CNC Machining Design Guide

Designing for CNC machining is not just about creating a geometrically correct model — it's about creating a model that can be manufactured efficiently, accurately, and affordably. This guide distills the most important design-for-manufacturability (DFM) rules that will save you time, cost, and engineering change orders.

Whether you are designing enclosures, brackets, precision instruments, or production hardware, following these rules ensures your parts arrive right the first time — without unnecessary back-and-forth or machining holds.

Internal Corner Radii

This is the single most important rule in CNC machining design. A rotating end mill has a circular cross-section — it cannot cut a perfectly sharp internal corner. Every internal corner on a milled pocket will have a radius equal to at minimum the radius of the cutter used.

The 130% rule

Specify corner radii at least 130% of the end mill radius that will enter the pocket. This gives the tool clearance to sweep through the corner without full-engagement chatter.

Relief options for sharp corners

If your design requires a sharp internal corner (e.g., for a mating square key or insert), use one of these relief strategies instead of specifying a zero-radius corner:

• Dogbone A circular relief at each corner sized to the cutter radius. Allows a square part to seat fully into the pocket.
• T-Bone Relief extends in one direction only — useful when one wall is the reference datum.
• Tear-Drop A small teardrop-shaped relief — cosmetically cleaner than dogbone but slightly less clearance.

Wall & Floor Thickness

Thin walls and floors vibrate during machining — a phenomenon called chatter. When the cutter engages a thin section, the material deflects away from the tool, springs back, and re-engages, producing a rough surface, dimensional error, and audible vibration. Below certain thresholds, the part may physically deform or crack.

Wall height-to-thickness ratio

Even if a wall meets the minimum thickness, excessively tall thin walls are prone to deflection. As a guideline:

• Aluminum: Wall height should not exceed 15× wall thickness
• Steel: Wall height should not exceed 10× wall thickness
• Plastics: Wall height should not exceed 8× wall thickness

Pocket Depth-to-Width Ratios

Deep narrow pockets require long, slender end mills that deflect under cutting loads. Tool deflection causes dimensional error, poor surface finish, and risk of tool breakage — which can damage the part.

Floor radius

Pocket floors will have a small radius where the floor meets the wall — determined by the cutter's corner radius or ball-nose profile. Specify a floor radius ≥ 0.010″ to allow standard tooling. If you need a truly flat floor-to-wall intersection, call it out explicitly and expect added cost.

Holes & Threads

Standard drilled holes

Standard twist drills produce holes in standard fractional, letter, or number sizes. Specifying standard sizes ensures the shop has the drill in stock and avoids custom tooling.

• Minimum diameter: 0.020″ (technically possible); prefer ≥ 0.060″ for reliability
• Maximum depth: 10× diameter for standard drills; deeper requires peck drilling or gun drills
• Tolerance: Standard drilled holes are ±0.003″; for tighter fits, specify reaming

Reamed holes

When you need precision bore diameters for dowel pins, bearings, or slip-fit assemblies, call out a reamed hole with an H7 tolerance (+0.000/+0.001″). Reaming adds one operation but guarantees roundness and size.

Tapped (threaded) holes

Always specify: diameter, pitch, class of fit, thread depth, and total hole depth separately.

Common thread sizes

Undercuts

An undercut is any feature that is not accessible from a straight tool-down (Z-axis) approach. Undercuts require either:

• 5-axis machine — tilts the spindle to reach the feature
• Specialty cutters — T-slot mills, lollipop cutters, or dovetail mills
• Additional setups — flip the part and re-fixture

All three options add cost. If the undercut is purely cosmetic, consider whether a chamfer or stepped geometry achieves the same visual result at far lower cost.

O-ring grooves & internal channels

Internal O-ring grooves on bore walls are a common undercut. These can be machined with a T-slot cutter or on a lathe. Always specify groove width, depth, and the O-ring dash number so the shop can verify fit.

