DFM Guide: 10 Principles for CNC Machined Parts

Most CNC machining cost and quality problems are created before a machine is programmed. This design for manufacturability guide for CNC machining covers ten specific design decisions — tolerances, setups, corner geometry, wall thickness, holes, surface finish, materials, datums, and threading — that consistently affect machinability, repeatability, and total production cost. They apply across materials and across industries.

The principles are most valuable when reviewed early. A tolerance change at the drawing stage costs nothing. The same change after first article costs significantly more.

DOWNLOAD DFM GUIDE (.PDF) >>

Principle 1: Specify Only the Tolerances the Application Requires

A reasonable general tolerance for CNC machined features is ±0.005″ (±0.127 mm) for most non-critical dimensions — a starting point consistent with standard commercial CNC practice. Every tolerance tighter than this range may require different process approaches: different workholding strategies, tighter thermal control, alternative finishing sequences, or more intensive inspection. The specific implication depends on geometry, material, machine capability, and the nature of the feature.

Before specifying a tight tolerance, confirm the functional consequence of being at the edge of that tolerance band. If the part still functions at the limit, the tolerance may be unnecessarily tight.

GD&T (Geometric Dimensioning and Tolerancing) is most useful where functional feature relationships, datum structures, orientation, and location all need to be controlled simultaneously. It communicates functional intent more precisely than coordinate tolerancing in those situations and can offer more manufacturing latitude than coordinate tolerances suggest — but it is not categorically superior for every part.

Principle 2: Design for the Fewest Possible Setups

Each time a part is repositioned in a machine, variation can accumulate and labor cost increases. Features that can be reached from the same direction should be grouped to complete in one setup where possible.

5-axis machining can complete complex geometry — compound angles, multiple intersecting features — in fewer setups than 3-axis machining. The specific reduction depends on part geometry, but consolidating setups through machine capability is a legitimate cost-reduction strategy worth evaluating during design. The setup reduction can offset the higher machine rate.

When multiple setups are unavoidable, design clear reference surfaces into the part that support consistent repositioning. A part that can be re-established consistently from controlled locating features is substantially easier to hold to tolerance across operations.

Principle 3: Specify Internal Corner Radii Larger Than the Tool Radius

Internal corners on machined parts cannot be perfectly sharp. A rotating end mill leaves a minimum radius equal to its own radius. However, specifying a corner radius exactly equal to the tool radius forces the cutter into full radial engagement at the corner — increased cutting forces, heat generation, and deflection risk, and the least efficient cutting condition. The corner radius should be larger than the tool radius to allow the cutter to clear the corner with controlled engagement.

A practical starting point: specify internal corner radii at approximately 1.25× to 1.5× the cutter radius; larger radii are preferred where geometry allows. For a pocket to be machined with a 1/4″ (0.250″) end mill, the cutter radius is 0.125″. Specifying a corner radius of 0.156″–0.188″ allows the tool to clear the corner cleanly rather than plunging into full engagement. A corner radius specified exactly at 0.125″ in this example does not provide that clearance.

End mills are available in a wide range of diameters — below 1/8″ for fine detail work through 1″ and larger for heavy roughing. Present the tool range to your machining partner early in design if internal geometry is complex, as the achievable corner radius depends on tool availability and the geometry of the specific pocket.

Principle 4: Observe Minimum Wall Thickness Guidelines

Thin walls flex under cutting forces, causing chatter, dimensional variation, and potential damage. The following values are starting-point guidelines — actual minimums vary with wall height, material condition, geometry, cutter engagement, workholding, machine rigidity, and the tolerance required on the wall feature:

Aluminum: 0.025″–0.040″ for short, well-supported walls; progressively thicker for taller unsupported sections
Steel: 0.050″–0.060″ as a reasonable starting point for most geometries
Titanium and nickel-based alloys: Higher minimums apply due to substantially greater cutting forces

The ratio of unsupported height to wall thickness matters as much as the absolute dimension. A 0.040″ wall at 0.200″ of unsupported height behaves very differently from the same wall at 1.000″ of unsupported height. Where thin walls are functionally required, discuss the geometry with your machining partner during design. Minor geometric changes can sometimes improve stability without changing the functional envelope.

Principle 5: Consider Hole Depth-to-Diameter Ratios in Tooling Selection

As a planning reference for conventional tooling, hole depths of approximately 3× to 5× the drill diameter are typical before chip evacuation and heat management become more demanding. The appropriate method — peck drilling, continuous feed with through-coolant, or specialized deep-hole tooling — depends on the drill type, material, diameter, coolant delivery, and chip formation characteristics, not on a single depth threshold.

