Designing for CNC machining isn’t just about geometry—it’s about minimizing cost without compromising precision. With 15+ years of experience manufacturing parts for aerospace, audio, and medical sectors, we’ve learned that a few smart design decisions can reduce machining costs by 40-60%. The difference between an affordable part and an expensive one often comes down to understanding manufacturing constraints early in the design process.
Design CNC parts for budget success by avoiding impossible geometries, using standard tool radii for corners, optimizing wall thickness for your material, and applying tight tolerances only where functionally required. Parts designed with machining constraints in mind typically cost 40-60% less than over-engineered designs.
Design rules to cut CNC costs: material thickness minimums, standard tolerances, and feature orientation strategies backed by real machining data.
Table of Contents
What Geometries Can't Be CNC Machined?
Sharp internal corners, deep narrow pockets deeper than 4x their width, and blind holes exceeding 8x diameter cannot be machined with standard CNC operations. Use this quick check: if a straight tool can’t reach the feature from above without interference, it’s likely impossible to machine. Most problematic features include 90° internal corners (minimum 0.5mm radius required) and any geometry requiring “wrap-around” tool paths.
Quick Decision Rules:
- Corner radius: Minimum 0.5mm for aluminum, 0.8mm for steel
- Pocket depth: Maximum 3x width (2mm wide = 6mm deep max)
- Blind holes: Maximum 8x diameter depth
- Wall thickness around threads: 1.5x thread diameter minimum
We see impossible geometry in 16.4% of initial design submissions. Sharp internal corners are the most common issue—CAD shows perfect 90° corners, but standard end mills require minimum radius clearance. Deep narrow features cause significant tool deflection, making tight tolerances difficult to achieve.
Internal threads in thin walls commonly fail during tapping operations. M6 threads require approximately 9mm of surrounding material to prevent wall failure. Undercuts requiring tool approach from multiple angles typically force expensive multi-axis setups or complete part redesign.
Standard tolerance guidelines like ISO 2768 assume conventional machining practices—impossible geometry makes these specifications unachievable.
Design Takeaway: Apply minimum 0.5mm radius to all internal corners, limit pocket depth to 3x width, and ensure straight-line tool access from above. When impossible features are functionally required, consider splitting the part or specifying press-fit inserts.
What's the Minimum Wall Thickness for CNC Parts?
Minimum wall thickness depends on material and unsupported length: 1.0mm for aluminum in small parts, 1.5mm for steel, and 2.0mm for plastics. Walls that are too thin deflect during machining, causing dimensional errors and potential cracking during use. The critical factor is unsupported span—a 20mm tall wall can be thinner than a 60mm tall wall due to cantilever effects.
Quick Thickness Reference:
- Audio enclosures: 1.5mm aluminum (adequate for mounting hardware)
- Mounting brackets: 2.5mm at load points, 1.5mm for non-critical sections
- Snap-fit features: 0.8mm minimum for flexibility without breaking
- Threaded bosses: 3mm minimum around M3 threads, 5mm around M5
We regularly machine 1.2mm walls in aluminum audio enclosures, but thinner walls require support ribs every 15-20mm to prevent deflection. Thin walls that deflect during cutting show taper—the top might measure differently than the bottom due to tool pressure. In plastic parts, thin walls can develop stress concentrations that affect long-term durability.
What happens when walls fail? Parts exhibit poor surface finish, fail tolerance inspection, or show dimensional instability. Aluminum walls under 0.8mm in unsupported spans typically bow during machining, making assembly fitment problematic.
Support ribs spaced every 20mm can allow thinner walls while maintaining rigidity. This approach works well for weight-sensitive applications where material removal is critical.
Design Takeaway: Use 1.5mm minimum for aluminum walls over 25mm tall, add support ribs every 20mm for thinner sections, and increase thickness around fastener locations to ensure structural integrity at connection points.
How Tight Can Inside Corners and Fillets Be?
Inside corner radius is limited by end mill diameter—0.5mm minimum for most applications, but 1.0mm radius offers the best cost-effectiveness. Smaller radii require micro end mills and slower cutting speeds. Standard end mills create these limitations because cutting tools are inherently round, not square.
Quick Radius Reference:
- Most cost-effective: 1.0mm radius
- Functional minimum: 0.5mm radius
- Gasket channels: 0.5-0.8mm
- Stress relief: 1.0mm minimum
The smaller the radius, the more specialized the tooling becomes. Micro end mills for 0.25mm radius corners cost more than standard tooling and require slower feed rates to prevent breakage. Smaller radii increase cycle times compared to standard 1.0mm radius corners.
When sharp corners matter functionally: If you need a sharp edge for part fit or sealing, consider post-machining operations, splitting the part at the corner, or using press-fit inserts rather than specifying unmachined geometry.
Corner radius affects part strength. Sharp corners create stress concentrations that can cause fatigue failure—larger radius corners typically show better fatigue life than smaller corners in cyclic loading applications.
Design Takeaway: Specify 1.0mm radius for optimal cost-effectiveness, use 0.5mm only where functionally required, and consider design alternatives for applications requiring sharper corners than standard tooling can achieve.
