Minimum Radius and Wall Thickness

Two design rules cause most manufacturability problems on CNC parts: internal corner radius and wall thickness. Both come from the same root cause, designing for the geometry on screen rather than for the tool that has to cut it. This guide explains the physics, the numbers to design to, and what OpusFab flags automatically.

Why sharp internal corners are impossible

A CNC end mill is a cylinder. It removes material by spinning and travelling along a programmed path, and the round tool physically cannot reach into the intersection of two walls. Every internal corner ends up with a radius that matches the tool, no matter what you drew.

The corner radius you can achieve equals the radius of the end mill used. A 0.5 mm internal corner requires a 1.0 mm diameter tool. A 0.2 mm radius requires a 0.4 mm tool, which is micro-machining territory.

Small tools are the problem. An end mill’s rigidity scales with the fourth power of its diameter, so a 1.0 mm tool is a fraction as stiff as a 6.0 mm tool, and a 0.4 mm tool barely functions in production aluminium. To keep a tiny tool alive the machinist cuts feed rate and depth so far that machining time multiplies, and the tool may still snap. That cost lands in your quote.

The 0.5 mm rule

The practical minimum internal corner radius for standard CNC machining is 0.5 mm, which corresponds to a 1.0 mm end mill, the smallest tool most shops run without a micro-machining surcharge. Where you can, go larger: a 1.0 mm radius allows a 2.0 mm tool at full production speed.

OpusFab’s DFM analysis extracts the minimum internal radius from your STEP file on upload. If it falls below the 0.5 mm warn threshold, the part gets a DFM Warning pill in the quote table. The part can still be quoted and ordered, but the warning means the price reflects a harder machining job. See DFM overview.

How to fix tight internal corners

• If the corner is cosmetic or a CAD default: increase the fillet to 1.0 mm or more. This is the fastest way to cut your CNC quote.
• If you need clearance for a square component: use a dog-bone or T-bone fillet so a round tool can clear the corner of the pocket.
• If the corner must be truly sharp: it needs a secondary operation such as wire EDM or broaching. Request a custom quote and expect extra cost and lead time.

Why thin walls fail

A spinning cutter applies serious force to the workpiece. A thick wall resists it; a thin wall flexes and vibrates, producing chatter marks, poor surface finish, dimensions that drift out of tolerance, and in bad cases a broken part. If a wall is thinner than the tool cutting it, the tool pushes the wall aside instead of cutting it.

CNC minimum wall thickness by material

These are practical minimums for unsupported walls (free-standing on at least one side). Walls supported on both ends can go thinner:

Material	Minimum wall thickness
Aluminium (6061-T6, 7075-T6)	0.8 mm
Steel	1.0 mm
Stainless steel	1.5 mm
Titanium	1.5 mm
Engineering plastics (POM, ABS)	0.5 to 0.8 mm

OpusFab estimates wall thickness from your part geometry on upload and warns when the estimate falls below roughly 0.6 mm. Thickening the wall and re-uploading removes the warning and usually drops the price, because the part can be cut at normal parameters.

How to fix thin walls

• Thicken the wall. Going from 0.4 mm to 1.0 mm can reduce machining cost substantially.
• Add ribs. Short perpendicular ribs stiffen a thin wall at almost no extra machining cost.
• Use a pocket instead of a through-slot. A slot creates two thin walls; a pocket leaves a solid floor that keeps the part rigid.
• Split the part. Two machinable components that assemble together can replace one unmakable thin-walled part.

Wall thickness for 3D printed parts

Printed walls do not face cutting forces, so the constraint is strength and printability rather than vibration. As a rule of thumb, keep walls at about 1 mm or above for SLA resin and SLS nylon; thinner walls get fragile and can warp. See CNC vs 3D printing design rules.

Checklist before you upload

• Internal corner radii are 0.5 mm or larger, ideally 1.0 mm.
• Unsupported walls meet the material minimums in the table above.
• Deep pockets stay within about 4:1 depth to width ratio.
• The STEP file is exported in millimetres at the correct scale.

Pass this checklist and your parts should quote without DFM warnings.