Design for Manufacturing Guides | CNC, Sheet Metal, Molding

Guide 01 · 8 min read

CNC machining design rules

Most CNC cost comes from three things: how many setups a part needs, how long the tool is in the cut, and how many special tools are required. These rules keep all three low.

Solid carbide end mills of different sizes

Feature	Recommended	Why it matters
Internal corner radius	≥ 1/3 of cavity depth	End mills are round. A slightly larger radius than the tool lets it keep moving instead of stopping in the corner, which improves finish and tool life.
Cavity depth	≤ 4× cavity width	Long, thin tools deflect and chatter. Deep pockets need slower cuts or special tooling.
Wall thickness	≥ 0.8 mm metal · ≥ 1.5 mm plastic	Thin walls vibrate during cutting and may warp once released from the fixture.
Hole depth	≤ 4× diameter (standard)	Up to 10× is possible with peck drilling, but costs more. Use standard drill sizes where you can.
Thread length	≤ 3× diameter	Almost all thread strength is in the first 3 turns. Deeper threads add cycle time without adding strength.
Text & engraving	Engraved, ≥ 20 pt sans-serif	Engraved text is cut with one small tool. Embossed (raised) text removes far more material.
Undercuts	Standard widths: 3–40 mm	Undercuts need T-slot or dovetail cutters. Stick to standard sizes so we don't grind a custom tool.
Setups	Design for 1–2 orientations	Every re-fixture adds cost and a chance of misalignment. Group features on as few faces as possible.

Engineer's tipAdd a 0.5 mm chamfer instead of a fillet on external edges. A chamfer tool cuts every edge in one pass; external fillets need a ball mill and far more toolpath.

Guide 02 · 6 min read

Sheet metal fundamentals

Sheet metal parts are cut flat and then bent. Most problems come from features too close to a bend, where the metal stretches and distorts. Design from the material thickness (T) outward.

Feature	Recommended	Why it matters
Inside bend radius	≥ 1× T	Tighter radii crack harder alloys like 6061-T6. Use one radius across the part so a single tool forms every bend.
Minimum flange length	≥ 4× T	The flange must rest across the press-brake die opening to bend cleanly.
Hole to edge distance	≥ 2× T	Holes too near an edge bulge or tear during cutting and forming.
Hole to bend distance	≥ 2.5× T + bend radius	Closer holes stretch into ovals as the metal bends.
Minimum hole diameter	≥ 1× T	Smaller holes are possible on the laser but leave rough edges and heat marks.
Bend relief	Width ≥ T, depth ≥ radius + T	Relief cuts stop tearing where a bend meets an unbent edge.
Bend tolerance	±0.5° standard	Tighter angles are achievable with angle-measuring brakes but add inspection time.

Engineer's tipUse a hardware specification (PEM nuts, studs and standoffs) instead of tapped threads in sheet under 3 mm thick. They're stronger and cost less to install than tapping thin material.

Guide 03 · 7 min read

Injection molding essentials

A mold is a large up-front investment, so design changes after tooling are expensive. Getting walls, draft and ribs right before the tool is cut is the single biggest lever on part quality.

Feature	Recommended	Why it matters
Wall thickness	1.2–3 mm, uniform	Uneven walls cool at different rates, causing sink marks, voids and warp.
Draft angle	≥ 1° (≥ 3° on textured faces)	Draft lets the part release from the mold without drag marks or ejector damage.
Rib thickness	50–60% of wall	Thicker ribs leave visible sink marks on the opposite (cosmetic) side.
Rib height	≤ 3× wall thickness	Tall ribs are hard to fill and to eject.
Boss outer diameter	2× screw diameter	Connect bosses to walls with ribs instead of thickening them.
Corner radius	Inside ≥ 0.5× wall	Sharp corners concentrate stress and restrict material flow.
Undercuts	Avoid, or plan side actions	Each side action or lifter adds tool cost and maintenance.