How Do I Design Pockets and Cavities for Efficient Machining?
Design pockets with depth-to-width ratios no greater than 3:1, provide adequate corner radii, and ensure straight tool access from above. Most cost-effective pocket design uses 1.0mm corner radius, uniform depth to minimize tool changes, and avoids narrow deep slots that force expensive micro-tooling. Any pocket deeper than 3x its width requires specialized techniques and longer cycle times.
Quick Pocket Check:
- Is pocket deeper than 3x width? → Add ribs or split into multiple shallow pockets
- Are corners sharp (under 0.5mm)? → Increase to 1.0mm radius minimum
- Need deep narrow slot? → Consider assembly solution instead
- Component won’t fit? → Use removable insert or two-piece design
Pocket Design Guidelines:
- Battery compartments: 15mm wide minimum for efficient tool access
- Wire channels: Multiple shallow pockets better than one deep slot
- Component recesses: 1.0mm corner radius prevents stress concentrations
- Mounting pockets: Keep depth under 3x width for standard tooling
We regularly machine component pockets in aluminum enclosures, but geometry optimization is critical. A 10mm wide battery compartment can efficiently go 25mm deep, while a 3mm wide wire channel becomes problematic beyond 8mm depth. Instead of one 2x20mm wire slot, we recommend three 6x6mm pockets connected by thin channels for better machinability.
When deep pockets are required functionally: Consider removable inserts, two-piece assembly designs, or adding internal ribs to break up large cavities. These alternatives often cost less than attempting to machine problematic geometry.
Design Takeaway: Keep pocket width-to-depth ratios at 3:1 or better, use 1.0mm corner radii, and consider assembly solutions for deep complex cavities that would require specialized machining techniques.
How Should I Orient Features to Reduce Machining Cost?
Orient parts so that most features can be machined from one primary face, group holes by size and type, and place critical tolerances on accessible surfaces. Each additional setup increases cost due to fixture time, repositioning complexity, and inspection requirements. Smart orientation reduces both machining time and positioning errors.
Setup Decision Framework:
- Can 90% of features be reached from one side? → Single setup works
- Are holes scattered on multiple faces? → Consider redesign or part splitting
- Do critical tolerances require multiple setups? → Move to primary face if possible
- Is second setup unavoidable? → Group secondary features efficiently
Orientation Guidelines by Part Type:
- Enclosures: Place all holes and pockets on the front face when possible
- Mounting brackets: Group bolt holes on one end, avoid features on both faces
- Housings: Keep snap-fit features and mounting points on the same surface
- Faceplates: Consolidate all openings to eliminate back-side machining
Feature grouping impacts efficiency significantly. Drilling all M3 holes together, then all M5 holes, minimizes tool changes. We’ve seen measurable time reductions by relocating scattered holes to a single face versus machining features on multiple surfaces requiring repositioning.
When multiple setups are unavoidable: Keep critical tolerances on the primary face where positioning accuracy is optimal. Secondary setup positioning introduces additional variation that affects final part quality and inspection complexity.
Design Takeaway: Consolidate features onto one primary face whenever functionally possible, group holes by size and type, and consider part splitting when features absolutely require multiple complex orientations rather than forcing expensive multi-setup operations.
Which Materials Are Easiest to Machine?
6061-T6 aluminum offers the best combination of machinability, strength, and cost for most CNC applications. It machines cleanly with standard tooling, holds tight tolerances reliably, and accepts common finishes like anodizing. For higher strength requirements, 7075 aluminum machines well but requires more careful tool selection.
Quick Material Picker:
- Need corrosion resistance? → 316 stainless steel
- Need anodizing + good strength? → 6061-T6 aluminum
- High stress application? → 7075-T6 aluminum
- General prototyping? → 6061-T6 aluminum
Material Selection by Application:
- Audio enclosures: 6061-T6 (excellent anodizing, adequate strength)
- Medical housings: 6061-T6 or 316 stainless (biocompatibility requirements)
- Aerospace brackets: 7075-T6 (high strength-to-weight ratio)
- Industrial equipment: 6061-T6 (most cost-effective)
We machine 6061 aluminum daily with predictable results—consistent surface finish, reliable tolerance holding, and excellent tool life. 7075 offers superior strength but requires sharper carbide tools and more conservative cutting parameters. Stainless steel work-hardens during cutting, making thin walls and interrupted cuts particularly challenging.
6061 aluminum consistently holds ±0.01mm tolerances with proper setup and works well with standard anodizing processes. 7075 machines to similar tolerances but increases both material and machining costs. Stainless steel requires specialized techniques for tight tolerance work due to work hardening characteristics.
Design Takeaway: Start with 6061-T6 aluminum for most applications requiring good strength and machinability. Upgrade to 7075 only when strength analysis shows necessity. Choose stainless steel only when corrosion resistance is functionally critical.
What Tolerances Are Achievable Without Extra Cost?
