Introduction
A drawing that looks clean in CAD can be a manufacturing nightmare on the shop floor. Designers who understand machining capabilities design parts that can be produced accurately, repeatably, and economically. Those who do not incur avoidable costs through special tooling, extended cycle times, multiple setups, and scrap. The gap between a machinable design and an unmachable one is often a single feature—an internal corner radius too small for available tooling, a depth-to-diameter ratio that causes tool deflection, or a tolerance that could be relaxed by 0.05 mm without affecting function.
This guide covers the practical capabilities and limitations of CNC milling and turning—the two most common machining processes—and provides design rules derived from actual production experience.
CNC Milling Capabilities and Limitations
Internal Corner Radii
The most common machinability error in milled parts is specifying sharp internal corners in pockets and slots. A milling cutter is cylindrical—it cannot produce a perfectly square internal corner. The minimum internal corner radius equals the radius of the end mill used. Standard tooling: 3 mm corner radius is achievable with a 6 mm end mill; 1 mm corner radius requires a 2 mm end mill that is fragile and slow.
Design rule: specify the largest internal corner radius functionally acceptable. In most cases, 3–5 mm corner radius is acceptable and allows robust tooling. If a mating part must fit into a corner, chamfer the mating part’s corner rather than forcing the machined pocket to have a sharp internal corner. Add corner relief features (circular pockets at corners) only when corner radius cannot be increased due to functional constraints.
Pocket Depth and Wall Thickness
Deep pockets require long-reach end mills which deflect under cutting forces, causing dimensional error, poor surface finish, and shortened tool life. General guidance: pocket depth should not exceed 3× the end mill diameter for good results; 4× is achievable with reduced feed rates; beyond 5× requires special tooling and extended cycle times.
Thin walls in pocketed parts deflect during machining, vibrate, and may spring after release from clamping. Minimum recommended wall thickness: aluminum 0.8–1.0 mm; steel 1.5–2.0 mm. Walls thinner than these values can be machined but require special fixturing and reduced cutting parameters.
Hole and Slot Features
Drilled holes have a practical depth limit of approximately 5–8× diameter with standard drill bits before step-drilling or gun drilling is required. For deep holes beyond this range, cost increases significantly. Holes with depth greater than 10× diameter are specialty operations.
T-slots and undercuts cannot be produced with standard end mills—they require T-slot cutters or dovetail cutters with limited reach and fragile geometry. Avoid undercuts unless they provide essential functional value. If required, design them on accessible faces with generous cutter entry space.
Surface Accessibility and Fixturing
A CNC machining center can only cut what the spindle can reach with the part fixtured in a given orientation. Complex parts requiring machining from more than 4 directions require multiple setups, each with its own fixturing cost and potential for cumulative positioning error. Design for minimum setups: orient all critical features so they can be machined from 3 faces or fewer; locate reference surfaces (datum faces) that allow consistent repositioning between setups.
CNC Turning Capabilities and Limitations
Turned Part Geometry
CNC turning produces surfaces of revolution. The fundamental constraint is that all features must be accessible from the ends or outer diameter of a rotating part. Internal features (bores, internal grooves, undercuts) are accessible from the chuck face. Radial features (cross holes, flats, keyways) require a live tooling turret or a second operation in a machining center.
Length-to-diameter ratio: for stable turning, L/D ratio should not exceed 4:1 without a tailstock and 8:1 with tailstock support. Long slender parts chatter, producing poor surface finish and dimensional error. If L/D exceeds these limits, consider whether the part can be made shorter, whether diameter can be increased, or whether alternative machining methods are appropriate.
Undercuts and Form Tools
Internal and external undercuts on turned parts require form tools or grooving operations. They add cost but are often necessary for retaining rings, O-ring grooves, and thread relief. Design undercuts to standard dimensions matching available tooling: common O-ring groove widths, standard snap ring groove dimensions. Non-standard groove dimensions require custom tooling.
Tolerance and Surface Finish Economics
Tolerance drives cost more than any other single design parameter. The relationship is non-linear: tolerances of ±0.1 mm are achieved routinely in a single operation; ±0.05 mm requires careful fixturing and possibly a light finish pass; ±0.02 mm may require grinding or lapping after machining; ±0.005 mm is a precision grinding operation that costs an order of magnitude more than a milled feature.
Design rule: specify the tolerance that functional requirements actually demand, not the tightest the designer can imagine. Review every tight tolerance on a drawing and ask: what breaks if this is 0.05 mm wider? If nothing breaks, relax the tolerance. The manufacturing cost saving is real and significant.
Summary Table
| Feature | Standard Capability | Limit / Constraint | Cost Impact if Exceeded |
|---|---|---|---|
| Internal corner radius (milling) | R3–5 mm | Min = cutter radius | Smaller cutter, reduced speed, higher cost |
| Pocket depth-to-width ratio | Up to 3:1 | Max 5:1 with special tooling | Reduced feeds, tool deflection, scrap risk |
| Drilled hole depth-to-dia ratio | Up to 8:1 | Beyond 10:1 = gun drilling | Specialty process, high cost |
| Turned L/D ratio | 4:1 (no tailstock) | 8:1 (with tailstock) | Chatter, poor finish, scrap |
| Tolerance (milled) | ±0.05–0.1 mm routine | ±0.01 mm = grinding needed | Exponential cost increase below ±0.02 mm |
| Setup count | 1–3 setups | Each additional setup = cost + error risk | +20–50% per additional setup |
FAQ
Q: The designer wants a sharp internal corner for a functional fit. What are the options?
A: There are three practical approaches. First, add a corner relief—a small circular pocket at the corner that allows a standard end mill to clear the corner while the mating part fits against the walls. Second, use EDM (electrical discharge machining) which can produce sharp internal corners but at significantly higher cost. Third, redesign the mating interface so the corner is in the mating part rather than the machined pocket (add a chamfer or radius to the mating part to clear the internal fillet). In most cases, option three is the best engineering solution.
Q: How do I communicate machinability requirements to the design team without slowing down their work?
A: Develop a one-page design-for-machinability (DFM) checklist specific to your shop’s capabilities and distribute it to all designers. Common items: minimum internal corner radius, minimum wall thickness by material, maximum aspect ratios for pockets and holes, tolerance guidelines by process. A brief DFM review at the 50% drawing stage (not at the final release) catches most problems before they are locked into the design. Most designers are receptive when the feedback is presented as cost data rather than criticism.
Q: We outsource machining. How do we ensure our drawings are machinable by external suppliers?
A: Request design feedback from your supplier during the quoting stage, before purchase order. Most shops will flag machinability issues if given the opportunity and will not charge for doing so—they prefer to quote jobs they can make profitably. Establish a standard drawing note that invites suppliers to flag manufacturability concerns before acceptance. This creates a communication channel without requiring your team to become machining experts for every material and operation.
コメント