Modern carbide drills with through-tool coolant can often be run continuously at substantially greater depth-to-diameter ratios without pecking. Specialized gun drills are designed for very deep holes — 10× diameter and beyond — in suitable applications. The 3×–5× range is a useful planning reference for conventional tooling, not a ceiling for all drilling.

Where possible, specify through-holes rather than blind holes. Through-holes are easier to drill, easier to inspect, and eliminate blind-hole depth tolerance as a variable. Counterbores for fastener heads are generally more cost-effective than recesses with tight depth or diameter tolerances.

Principle 6: Avoid Undercuts Unless Functionally Required

An undercut is any feature that cannot be reached by a standard end mill moving axially — a groove, channel, or recess that faces away from the machining direction. Undercuts require alternative tooling or approaches: T-slot cutters, lollipop (back-turning) cutters, form tools, or additional setups in which the part is repositioned to access the feature from a different angle.

Each of these adds cost disproportionate to the feature’s typical size. Where an undercut is genuinely required — for a snap-fit groove, a sealing channel, or a specific assembly interface — specify it explicitly and verify that the geometry is compatible with available standard tooling. Custom form tools add lead time and cost.

In many cases, an undercut is present because a design was carried over from a casting or a different manufacturing process. Review whether the feature is still functionally required in the machined version of the part.

Principle 7: Specify Surface Finish by Functional Requirement

Surface finish specifications affect cost. Finer finishes require additional machining passes, slower feeds and speeds, or in some cases secondary operations. Applying a fine finish callout uniformly across an entire part — when only specific features require it — is a common source of unnecessary cost.

The following Ra values (in microinches) are directional manufacturing benchmarks, not application prescriptions. Bearing, sealing, and interface requirements vary with seal type, lubrication, material pair, relative motion, and application-specific standards:

125 Ra: A commonly achievable reference finish from conventional milling or turning.
63 Ra: An improved finish often achievable with careful finish passes. Appropriate as a starting benchmark for many interface surfaces.
32 Ra: A fine finish. Often achievable by conventional finish turning or milling under appropriate conditions. Some applications may require dedicated finishing operations.
16 Ra and below: Frequently requires additional operations such as grinding, lapping, or precision hard turning, depending on material and geometry.

Apply surface finish callouts to specific features based on their confirmed functional requirement, not as a blanket specification in the title block. Where a general note appears on a drawing, review whether every surface on the part genuinely needs that finish.

Principle 8: Consider Machinability Alongside Function in Material Selection

Material choice drives cycle time, tooling cost, and surface finish achievability. When two materials can satisfy the functional requirement, machinability is a real cost consideration. The following observations are general guides — actual cycle times depend on geometry, removal rate, tooling, and machine capability:

Aluminum alloys: 6061-T6 is among the most machinable common engineering alloys — fast cycle times, good surface finish. 7075 machines well but requires more care at feed and speed selection.
Stainless steel: 303 stainless steel machines significantly better than 316 due to the sulfur addition in its chemistry. However, that same sulfur addition reduces corrosion resistance and toughness compared to 316. If corrosion resistance is the primary design requirement, 316 or another high-corrosion-resistance grade may be the correct choice despite the machinability difference.
Carbon and alloy steel: 1018 and 1045 machine well. 4140 is machinable in commonly machined hardness and heat-treatment conditions; machinability changes materially at higher hardness levels.
Titanium (Ti-6Al-4V): Requires slower speeds, specialized carbide tooling, and careful heat management. Cycle times are substantially longer than aluminum and longer than most steel grades.
Nickel-based superalloys (Inconel, Hastelloy, Waspaloy): Work-harden during cutting, require premium tooling, and have significantly higher machining costs than steel. Understanding the machining implications early avoids cost surprises when nickel superalloys are specified.

Material selection is an engineering decision driven by function. The note here is that machinability is one of the variables worth considering alongside strength, corrosion resistance, and weight when two materials could satisfy the requirement.

Principle 9: Define Datum Features Based on Function and Accessibility

Datum features are the reference framework for both fixturing during machining and measurement during inspection. Effective datum features are not limited to flat surfaces — they may be flat surfaces, cylindrical features (such as bores or pins), slots, or patterns, each establishing a datum through physical contact or through derived geometry such as an axis or plane. The defining quality of a well-chosen datum is that it accurately reflects the part’s functional relationship to its assembly while remaining accessible and stable enough for fixturing and inspection.