Engineer's tipAsk for a mold-flow analysis before steel is cut. We include one free with every production tool. It shows weld lines, air traps and warp before they cost you a tool modification.

Guide 04 · 5 min read

Designing for additive

Additive frees you from tool access, but it introduces its own rules around overhangs, supports and powder removal.

Feature	Metal (DMLS)	Polymer (SLS / MJF)
Minimum wall	0.4 mm	0.8 mm
Self-supporting overhang	≥ 45° from horizontal	No supports needed
Minimum hole	0.5 mm	1.5 mm
Escape holes (hollow parts)	≥ 2 × Ø3 mm	≥ 2 × Ø5 mm
Typical tolerance	±0.1 mm + 0.1%	±0.3 mm + 0.3%
Post-machining	Leave 0.5 mm stock on critical faces	Rarely needed

Guide 05 · 5 min read

How tight is too tight?

Over-tolerancing is the most common cost driver we see. Every extra decimal place means slower cutting, more inspection and sometimes a different machine. Tighten only the features that need it, and let a general tolerance block cover the rest.

Tolerance	Typical use	Relative cost
±0.25 mm	Non-critical external features, clearance holes	1.0×
±0.10 mm	Our standard. Most mating features	1.0×
±0.05 mm	Locating features, press-fit bores	1.2–1.5×
±0.025 mm	Bearing seats, precision alignment	1.5–2.5×
±0.005 mm	Optical, metrology, valve spools. Often needs grinding	3–5×

Engineer's tipUse GD&T position tolerances for hole patterns instead of tight ± dimensions on each hole. A ±0.05 mm square zone rejects good parts at its corners; a Ø0.14 mm position zone accepts the same worst-case corners and gives 57% more usable area, at no loss of function.

Guide 06 · 4 min read

Choosing a surface finish

Finishes protect parts and set how they look and feel. Remember that coatings add thickness, so critical dimensions may need masking or adjusted machining.

Finish	Materials	Thickness added	Best for
As machined	All	0	Prototypes, internal parts. Ra 3.2 µm typical
Bead blast	All metals	0	Uniform matte look, hides tool marks
Anodize Type II	Aluminum	5–25 µm	Color, corrosion protection, consumer products
Anodize Type III	Aluminum	25–75 µm	Wear resistance, aerospace and defense
Passivation	Stainless steel	0	Medical and food contact, corrosion resistance
Powder coat	Steel, aluminum	50–150 µm	Durable color on enclosures and frames
Electroless nickel	Steel, aluminum, copper	5–25 µm	Uniform hard coating, even in bores

Reference

Manufacturing glossary

DFM: Design for Manufacturing. Reviewing a design to make it easier and cheaper to produce without changing its function.
FAI (AS9102): First Article Inspection. A full measurement of the first production part against every drawing requirement.
CMM: Coordinate Measuring Machine. A precision probe that measures part geometry in 3D, often to within a few microns.
PPAP: Production Part Approval Process. The automotive standard for proving a process can consistently make good parts.
CoC: Certificate of Conformance. A signed statement that parts meet the order and drawing requirements.
Cpk: Process capability index. Shows how well a process stays within tolerance. 1.33 or higher is generally considered capable.
GD&T: Geometric Dimensioning and Tolerancing. A symbolic language for defining form, orientation and position on drawings.
Ra: Average surface roughness, in micrometers. Lower is smoother. Ra 0.8 µm feels smooth; Ra 0.1 µm looks like a mirror.
T1 sample: The first parts shot from a new injection mold, used to verify the tool before production.
Lights-out machining: Automated machining that runs unattended overnight, lowering cost and lead time.

Design for manufacturing.

CNC machining design rules

Sheet metal fundamentals

Injection molding essentials

Designing for additive

How tight is too tight?

Choosing a surface finish

Manufacturing glossary

Your next part is 24 hours from a real quote.