Aluminum is one of the most common materials we machine at Anco Precision. Its combination of light weight, good strength-to-weight ratio, excellent thermal conductivity, and natural corrosion resistance makes it the material of choice across industries from aerospace to electronics. It cuts cleanly, holds reasonable tolerances, and works well for both prototype and production runs. But not all aluminum part designs are created equal. The choices you make during the design phase directly affect machinability, cost, lead time, and whether the part can be manufactured as drawn.
This article walks through the practical considerations that matter when designing aluminum parts for CNC machining, from the machine shop's perspective. Whether you're an engineer finalizing a design or a purchasing manager preparing an RFQ, understanding these factors helps ensure your parts are manufacturable, cost-effective, and delivered on time.
Choosing the Right Aluminum Alloy
Aluminum alloys vary significantly in machinability, strength, corrosion resistance, and cost. The most common alloys we see in aluminum CNC machining are 6061-T6, 7075-T6, and 2024-T3, each with distinct characteristics.
6061-T6 is the workhorse. It machines well, welds easily, anodizes cleanly, and offers good corrosion resistance. It's suitable for a wide range of applications and is typically the most cost-effective option. If your design doesn't require exceptional strength or specific material properties, 6061-T6 is usually the right choice.
7075-T6 provides higher strength, making it popular in aerospace and high-stress applications. It machines well but costs more than 6061 and doesn't weld as easily. Anodizing 7075 can produce a less uniform appearance compared to 6061.
2024-T3 offers excellent fatigue resistance and is common in aircraft structures. It machines reasonably well but has lower corrosion resistance than 6061, often requiring protective coatings or anodizing.
When specifying material on your drawing or RFQ, include the alloy and temper. Simply calling out "aluminum" leaves room for interpretation and can lead to delays or the wrong material selection.
Wall Thickness and Structural Considerations
Thin walls are a common challenge in aluminum CNC machining. While aluminum is relatively stiff, thin sections can deflect under cutting forces, leading to chatter, poor surface finish, or dimensional inaccuracy.
As a general guideline, try to maintain wall thickness of at least 0.030" to 0.040" for small parts and 0.060" or greater for larger components. Thinner walls are possible but may require special fixturing, multiple setups, or reduced cutting parameters, all of which add time and cost.
The practical impact of this consideration is significant. A part with a 6-inch long wall at 0.025" thickness will be prone to deflection during machining. Increasing that wall to 0.050" or adding a mid-span rib significantly improves rigidity and makes the part easier to machine to specification. This design change might add a small amount of material cost but can reduce machining time and improve dimensional consistency, often resulting in a net cost reduction.
Ribs and gussets can reinforce thin sections without adding excessive weight. If weight reduction is critical, consider a honeycomb or lattice structure in non-critical areas rather than uniformly thin walls throughout the part.
Deep pockets with thin floors present similar challenges. The floor can deflect during machining, making it difficult to hold flatness or thickness tolerances. If a pocket must be deep, consider adding support ribs or increasing floor thickness where possible.
Pockets, Cavities, and Internal Features
Pockets and cavities are straightforward to machine, but a few design choices make the process more efficient and improve the final result.
Corner radii: Sharp internal corners are impossible to machine with rotating cutting tools. Every internal corner will have a radius equal to the tool radius used. Standard end mills range from 1/16" to 1/2" diameter, with smaller tools available for fine features. For example, a 1/8" diameter end mill produces a 1/16" corner radius. Specifying a corner radius of 0.030" to 0.060" is usually practical and avoids the need for very small, fragile tooling. If your design requires a sharp corner for fit or function, consider a post-machining operation like wire EDM, or redesign the mating part to accommodate a radius.
Pocket depth: Deep pockets require longer cutting tools, which are more prone to deflection and chatter. A depth-to-width ratio of 3:1 or less is generally manageable. For instance, a pocket that's 0.5" wide should ideally be no deeper than 1.5". Deeper pockets are possible but may require multiple tools, slower feeds, or additional operations.
Flat floors: A flat pocket floor is easier to machine than a contoured or angled floor. If the floor must be angled, provide adequate clearance for the tool and avoid sharp transitions.
Holes, Threads, and Fastener Features
Holes are among the simplest features to machine, but thread specifications and hole tolerances require attention.
Hole diameter and depth: Standard drill sizes are readily available and cost-effective. Non-standard diameters require reaming or boring, which adds time. For through holes, specify a diameter that matches standard drill sizes when possible. Blind holes should have a depth callout that accounts for the drill point—typically add 0.25" to 0.5" beyond the required thread or feature depth.
Threads: Tapped holes are common in aluminum parts. Unified National Coarse (UNC) threads are stronger and more forgiving in aluminum than fine threads, especially for smaller sizes. Specify thread depth clearly, and ensure there's adequate material behind the thread for strength. A general rule is to provide at least 1.5 times the thread diameter in engagement length for steel fasteners in aluminum.
Threads should be called out with standard designations, such as 1/4-20 UNC or M6x1.0. If a thread requires a specific class or tolerance, note that on the drawing.
Counterbores and countersinks: These are straightforward features but should be clearly dimensioned. For counterbores, specify diameter and depth. For countersinks, specify angle (typically 82° or 90°) and diameter.
