NEWS

Understanding the physical limits of CNC machining is the first step for engineers and procurement specialists looking to reduce costs. DFM—Design for Manufacturability—addresses precisely this issue: integrating machining feasibility into the design phase rather than waiting until the blueprints reach the factory to discover problems. Milling cutters are round; they cannot cut perfect square corners. Tools with excessive overhang will vibrate. Thin walls will deform during the machining process. These are all governed by physical laws, not by a manufacturer's lack of skill.

Aluminum itself possesses excellent machinability, offering designers a significant margin for error; however, this margin is not infinite. Each of the 10 rules outlined below is backed by practical machining principles. By understanding them, you can eliminate hidden costs during the design phase.

 

Rule 1: Avoid Deep, Narrow Slots Whenever Possible; If Unavoidable, Control the Aspect Ratio

Deep, narrow slots are among the features CNC operators are most reluctant to tackle. The reason is simple: the deeper the slot, the further the cutting tool must extend; and the longer the tool extension, the lower its rigidity. This is analogous to using chopsticks to pry something open—the longer the lever arm, the more the rigidity naturally diminishes.

In quantitative terms, an aspect ratio (Length/Width) exceeding 4:1 enters the "high-risk zone," while anything over 6:1 is essentially asking for trouble. The same applies to deep cavities: tool vibration becomes noticeable when the depth exceeds four times the tool diameter, and depths exceeding six times the diameter are classified as "deep cavity machining."

Why does this issue significantly increase costs? Because tools with long overhangs require slower speeds and feed rates, thereby extending machining time. Furthermore, once a tool begins to vibrate, the resulting surface finish may fail to meet specifications, potentially necessitating rework or even leading to part scrap.

If your design absolutely requires deep slots, consider a split design approach—dividing the part into two separate components that can be machined independently and then assembled. This approach typically results in significantly lower costs and reduced machining complexity compared to machining the part as a single monolithic block.

 

Rule 2: The Larger the Internal Corner Radius, the Better; Avoid Specifying Radii That Are Too Small

This is one of the most fundamental—yet most frequently overlooked—principles of DFM. Milling cutters are cylindrical rotating tools and, as such, cannot produce perfect right angles; when the tool reaches a corner, it inevitably leaves a small radius on the material. If the technical drawing specifies a sharp right angle, achieving this in reality requires secondary processing—typically via Electrical Discharge Machining (EDM) or Wire EDM—which causes manufacturing costs to skyrocket instantly.

A general rule of thumb is: the radius of an internal corner should be no less than one-sixth of the cavity's depth. For depths exceeding a certain threshold, it is advisable to design the radius to be one-third of the depth. Ideally, this radius should be slightly larger than the cutter's own radius; this allows the tool to follow a smooth arc rather than making a sharp, abrupt turn, resulting in a much smoother cutting process. Across an entire design, it is best to standardize on a few specific radii that correspond to standard milling cutter sizes (e.g., R3, R4, R5, R6). This not only streamlines production but also minimizes the frequency of tool changes. Even a simple change—such as increasing a radius from R1 to R2—can, in practice, allow for the use of a sturdier cutter and significantly faster feed rates.

 

Rule 3: Standardize Datum Planes and Bottom Surface Heights to Minimize Clamping Operations

The number of clamping operations required is a cost factor that many engineers tend to overlook. Each additional clamping setup entails an extra tool calibration step, the re-establishment of a precision datum, and a corresponding increase in the probability of manufacturing errors. An ideal part design should allow for the completion of all machining operations in just one or two setups. This is achieved by orienting all features requiring machining in the same direction, or by distributing them across a limited number of surfaces that can be accessed within a single clamping configuration.

By ensuring that all bottom surfaces requiring machining within a design lie on the same height plane, one can drastically reduce the need to flip and re-clamp the workpiece. The nightmare scenario in machining is a part where features requiring work are scattered across all six faces—turning a simple cubic part into a complex operation requiring six separate clamping setups.

 

Rule 4: Prioritize Through-Holes Over Blind Holes, and Limit Hole Depth to Within 4 Times the Diameter

The cost disparity between machining deep holes and shallow holes is far greater than most people imagine. From a tooling perspective, the effective cutting depth limit for standard drill bits is approximately four times their diameter. Exceeding this limit necessitates the use of specialized tools—such as chip-breaking drills, peck-drilling techniques, or dedicated deep-hole drills—causing machining times to increase exponentially.

By making a few simple trade-offs during the design phase, costs can be significantly reduced: whenever possible, choose through-holes over blind holes. Through-holes provide an unobstructed path for chip evacuation, and the cutting forces acting on the tool are far more uniform than with blind holes, resulting in faster machining speeds. Furthermore, aim to keep the depth of any hole within four times its diameter whenever feasible. Hole diameters should be standardized to align with standard tooling sizes—for instance, using standard tap drill sizes for common threads like M3, M4, M5, and M6. This allows for the use of standard drills and taps, resulting in fewer tool changes and lower costs.

 

Rule 5: Limit Thread Depth to No More Than 3 Times the Nominal Diameter; Use Thread Inserts for Small Threads

Aluminum alloys have relatively low hardness, making their threads prone to stripping. This is particularly true for fine threads (M3 and smaller); after just a few assembly-disassembly cycles, the threads in the base material may become permanently damaged. Furthermore, for deeper threaded holes—specifically those exceeding three times the nominal diameter—the risk of tap breakage during machining increases significantly.

A common solution is to install steel wire thread inserts (such as Heli-Coils) into the aluminum components. Although this adds an extra step to the initial manufacturing process, it can exponentially extend the lifespan of the threads—a crucial benefit in applications requiring frequent assembly and disassembly. Another easily overlooked design consideration is the need to re-tap the threads *after* surface oxidation (anodizing), as the anodized layer adds material thickness and alters the thread profile dimensions.