General tolerances of ±0.05mm are standard for most CNC operations and align with ISO 2768-m guidelines. Tolerances of ±0.02mm require careful setup procedures. Apply tight tolerances only to functional features—over-specifying tolerances on non-critical dimensions increases inspection complexity unnecessarily.
Quick Tolerance Guide:
- Is this a critical dimension? → Yes: ±0.02mm, No: ±0.05mm
- Press-fit or bearing surface? → ±0.01mm required
- Mounting or clearance hole? → ±0.1mm adequate
- Cosmetic edge or surface? → ±0.05mm standard
Tolerance Guidelines by Feature Type:
- Mounting holes: ±0.1mm (adequate clearance for standard fasteners)
- Press-fit features: ±0.01mm (required for proper interference fits)
- Bearing surfaces: ±0.02mm (typical for mechanical interfaces)
- Cosmetic edges: ±0.05mm (ISO 2768-m standard)
We routinely hold ±0.02mm on aluminum parts using standard machining centers with proper fixturing and temperature control. Tighter tolerances require additional setup time and extended inspection procedures. Parts requiring ±0.005mm tolerances typically need specialized equipment beyond standard CNC capabilities.
Functional examples clarify tolerance selection: Clearance holes for M5 bolts work fine with ±0.1mm tolerance. Press-fit pins require ±0.01mm for proper interference. Gasket surfaces may need ±0.02mm flatness for reliable sealing performance.
Design Takeaway: Use ±0.05mm general tolerances for most features, specify ±0.02mm for functional surfaces requiring precision, and reserve ±0.01mm tolerances for critical fits. Apply tolerances based on functional requirements rather than arbitrary precision.
What Surface Finishes Can I Get As-Machined?
Standard CNC machining achieves Ra 1.6-3.2 μm surface finish on aluminum parts without secondary operations. This finish quality works well for most functional applications. Finer finishes require slower feeds and specialized toolpath strategies.
Quick Finish Guide:
- Will this be painted? → Ra 3.2 μm adequate
- Anodized appearance part? → Ra 1.6 μm preferred
- Gasket sealing surface? → Ra 0.8 μm required
- Show surface or aesthetic? → Ra 0.4 μm (secondary ops needed)
Surface Finish by Application:
- Painted surfaces: Ra 3.2 μm adequate (paint fills minor tool marks)
- Anodized aluminum: Ra 1.6 μm preferred (better visual appearance)
- Gasket sealing surfaces: Ra 0.8 μm for reliable O-ring sealing
- Consumer show surfaces: Ra 0.4 μm or better (requires secondary operations)
Material significantly affects achievable surface quality. 6061 aluminum produces excellent finishes with standard tooling. Stainless steel requires sharper tools and optimized cutting parameters to prevent work hardening marks that degrade surface quality.
Most parts function perfectly with as-machined Ra 3.2 μm finish. Gasket surfaces requiring Ra 0.8 μm need slower cutting speeds but remain achievable with standard CNC operations. Finishes smoother than Ra 0.4 μm typically require secondary polishing operations.
Surface finish specification should match functional needs. Sealing surfaces benefit from Ra 0.8 μm for O-ring compatibility. Painted parts work fine with Ra 3.2 μm as paint fills surface texture effectively.
Design Takeaway: Specify Ra 3.2 μm for general surfaces, Ra 1.6 μm for anodized parts, and Ra 0.8 μm for sealing surfaces. Reserve smoother finishes for applications where function truly requires enhanced surface quality.
Conclusion
Smart CNC design choices—proper material selection, realistic tolerances, and machinable geometry—can reduce part costs by 40-60% while maintaining full functionality. Focus on 6061 aluminum with ±0.05mm general tolerances and 1.0mm corner radii for most applications. Contact us to explore manufacturing solutions tailored to your product design requirements.
Frequently Asked Questions
POM and Delrin plastics typically hold ±0.05mm tolerances reliably. Tighter tolerances are challenging due to thermal expansion during cutting and post-machining stress relief. Consider ±0.1mm for non-critical plastic part dimensions.
Use 7075 only when stress analysis shows 6061 is inadequate for your load requirements. While 7075 offers higher strength, it increases both material cost and machining time compared to 6061’s excellent machinability.
If 90% of your features can be accessed from one primary face, single setup works. Features on opposite faces or requiring different orientations typically need additional setups, increasing cost due to repositioning and fixture complexity.
Ra 1.6 μm provides good appearance for anodized parts and is achievable with standard CNC operations. Ra 3.2 μm works for painted surfaces, while Ra 0.8 μm is recommended for gasket sealing surfaces requiring O-ring compatibility.
Sharp corners (under 0.5mm radius) require EDM or specialized micro-machining, typically adding 200-300% to part cost. Consider design alternatives like split parts, press-fit corner inserts, or assembly solutions rather than attempting to machine impossible geometry.
6061-T6 aluminum with ±0.05mm general tolerances and ±0.02mm on critical mounting surfaces offers the best balance of strength, machinability, and cost. This combination works well for most structural applications while keeping machining time and inspection requirements reasonable.