The primary driver of datum selection should be functional design intent — the datum should represent how the part locates in its assembly. Accessibility for fixturing and inspection is a secondary but important practical consideration. When possible, machine datum features and the features referenced to them in the same setup, as this reduces the variation introduced by repositioning — but this should not override functional datum selection.

Datums that are inaccessible, unstable under fixturing load, or difficult to measure add setup time and inspection uncertainty. A brief conversation with your machining partner about datum accessibility early in design often prevents problems at first article.

Principle 10: Use Standard Thread Forms and Specify Inserts for High-Cycle Assemblies

Non-standard thread forms and pitches require custom taps and inspection gauges and complicate lead times. Standard Unified Coarse (UNC), Unified Fine (UNF), and metric thread forms use off-the-shelf tooling and can be inspected with standard gauges.

Between coarse and fine threads:

Coarse threads (UNC or coarse metric) are generally preferred for rapid assembly, tolerance of minor handling damage, use in soft materials, and resistance to cross-threading. They are more tolerant of contamination and cross-threading and are generally faster to assemble.
Fine threads (UNF or fine metric) offer tighter preload control and, due to their smaller helix angle, can be more resistant to vibrational loosening in some applications. Fine threads are better suited to thin-walled sections and precision adjustment.

Neither thread form is categorically superior in vibration resistance — application-specific fastener engineering should determine the appropriate choice.

In aluminum or soft materials subject to repeated assembly and disassembly, specify thread inserts (Helicoil, Keensert, or equivalent). The host thread engagement is larger, the insert material is harder and more durable, and a damaged insert can often be replaced without scrapping or extensively reworking the parent component.

Thread engagement depth is application-dependent. A commonly cited starting-point guideline for steel fasteners into aluminum is 1.5× to 2× the thread diameter, but appropriate engagement depends on aluminum alloy, thread class, loading, and whether thread inserts are used. Published references and application-specific fastener analysis should be used to confirm engagement requirements for structurally loaded joints.

Applying This DFM Guide to CNC Machining Projects

These ten principles do not all apply to every part. A simple turned component may involve only a few of them. A complex 5-axis aerospace housing may touch all ten.

The value of a DFM review is in knowing which principles apply to a specific design — and catching the ones that create unnecessary cost or risk before the drawing is released. That review is most useful at the concept or first-revision stage, before tooling is ordered or first articles are in process.

Borg Design’s engineering team, including registered mechanical engineers, reviews drawings for manufacturability during the normal quoting process. If a design decision is likely to create production challenges, we raise it before committing to a price — not after the first article reveals the problem.

To discuss a specific part or program, submit an RFQ → or contact our engineering team →

Frequently Asked Questions

Q: What is design for manufacturability (DFM)?

A: Design for manufacturability is the process of evaluating a part’s design to identify features, tolerances, materials, or geometry choices that create unnecessary manufacturing cost or risk — and addressing those decisions before the drawing is released. Effective DFM review reduces cost, improves repeatability, and reduces the likelihood of first-article and production problems.

Q: When in the design process should a DFM review happen?

A: The earlier, the better. A DFM review is most valuable at the concept or first-revision stage, when changes are low-cost. By the time tooling is ordered or first articles are in production, the cost of design changes increases significantly. At minimum, a DFM review should occur before a drawing is released to a machining supplier for quoting.

Q: Does DFM mean compromising the design?

A: No. DFM is about preserving the design’s functional intent while reducing unnecessary manufacturing complexity. A good DFM review does not change what the part needs to do — it identifies tolerances that are tighter than the function requires, features that create avoidable setups, and material or finish specifications that add cost without adding performance.

Q: What is the difference between DFM and design for assembly (DFA)?

A: DFM focuses on how a part is manufactured — tolerances, features, materials, and processes. DFA focuses on how parts fit together in an assembly — fastening methods, clearances, part count, and assembly sequence. In precision machined assemblies, DFM decisions frequently affect DFA outcomes: a feature location that simplifies machining may also affect assembly.

Q: Which industries benefit from DFM review?

A: DFM principles apply across all industries that use CNC machined components, including aerospace, defense, medical device, automotive, and industrial manufacturing. The stakes are higher in regulated industries where first-article testing and qualification cycles are long, but the cost impact of DFM decisions exists in every machining program.