 

Rule 6: Maintain a Minimum Wall Thickness of 1mm for Aluminum Parts; Add Reinforcing Ribs to Large, Thin-Walled Areas

While aluminum alloys possess inherent ductility, walls thinner than 0.8mm are susceptible to deformation caused by cutting forces during machining. Extremely thin-walled sections may vibrate like leaf springs; this not only compromises dimensional accuracy but also results in a poor, unsightly surface finish.

If weight-saving requirements necessitate a thin-walled design, the issue can be resolved by incorporating reinforcing ribs. The function of these ribs is to enhance the component's bending stiffness and torsional rigidity without significantly increasing its overall weight. Additionally, a specific machining technique—Climb Milling—can effectively reduce the lateral cutting forces exerted on thin walls by the tool, thereby helping to maintain the structural stability of thin-walled parts.

 

Rule 7: Employ Ribbed Structures Instead of Solid Thickening for Weight-Reduction Designs

This rule and the previous one represent two facets of the same fundamental design philosophy: one addresses "how to stabilize thin-walled structures," while the other addresses "how to hollow out thick sections." The quintessential example involves starting with a solid block of material, removing a significant volume of excess material, and then restoring the necessary structural strength by incorporating reinforcing ribs. When incorporating reinforcing ribs, keep the following practical guidelines in mind: The thickness of the ribs should typically be kept between 50% and 60% of the main wall thickness; ideally, the rib height should not exceed three times its thickness; and a rounded fillet transition should be included at the junction between the rib and the main body to minimize stress concentration. Furthermore, the orientation of the ribs should align with the primary direction of structural load-bearing, rather than being added haphazardly.

 

Rule 8: If a 3-axis machine suffices, avoid using 4- or 5-axis machines; if standard tooling works, avoid custom tooling.

Simply put, this rule translates to: minimize process complexity. The addition of every extra axis significantly escalates the capital cost of the machining center; similarly, the use of a custom (non-standard) cutting tool implies that a specialized instrument—which may potentially be used only once—had to be specifically fabricated for that particular machining job.

A highly practical principle is this: during the design phase, strive to orient all features requiring machining in the same direction. This allows a 3-axis machine to complete the entire job in a single setup (with just one clamping operation)—a level of efficiency far superior to processes requiring the part to be flipped over or re-oriented at different angles. Another effective method for simplifying the process is to apply a uniform fillet radius across multiple features, enabling a single cutting tool on the machine to machine several distinct areas simultaneously.

 

Rule 9: Apply tight tolerances only to critical mating surfaces; keep tolerances loose for all other areas.

Tolerances are, among all cost factors, the easiest to spiral out of control. When a manufacturing facility prepares a quotation, the sight of a drawing screen filled with ±0.01mm tolerance callouts is an immediate signal that the resulting part will not come cheap.

The truly rational approach is to manage tolerances hierarchically based on functional requirements: tight tolerances (e.g., ±0.01mm) should be reserved exclusively for critical surfaces involved in assembly—specifically those governing relative positioning, sealing, or shaft-to-bore fits. For non-critical cosmetic surfaces, clearance slots, or weight-reduction pockets, simply applying the "medium" tolerance class defined in the ISO 2768 standard (e.g., ±0.1mm) is entirely sufficient. This approach offers an additional benefit: during quality inspection, the factory is spared the need for a full-dimensional CMM scan; instead, they need only verify the critical dimensions, thereby effectively cutting inspection time in half.

 

Rule 10: Optimize the layout of internal cavities; if necessary, split the part into separate components for machining, then reassemble.

When designing parts with complex internal cavities, a common pitfall arises: all internal features become crammed into a single enclosed space. This congestion prevents cutting tools from reaching the necessary areas, hinders the evacuation of chips and debris, and makes it impossible to thoroughly remove machining burrs. A simple yet effective solution is the "divide and conquer" approach—breaking down a large, complex cavity part into several independent components that are machined separately, and then reassembling them using bolted connections or snap-fit ​​mechanisms. Although this appears to add an extra assembly step, machining costs are typically reduced significantly, as each individual component can be processed using standard tooling under optimal cutting conditions.

Summary: Key DFM Optimization Parameters at a Glance

Design Feature	Recommended Value	High-Cost Threshold
Deep Slot/Cavity Depth	≤ 4 × Tool Diameter	Depth exceeding 6 × Tool Diameter
Internal Corner Fillet Radius	≥ 1/3 × Cavity Depth (and ≥ R3)	Sharp corners (R0) require secondary processing
Minimum Aluminum Wall Thickness	≥ 1 mm (Recommended)	< 0.8 mm; prone to deformation during machining
Deep Hole Depth	≤ 4 × Hole Diameter	> 10 × Hole Diameter requires specialized equipment
Blind Hole Depth	≤ 3 × Hole Diameter	Exceeding 3× increases chip evacuation difficulty
Thread Depth	≤ 3 × Nominal Diameter	Exceeding 3× increases risk of tap breakage
Clamping Operations	1–2 setups	> 4 setups; risk of cumulative precision errors
Tolerance	± 0.1 mm (Standard); Tighter for critical features	± 0.01 mm applied across entire drawing

(The values ​​above are based on common aluminum alloys such as 6061-T6 and 7075-T6. Actual machining capabilities vary depending on the specific material and equipment used; it is recommended to consult with your manufacturing partner during the design phase.)

 

About Us

If you are currently working on aluminum parts and encountering issues such as "unmachinable designs" or "excessively high quotes," we invite you to send us your drawings for an evaluation. We will provide optimization recommendations from a Design for Manufacturability (DFM) perspective—there is no obligation to proceed to production immediately; our goal is simply to help you clearly identify and resolve any potential design issues first.