Draft Angles

Unlike injection molding, CNC machining does not require draft angles. Milled walls can be perfectly vertical (0° draft). However, there are cases where a small draft is beneficial:

• Deep pockets: A 0.5°–1° draft on deep pocket walls allows easier chip evacuation and reduces tool engagement pressure
• Mold cavities: If your machined part is a mold or die, incorporate draft for the molded part's release — typically 1°–3°
• Tapered fits: Morse tapers, alignment cones, and self-centering features use intentional draft/taper

Tolerances

Tolerance is the allowable deviation from a nominal dimension. Specifying tighter tolerances than necessary adds cost without benefit — every feature at ±0.001″ means every feature gets individually inspected.

Geometric tolerances (GD&T)

When positional relationships, flatness, or perpendicularity matter more than a simple ± on a dimension, use GD&T controls. CNC milling readily achieves:

• Flatness 0.001″ – 0.003″ on a faced surface
• Perpendicularity 0.002″ per inch of wall height
• True Position ⌀0.005″ at MMC for drilled patterns
• Cylindricity 0.001″ on reamed bores

Surface Finish

Milled surfaces have a characteristic scallop pattern from the rotating cutter. Roughness is quantified as Ra (arithmetic average). Finer finishes require lighter cuts, slower feeds, and more passes — increasing cycle time and cost.

Anodizing & coatings

• Type II anodize adds 0.0002″ – 0.0004″ per side. Account for this in precision bores.
• Type III (hardcoat) adds up to 0.001″ per side. Machine tight holes undersized to compensate.
• Break all sharp edges (0.010″ – 0.020″ chamfer) before anodizing to prevent coating burn-through.

Material Selection

Material choice directly impacts machinability, cost, lead time, and available finishes. Here are the most common materials for CNC machining:

Aluminum alloys

• 6061-T6 General-purpose workhorse. Excellent machinability, anodizes well. Use for enclosures, brackets, structural frames.
• 7075-T6 High-strength aerospace alloy. Harder, higher cost. Use where 6061 isn't stiff enough.
• MIC-6 Cast tooling plate. Exceptional flatness. Ideal for fixture plates and optical breadboards.

Steel alloys

• 1018 Low-carbon, free machining. Good for fixtures and non-critical parts.
• 4140 Chromoly — strong, tough, heat-treatable. Shafts, gears, die sets.
• A2 / D2 Tool steels. Very hard after heat treat. Slow to machine; specialty only.

Stainless steel

• 303 Best machinability in stainless family. Good for parts that don't need welding.
• 304 Standard food-contact and corrosion-resistant grade.
• 316 Marine/chloride resistance. Harder to machine; specify when exposure demands it.

Engineering plastics

• Delrin (POM) Low friction, dimensionally stable. Great for gears and bushings.
• PEEK High-temp, chemical-resistant. Expensive; use when metal is too heavy or conductive.
• UHMW Ultra-low friction, impact-resistant. Slides, wear strips.

CAD & File Preparation

Clean, complete files are the fastest way to reduce quoting time and avoid manufacturing holds.

Accepted formats

• .STEP Preferred — preserves solid geometry faithfully across all CAM systems
• .IGES Acceptable; verify surface normals and check for gaps
• .SLDPRT Native SolidWorks accepted with full feature tree

Model checklist

• Model threaded holes as plain holes — call out thread spec on the drawing only
• All corner radii present and dimensioned — don't leave sharp corners for the machinist to guess
• Final part geometry only — do not include machining stock in the model
• Confirm model units (inches vs. mm) in order notes
• Tight-tolerance features called out in an accompanying PDF print or MBD

Drawing best practices

Even in a model-based workflow, a 2D PDF drawing eliminates ambiguity. Include at minimum:

• Title block with part number, revision, date, and drawn-by
• General tolerance block (e.g., .XXX ±.005, .XX ±.010, angles ±0.5°)
• Material spec with alloy and temper (e.g., Aluminum 6061-T6 per AMS-QQ-A-200/8)
• Finish specification and masking notes
• Critical dimensions with explicit tolerances