Minimum Wall & Feature Sizes by Process

Every manufacturing process has a floor below which walls, holes, and corners stop being reliable, and the floor comes from process physics, not from shop skill. A machined steel wall below about 1.5mm deflects under cutting force and comes back oversize. A laser-cut hole smaller than the sheet thickness fights the kerf the beam removes, 0.15 to 0.30mm on thin to medium sheet. An injection-molded wall under about 1.0mm may not fill before the melt freezes, and a die-cast wall below the alloy’s range cannot be fed as it shrinks. Printed walls have their own floors: 0.5 to 1.0mm on FDM, as thin as 0.2mm on SLA, 0.7 to 1.0mm on SLS.

This page is the consolidated per-process data reference: two tables covering minimum wall thickness and minimum hole, slot, and corner sizes for CNC machining, laser cutting, sheet-metal bending, injection molding, die casting, and the three main polymer printing processes. The general principles, simplifying geometry and tolerancing only what matters, live on the design for manufacturing page. Here the question is narrower: how thin, how small, and how sharp can each process actually go?

Why each process has a floor

A floor exists where the process loses control of the feature. That happens for a different physical reason in each family, and knowing the reason tells you when a published minimum can be beaten and when it cannot.

Machining: chip load against wall rigidity

An endmill removes metal by pushing a cutter through it, and the workpiece pushes back. On a thick wall the push is absorbed; on a thin one the wall deflects away from the cutter and springs back once the cutter passes, so the wall finishes oversize, often with chatter marks. The machining rules put reliable non-critical details at 0.5 to 1.0mm and structural walls at 1.5mm or more, and walls under 1.5mm may need extra contour passes or special fixturing. The material compounds it: stainless 304 work-hardens if the tool dulls and titanium traps heat at the cutting edge, so the same thin wall is harder to finish in those alloys than in 6061 aluminum.

Laser cutting: beam kerf and heat

A fiber laser removes a 0.15 to 0.30mm slot of material on thin to medium sheet, the kerf, as it cuts. In a 2mm sheet that kerf is a manageable slice of the geometry; in a 0.8mm hole it is most of the feature, so the hole comes out ragged. That is why laser minimums scale with thickness: holes and slots at one times thickness, bridges and tabs at two times, inside corner radius at 0.5mm, and text lines at 0.5mm. Heat is the second constraint, because a small feature concentrates heat and warps, so small parts want bridges holding them to the sheet until the cut finishes.

Bending: the die needs something to grip

Bending has no wall minimum of its own, since the wall is the sheet, but it has three geometric minimums that act the same way. The inside bend radius needs at least half the thickness or the outside of the bend cracks. The flange needs to be three times the thickness tall or the die cannot hold it and the part slips. Two parallel bends need four times the thickness between them or the tooling interferes with itself. Springback of 1 to 15 degrees by material then sets how much overbend the brake applies.

Molding and casting: flow, packing, and shrink

Injection molding and die casting both force a liquid into a cavity and hold pressure on it while it solidifies, so their minimums are set by how far the material flows and how it feeds its own shrink. In molding, a conventional machine develops 20,000 to 30,000 psi of plastic pressure and wants the fill to use 50 to 75 percent of capacity, so a wall thin for its flow length either will not fill or needs more gates. Common plastics run walls of 1.0 to 1.5mm, kept uniform, because thickness variation causes preferential flow and warp, and cooling time grows with the square of thickness. Ribs are the stiffness move, kept thinner than the wall so the show face does not sink.

Die casting follows the same physics in metal. NADCA’s product standard lists typical walls from 1.0 to 5.0mm depending on alloy, size, and configuration, notes castings as thin as 0.5mm on small parts with the die caster consulted, and asks that walls stay uniform within about 10 percent of the typical section. Draft is part of the floor: commonly 2 degrees on inside surfaces and 1 degree on outside, with NADCA computing standard draft by depth and alloy and calling for twice as much inside as outside, so the part ejects without binding.

3D printing: nozzle, peel, and powder

Each printing process fails thin features in its own way. FDM extrudes a round bead through a nozzle, so walls below about 0.5mm extrude inconsistently, holes below 2 to 3mm plug, and the part is 20 to 30 percent weaker across the layer lines than in the print plane. SLA resolution is finer, but each cured layer is peeled off the tank window, so thin and unsupported sections warp; Formlabs Form 4 specifications put walls at 0.2mm and holes at 0.5mm, with shrink of 0.1 to 0.3 percent in post-cure. SLS and MJF parts sit in unfused powder that supports them, allowing self-supporting angles above 30 degrees, but that powder has to escape, so SLS holes need 1.0 to 2.0mm and escape holes 2 to 3mm.

Minimum wall thickness by process

The wall table is the core of this reference. Read the minimum column as the floor for short, well-supported, non-critical walls, and the structural column as the value to design to when the wall carries load, gets handled, or holds a tolerance. Most real parts live near the structural value, because a wall at the exact minimum costs more to make than a wall one step thicker.

