The 2026 CNC Design Guide for Production Engineers

CNC machining is still the workhorse of custom manufacturing in 2026 — every quote on Uretyco that involves metal almost always touches a milling or turning center somewhere. The cost difference between a clean DFM-ready part and a poorly toleranced one can easily be 2–4x. This guide is a pragmatic walkthrough of what actually moves the needle on price, lead time, and yield.

What CNC is genuinely good at

CNC excels at solid metal and plastic parts that need tight, repeatable tolerances and well-defined surface finishes. For volumes between one and a few thousand pieces, it remains the most cost-effective option for parts that cannot tolerate the variation of casting, the cosmetic limits of FDM, or the tooling cost of injection molding.

Functional metal prototypes that have to survive testing.
Production runs of 10 to ~5,000 pieces in aluminum, stainless, or engineering plastics.
Brackets, manifolds, fixtures, housings, mating components.
Anything that needs threaded features, sealed surfaces, or precision interfaces.

When CNC is the wrong tool

If your part is a thin shell with mostly cosmetic features, an additive process (MJF, SLS) or sheet metal is almost always cheaper. Use CNC for parts where geometry, strength, or surface accuracy matters more than complexity.

Tolerances and ISO 2768

On Uretyco we treat unspecified tolerances as ISO 2768-mK by default. This is the standard most reputable shops in our network design and inspect to. If a feature does not have a tolerance called out on the drawing, it falls under medium general tolerances for linear dimensions and fine for geometric form.

Linear range	Fine (f)	Medium (m)	Coarse (c)
0.5 - 3 mm	±0.05	±0.1	±0.2
3 - 6 mm	±0.05	±0.1	±0.3
6 - 30 mm	±0.1	±0.2	±0.5
30 - 120 mm	±0.15	±0.3	±0.8
120 - 400 mm	±0.2	±0.5	±1.2

Asking for tighter tolerances than you actually need is the single most common cost driver we see. A ±0.025 mm callout on a non-mating face can double the cost of a part because it forces an additional setup, slower feeds, and 100 percent inspection.

Wall thickness, pockets, and ribs

Thin walls deflect under cutting forces and chatter. A wall thinner than 0.8 mm in aluminum or 1.2 mm in steel becomes risky and may need a custom fixture. As a rule of thumb keep aspect ratios reasonable: pocket depth at most 4x its narrowest opening.

Material	Min wall thickness	Min pocket aspect ratio (depth:width)
Aluminum 6061-T6	0.8 mm	4:1
Stainless 304	1.2 mm	3:1
Steel 1018/4140	1.0 mm	3:1
Brass C360	0.6 mm	5:1
Delrin / POM	1.5 mm	3:1

Internal corners and fillets

Internal corners cannot be sharper than the cutter that machined them. If your drawing requires a sharp internal corner, a secondary EDM operation is needed and the cost rises sharply. The cheaper alternative is to keep internal corner radii at least one-third of the pocket depth.

Watch for hidden EDM

Square pockets with sharp internals usually trigger wire EDM. We will flag this on the platform during DFM, but designing it out from the start is much cheaper.

Threads, holes, and inserts

Tapped threads are inexpensive when they fit standard cutters. Threads smaller than M2 or longer than 3x the diameter become risky to tap and may snap a tool. Use heat-set inserts in plastics or threaded inserts in soft metals when the part must survive repeated assembly cycles.

Reach a minimum thread depth of 1.5x the diameter and a maximum of 3x the diameter.
Avoid threading into blind holes shorter than 1.5x diameter without a thread relief.
Use standard tap sizes: M2, M2.5, M3, M4, M5, M6, M8, M10. Custom pitches add cost.
Counterbores should clear the screw head plus 0.2 mm on radius.

Fixturing and setups

Most cost on a CNC quote is driven by the number of setups. Every flip of the part adds clamping time, re-zeroing, and inspection. A part that runs in two setups costs roughly half of one that needs four. Clearance for fixtures, datum surfaces, and tool reach should be planned during design — not after the quote arrives.

Surface finishes

By default Uretyco delivers an as-machined surface around Ra 1.6–3.2 µm with light deburring. Anything finer or cosmetic must be called out. The most common after-treatments and their typical add-on cost ranges are below.

Finish	Typical Ra	Cost adder	Best for
As-machined	1.6 - 3.2 µm	Baseline	Internal parts, prototypes
Bead blast	0.8 - 2.0 µm	+5-10%	Uniform matte appearance
Anodize Type II	Same as base	+10-25%	Aluminum cosmetic + corrosion
Anodize Type III (hard)	Same as base	+25-50%	Wear-critical aluminum
Powder coat	Cosmetic	+10-20%	Steel parts needing color
Mirror polish	<0.4 µm	+50-150%	Optical / sealing surfaces

Drawing package and file formats

STEP is the default 3D format. Send a 2D PDF drawing whenever a feature has a tighter tolerance than ISO 2768-mK, a critical surface finish callout, a thread specification beyond standard ISO, or any geometric tolerance. Without a drawing, we will quote the model assuming general tolerances and standard finishes.

1
Export STEP AP214 or AP242
Native CAD formats are accepted but STEP is universal across the supplier network.
2
Provide a flat 2D PDF
Title block, datums, critical dimensions, GD&T as needed, finish callouts, edge break, and material spec.
3
Specify finish and inserts
Anodize colors via RAL or sample, insert types and quantities as a BOM.
4
Upload to Uretyco
The platform runs topology analysis and surfaces any DFM concerns before the quote is final.

What Uretyco checks before the quote

When you upload a STEP and a PDF, our analysis engine inspects bounding box, volume, surface area, hole count and depths, internal corner minima, deepest pocket aspect ratio, and thread features. Anything that is likely to drive cost or risk is highlighted before the quote is finalized so you can adjust without losing time.

DFM is collaborative

Our AI co-pilot suggests changes (e.g. relax a tolerance, swap a wall thickness) but never edits your design. You decide what to apply. Quote updates are immediate.