Tolerances: When to Tighten and When to Relax
Tolerances have a direct impact on machining time and cost. Tighter tolerances require more careful setups, slower cutting speeds, additional inspection, and sometimes secondary operations.
Modern CNC equipment typically achieves ±0.005" for most dimensions without special effort. This is the standard machining tolerance for aluminum across the industry. Dimensions that require ±0.001" or tighter need extra attention, and tolerances below ±0.0005" may require grinding or other finishing operations.
The key is to apply tight tolerances only where necessary. If a hole location must align with a mating part, tolerance it accordingly. If a pocket depth is non-critical, a looser tolerance reduces cost without affecting function. The difference in cost between a part with all dimensions held to ±0.001" versus one with most dimensions at ±0.005" and only critical features tightened can be substantial—sometimes 30% or more depending on the complexity.
Geometric dimensioning and tolerancing (GD&T) is helpful for defining functional requirements clearly. Callouts like position, perpendicularity, flatness, and parallelism communicate design intent more precisely than coordinate dimensions alone. When used correctly, GD&T can actually reduce cost by allowing the machinist to focus on what truly matters.
The drawing typically serves as the controlling specification. If a dimension is not toleranced, the shop will apply standard tolerances per the title block or general notes. Make sure your drawing clearly states what those standard tolerances are.
Surface Finish and Cosmetic Requirements
Surface finish is another area where specifying only what's needed keeps costs down. Standard machining practice for aluminum typically produces a finish of 125 Ra or better, which is smooth to the touch and suitable for most applications.
If a surface requires a finer finish—such as 63 Ra or 32 Ra—it may need additional operations like fine milling, grinding, or polishing. These finishes are common for sealing surfaces, bearing surfaces, or cosmetic areas.
Anodizing is a popular finish for aluminum. It improves corrosion resistance, provides a hard surface, and allows for color options. Type II anodizing (standard) adds about 0.0001" to 0.0003" per surface, while Type III (hard anodizing) adds more. If dimensions are critical, specify whether they apply before or after anodizing.
Bead blasting produces a uniform matte appearance and is often used before anodizing or as a standalone finish. Powder coating and painting are also options, particularly for parts that require specific colors or additional corrosion protection.
If appearance matters, note which surfaces are visible or cosmetically critical. This allows the shop to orient the part in the machine to minimize tool marks or fixture contact on those surfaces.
Part Geometry and Machining Setup
The overall geometry of the part affects how many setups are required and how securely it can be held during machining. Parts that can be completed in a single setup are faster and less expensive than those requiring multiple setups or complex fixturing.
Prismatic parts with features on one or two sides are straightforward. Parts with features on three, four, or five sides require additional setups, each introducing the possibility of slight alignment variation.
Consider how the part will be fixtured. Large flat surfaces, parallel sides, and simple shapes are easy to clamp. Parts with complex contours, thin projections, or delicate features may require soft jaws, custom fixtures, or creative workholding solutions.
If possible, design the part so that critical features can be machined in a single setup. For example, if two holes must be precisely located relative to each other, having them on the same face allows them to be drilled in one operation, ensuring accuracy.
Prototype vs. Production Quantities
The quantity you're ordering affects how the shop approaches the job. Prototype and low-volume runs prioritize speed and flexibility, while production runs justify more investment in tooling and process optimization.
For smaller quantities, the shop may use standard tooling and straightforward setups to minimize programming and setup time. For larger production runs, custom fixtures, dedicated tooling, and optimized programs reduce cycle time and per-part cost.
If you anticipate moving from prototype to production, mention that in your RFQ. It allows the shop to consider scalability during the quoting process and may influence decisions about tooling and setup.
What to Include in Your RFQ
To help us quote your project accurately and quickly, here's what makes a difference:
Engineering drawing or CAD file: A detailed drawing is essential. If available, include a STEP or IGES file, which allows the shop to import the geometry directly into CAM software and identify potential manufacturing challenges early.
Material specification: Include alloy and temper, such as 6061-T6 or 7075-T6. If material certification is required, note that as well.
Quantity: Specify the number of parts needed. If you're ordering prototypes with potential for future production, mention that—it helps us consider the most cost-effective approach for both phases.
Tolerances: Ensure tolerances are clearly marked on the drawing. If certain dimensions are critical, highlight them or provide additional notes explaining why they matter.
Surface finish: Call out required finishes, whether machined, anodized, bead blasted, or other. If specific surfaces have cosmetic requirements, note which ones.
Required completion date: Provide a realistic timeline. This helps us schedule your project appropriately and let you know if your timeframe is achievable.
Inspection requirements: If you need a first article inspection report, material certification, or dimensional inspection report, specify that. Some customers may request compliance with specific standards—these should be noted as requirements in your RFQ.
Special notes: Include any other relevant information, such as packaging requirements, shipping instructions, or unique handling needs.
Get Your Aluminum Parts Machined at Anco Precision
Ready to move forward with your aluminum machining project? Our engineering team will review your design for manufacturability, identify any potential issues early, and provide a detailed quote with recommendations to optimize cost and quality.
To request a quote, provide your drawing or STEP file, material specification (alloy and temper), quantity, any critical tolerances or special requirements, and your desired delivery date. We'll evaluate your design and respond with a comprehensive quote that addresses your specific needs.
Contact Anco Precision today to discuss your aluminum machining needs and get expert guidance on optimizing your parts for manufacturing.