Material and geometry dependencies

The floors move with the situation, and three dependencies matter most. CNC wall behavior depends on the alloy and on clamping: the 1.5mm structural floor is for cut metal generally, but gummy stainless and heat-trapping titanium punish thin walls harder than free-machining aluminum. Molded and cast walls depend on flow length, not just thickness: the fix for a wall that will not fill is more gates or an easier-flowing resin, which is a mold decision, not a wall decision. Printed walls depend on orientation: MJF holds 0.3mm in the print plane but only 0.5mm in Z, and SLA holds its tightest tolerance in XY, so orient the critical wall before trusting the minimum.

Minimum hole, slot, and corner sizes by process

Walls get the attention, but holes, slots, and corners fail more often, because each process controls them with a specific tool or physics. The feature table puts those minimums side by side.

Holes: drilled, cut, cored, and printed

A drilled hole is limited by depth, not diameter: a standard drill holds about a 4-to-1 depth-to-diameter ratio before it wanders, and gun drilling extends that to 10 to 1. A laser-cut hole is limited by thickness, at one times the sheet. A cored die-cast hole is limited by the core pin surviving injection pressure: NADCA’s table allows roughly 2.5 diameters of depth on a 3.2mm hole and up to about 6 diameters on a 25.4mm hole. Printed holes are limited by the medium: 2 to 3mm on FDM before they plug, 0.5mm on SLA, 1.0 to 2.0mm on SLS with 2 to 3mm escape holes for powder, and 1.0mm on MJF.

Corners, slots, and fine detail

Inside corners are where processes differ most. A milled inside corner can never be sharper than the endmill that cuts it, so pockets carry at least a 0.8mm radius with standard tooling and 0.5mm with precision tooling, and a plain corner radius runs 0.2 to 0.5mm. A laser-cut inside corner needs 0.5mm to avoid the heat stress concentration of a sharp intersection. Detail floors round out the picture: FDM prints text at 0.5mm height and 0.3mm line width, SLA embosses at 0.1mm, and SLS embossed text needs 4.5mm height because powder must release it.

Worked examples: three parts at the floor

The numbers are easiest to use on a real part. These three cover the most common failures.

A machined steel bracket with a 0.5mm wall

A mounting bracket in 1045 steel is modeled with a 0.5mm rib wall to save weight. That is below even the 0.5 to 1.0mm non-critical band and a third of the 1.5mm structural floor, so the wall deflects under the endmill, springs back, and finishes oversize with chatter marks; slowing the cut lowers the force but does not remove it. The fixes, in order of cost: thicken the wall to 1.5mm or more, pocket from solid stock leaving ribs at 2mm, or make it a sheet-metal bracket and bend the stiffness in, where 2mm sheet with a 1mm inside radius and a 6mm minimum flange does the same job.

A laser-cut bracket in 2mm sheet

A 2mm 5052 aluminum bracket carries a 1mm slot, a 3.5mm bridge between two cutouts, and 0.4mm inside corners. All three fail their rules: the slot is under 1× thickness, the bridge is under 2× thickness, and the corners are under 0.5mm. Corrected, the slot opens to 2mm, the bridge widens to 4mm, and the corners get 0.5mm radii. The bend that follows adds its own set: a 1mm minimum inside radius, a 6mm minimum flange, and 8mm between parallel bends.

A printed enclosure with 0.4mm walls and 1.5mm holes

An FDM enclosure is modeled at 0.4mm walls with 1.5mm ventilation holes. The walls sit under the 0.5 to 1.0mm floor and will extrude inconsistently, and the holes sit under the 2 to 3mm floor and will plug. Raise the walls to 1.0mm, print the holes at 3mm, and if 1.5mm holes are required for hardware, print them solid and drill after printing. If the enclosure carries load, remember the 20 to 30 percent Z-direction penalty and orient the print so the load sits in the print plane.

Design moves when you are under the floor

When a required feature sits below its floor, you have four moves. Thicken it to the floor, which is usually cheapest. Add ribs or gussets so a thin wall gets its stiffness elsewhere, the standard move in molding, where ribs beat thick sections on sink and cycle time. Move the feature to a secondary operation: print solid and drill, cast a core hole and tap it, machine a critical face after casting. Or change process: a part full of 0.5mm walls is telling you it wants to be sheet metal, and a part full of fine internal detail is telling you it wants to be printed.

A checklist for thin features

• Every wall is at or above its process floor, and load-bearing walls sit at the structural value, not the minimum.
• Holes are checked against the right rule: drill depth ratio for CNC, 1× thickness for laser, cored depth for casting, and 2 to 3mm for FDM.
• Inside corners carry a radius the tool can cut: 0.8mm or more for standard milled pockets, 0.5mm for laser corners.
• Sheet-metal bends respect the trio: radius 0.5× thickness, flange 3× thickness, bend spacing 4× thickness, with relief at acute corners.
• Molded and cast parts keep a uniform nominal wall, carry draft, and use ribs instead of thick sections.
• Printed parts are oriented so critical walls and holes print in the XY plane, with escape or drain holes for powder and resin.
• Any feature deliberately under the floor has its fix written on the drawing, so the shop knows the plan.