerance the process can hold. Change the thickness by 50 percent and every one of those limits moves with it, which is why "make it thicker so it is stronger" is such an expensive instinct: a formed rib, a swage or a change of section will often deliver the stiffness at a fraction of the cost, without moving every constraint on the drawing.
The practical range for fabricated sheet parts is 0.5 to 3 mm for enclosures and brackets, 3 to 6 mm for structural work, and beyond 6 mm bending capability falls away quickly and machining or casting usually becomes the better route. Standardising on one or two gauges across an assembly is worth more than optimising each part individually, because it removes material changes, separate setup and separate scrap handling from the shop floor.
Holes, slots and edges
Holes smaller than the material thickness are the classic DFM error. A laser can technically cut a 0.5 mm hole in 2 mm steel, but the cut is slow, the hole tapers, and the heat-affected zone around it is larger than the hole itself; a punch needs a tool that small and will break it. The working rule is a minimum diameter equal to the thickness, with 1.2 times the thickness preferred for a clean laser cut. The same logic applies to slots: a slot narrower than the sheet thickness cuts badly and wears tooling, so keep the width at one thickness or more.
Position matters as much as size. Holes placed inside the bend deformation zone stretch into ovals as the material flows, and the distortion is not recoverable after forming. Keep holes and slots at least 2.5 times the thickness plus the inside bend radius away from the bend line, keep them 1.5 times the thickness from any edge, and leave 2 times the thickness between adjacent holes so the web between them does not distort. Where a hole must sit close to a bend for functional reasons, the usual fix is to cut it after forming, or to add a relief so the deformation has somewhere else to go.
| Feature | Rule of thumb | Reason |
|---|---|---|
| Hole diameter | at least 1.0 x t, 1.2 x t preferred | smaller holes burn, taper or need a second operation |
| Hole to bend line | 2.5 x t + inside radius | the bend deformation zone pulls the hole out of round |
| Hole to edge | 1.5 x t | thin ligaments tear during forming and handling |
| Hole to hole | 2.0 x t | the web distorts and the pitch drifts |
| Slot width | 1.0 x t | narrow slots cut with dross and wear the punch |
| Internal corner radius | 0.5 x t | a round cutter cannot produce a sharp internal corner |
| Minimum flange | 4.0 x t + bend radius | shorter flanges cannot be supported by the V-die |
Bend radius and flange length
The minimum inside bend radius is a material property, not a shop preference. Mild steel and soft aluminium form at about one thickness; stainless work-hardens in the bend and needs 1.5 to 2 thicknesses; 6061-T6 aluminium is the exception that catches designers out, needing 3 to 4 thicknesses because the tempered alloy has almost no ductility left and cracks on the outside of a tight bend. Bending across the rolling direction rather than along it also raises the safe radius, because the grain structure is anisotropic. When a design needs a tighter radius than the material allows, the answer is usually a softer temper or a different alloy rather than a press brake operator trying harder.
Flange length is the other half of the bend rule. A press brake grips the flange between the punch and the V-die, and a flange shorter than about four thicknesses plus the bend radius cannot be supported through the stroke; it slips, the angle drifts, and the operator ends up making a special tool. The same constraint applies to the distance between two bends: if the flat between them is shorter than the tooling needs, the part cannot be formed in the intended sequence. Both are visible on the flat pattern before any tooling is cut, which is why the flat pattern, not the 3D model, is the drawing the shop actually quotes from.
Tolerances: spend them only where they matter
Over-tolerancing is the single largest avoidable cost in sheet metal. A fabricated part is a stack of processes, each with its own natural variation: laser positioning, bend angle, bend position, hole distortion after forming, and welding distortion if the part is assembled. ISO 2768-m general tolerances cover the overwhelming majority of features at no extra cost. Naming a tighter value on a feature that does not mate, seal or locate does not make the part more accurate; it adds inspection, rejection and price. The workable discipline is to tolerance by function: identify the features that locate a mating part, carry a load or seal against something, give those an informed callout, and leave everything else under general tolerance.
| Characteristic | Normal capability | What tightening costs |
|---|---|---|
| Laser cut feature position | ±0.1 mm under 300 mm | inspection time, not accuracy |
| Bend angle | ±0.5 degrees | in-process adjustment, slower cycle |
| Bend to bend dimension | ±0.3 to 0.5 mm | special tooling or a second hit |
| Hole position after forming | ±0.3 mm | post-form drilling |
| General tolerance | ISO 2768-m | nothing, it is the default |
| Halving any of the above | not a process capability | 15 to 30 percent added to part price |
Features that quietly add operations
Several features are cheap on a drawing and expensive on a routing. A countersink or counterbore is a second operation, and on a laser-cut part it usually means a drill press and a fixture. A tapped hole is a third. A press-fit insert needs a hole sized for it and enough material around it to displace into, which sets a minimum thickness and edge distance that the design may not have. A weld seam adds fixturing, distortion and post-weld finishing, and a full-length cosmetic weld on thin sheet is one of the most expensive lines you can put on a drawing. A blanket "deburr all edges" note is also an operation, sometimes a manual one, on a part that may only need two edges dressed. Each of these is legitimate when the function requires it; the error is adding them by default.
The review order that catches cost early
Because the constraints cascade, the review has to run in order. Fix the thickness first and check that it is a stocked gauge. Place holes and slots next, against the bend lines rather than against the part outline, because the bend lines are what move during forming. Then set the bend rules: inside radius, flange length, relief at the end of every bend line, and a bend sequence the tooling can actually run. Tolerance last, general first and critical features only where they earn their cost. Finish after that, because a powder coat adds 60 to 90 microns and will close a small gap or fill a fine thread that was dimensioned before coating was considered.
See sheet metal fabrication for the laser cutting, bending and assembly capability these rules are written against, custom sheet metal parts for bracket and enclosure work quoted from a flat pattern, and metal bending for press brake work where flange length and radius decide the tooling.
Scope and sources. The DFM checklist of hole diameter at least one thickness, internal corner radius at least half a thickness, hole to bend line at least 2.5 thicknesses plus the inside radius, minimum flange set by the V-die, slot width at least one thickness, edge distance at least one thickness and ISO 2768-m as the default tolerance is set out in a sheet metal DFM rule set written for the shop floor. The thickness bands of 0.5 to 3 mm for enclosures, 3 to 6 mm for structural parts, the 1.0 and 1.5 thickness bend radius rules, the hole spacing figures and the ISO 2768-m reference come from a manufacturability guide for sheet metal parts. The laser tolerance of ±0.1 mm, bend angle of ±0.5 degrees, flange of ±0.5 mm, formed hole position of ±0.3 mm and the 15 to 30 percent cost of halving a tolerance are from a sheet metal fabrication design guide. The 4 times thickness plus radius flange minimum, the 2.5 times thickness plus radius hole clearance and the 3 to 4 times thickness radius for 6061-T6 are from a fabrication guide covering bend radius and hole placement, with slot orientation and tolerance-by-function advice in a sheet metal design guide. These are standard-tooling rules; the exact limits for a specific gauge, temper and tool set should be confirmed by the fabricator on your flat pattern.