How to Design CNC Machined Parts: Pocket Depths, Wall Thicknesses, and Internal Corners
Designing CNC Machined Parts: Pocket Depths, Wall Thicknesses, and Internal Corners
Every CNC machined part begins as a design decision. Pocket depths, wall thicknesses, and internal corner radii are the three features that most strongly determine whether a part machines quickly and cheaply — or fights the tool at every pass. Designers who understand these limits before sending a file to the shop routinely cut machining cost by 20–50%, shorten lead times, and eliminate scrap. This guide explains the numbers behind machinable geometry, what happens when a design exceeds them, and how SOMI Custom Parts applies these rules on every project.
What Makes a CNC Machined Part "Machinable"?
Machinability is not about material alone. A part is machinable when its geometry can be produced with standard cutting tools at reasonable feed rates, with predictable accuracy and surface finish. Three design features dominate this equation: how deep a pocket can go relative to its width, how thin a wall can be before it vibrates, and how small an internal corner radius can be before it forces a fragile tool.
Industry research shows why these features matter so much. According to aPriori engineering case studies, more than 70% of a part's manufacturing cost is locked in during the early design phase, before a machinist ever sees the file. And research from Modus Advanced shows that effective Design for Manufacturing (DFM) implementation reduces manufacturing costs by 15–40% and cuts lead times by up to 25%. In documented cases, design optimization alone has cut CNC machining costs by 50%. The design stage is the cheapest place to save money — and the most expensive place to ignore it.
Key Benefits of Machinable Part Design
- Lower unit cost: Parts that follow DFM rules cost 30–50% less to machine, with savings from fewer setups, faster cycle times, and less tool wear.
- Shorter lead times: Standard tooling and moderate depth ratios avoid long-reach tool orders and slow finishing passes, so quotes and deliveries both accelerate.
- Better accuracy and finish: Stiff walls and short tools cut without chatter, holding tolerances reliably and producing consistent surface finish.
- Fewer rejected parts: Thicker walls and sensible depths reduce deflection, distortion, and scrap — critical for production runs.
- More suppliers can quote you: A machinable design can be made on standard 3-axis CNC machines, widening your supplier pool.
Pocket Depths: How Deep Is Too Deep?
A pocket is an enclosed cavity milled from above. The depth limit exists because of tool stiffness: to cut a deep, narrow pocket, the machinist must use a long, small-diameter end mill. Long tools flex under cutting force, causing chatter, poor surface finish, tapered walls, and even tool breakage. The practical rule used across the industry is a depth-to-width ratio of 4:1 — a pocket should be no deeper than four times its narrowest width.
The cost impact of increasing pocket depth is steep. A 10 mm wide pocket is straightforward at 20 mm deep, moderate at 40 mm, and significantly more expensive beyond that. As the depth-to-width ratio climbs, so do cycle time, tool cost, and risk.
| Depth-to-Width Ratio | Difficulty | Tool Type | Cost Impact |
|---|---|---|---|
| Up to 2:1 | Easy | Standard end mill | Base cost |
| 2:1 to 4:1 | Moderate | Standard or slightly extended | 1.2–1.5x |
| 4:1 to 6:1 | Hard | Extended-reach end mill | 2–3x |
| 6:1 and above | Very hard | Specialty long-reach tooling | 4x+ |
If a design truly needs a deep feature, options include widening the pocket so a stiffer tool fits, stepping the pocket walls in tiers so each level stays within reach, or — for mating assemblies — splitting the deep feature across two machined faces. Real shops report that a 15 mm deep pocket can easily triple cycle time compared with an 8 mm version of the same opening, purely because of the longer tool and slower feeds required.
Wall Thicknesses: Thin Walls Vibrate, Chatter, and Fail
Thin walls act like springs during machining. Cutting forces push the wall sideways; if the wall is too thin relative to its height, it vibrates, leaving a wavy surface, drifting out of tolerance, and sometimes breaking the tool. Every material has a minimum safe wall thickness that balances rigidity with the cutting forces the material generates.
| Material | Minimum Wall | Recommended Wall | Notes |
|---|---|---|---|
| Aluminum | 0.5 mm (0.020") | 0.8–1.0 mm (0.031–0.040") | Softer, more forgiving |
| Steel | 0.8 mm (0.031") | 1.0–1.5 mm (0.040–0.060") | Higher cutting forces |
| Stainless steel | 0.8 mm (0.031") | 1.2 mm (0.047") | Work hardens under stress |
| Titanium | 1.0 mm (0.040") | 1.5 mm (0.060") | Spring-back causes deflection |
| Plastics | 1.0 mm (0.040") | 1.5 mm (0.060") | Melts and deforms easily |
Thickness is only half the story — height matters equally. A wall that is 5x taller than it is thick will almost certainly vibrate. Keep the height-to-thickness ratio below 4:1 for best results; 4:1 to 8:1 requires light passes and careful workholding; above 8:1 becomes expensive and may need special fixturing. For tall thin webs, add ribs or gussets to stiffen the structure — this simple change can make an un-machinable part completely standard.
Internal Corners: Why Sharp Corners Cost the Most
End mills are round, so they physically cannot cut a perfectly sharp 90° internal corner. Every internal corner carries a radius equal to the tool radius: a 6 mm end mill leaves a 3 mm corner radius, a 3 mm end mill leaves a 1.5 mm radius. The radius you specify directly sets the tool size — and smaller tools are slower, weaker, and break more often.
| Corner Radius | Tool Diameter | Relative Speed | Cost Impact |
|---|---|---|---|
| 6 mm+ (0.25"+) | 12 mm (0.5") | Fast | Lowest cost |
| 3 mm (0.125") | 6 mm (0.25") | Medium | Standard |
| 1.5 mm (0.060") | 3 mm (0.125") | Slow | 1.5–2x more |
| 0.5 mm (0.020") | 1 mm (0.040") | Very slow | 3–5x more |
The industry-standard "1/3 rule" ties corner radius to pocket depth: use a corner radius of at least one-third the pocket depth, with a practical minimum of 1 mm. A 12 mm deep pocket should carry a 4 mm or larger corner radius. This keeps the tool stiff enough to cut without vibration.
Two more corner rules prevent expensive surprises. First, never mix different corner radii within the same pocket — one radius means one tool, while multiple radii force multiple tool changes. Second, if a mating part genuinely needs a square corner, specify a dog-bone or T-bone relief cut in the corner instead of a tiny radius: the relief allows a standard tool to clear the corner, or the mating part's external corner can be rounded instead.
Related Rules: Holes, Threads, and Feature Access
The same logic extends to other features. Standard twist drills reach about 4x their diameter in one pass; up to 10x is possible with peck drilling, and beyond that requires specialized gun drilling or boring bars — both costly. Thread engagement of 1.5–2x the bolt diameter provides full strength; deeper threads add cost without meaningful strength. Blind holes need at least 0.5x the diameter of extra depth for the drill point, and using a through-hole instead of a blind hole wherever possible is always the cheaper choice.
Access is the other half of machinability. A CNC tool can only cut what it can physically reach. Internal undercuts, cavities with small openings, and features hidden behind other geometry add significant complexity. If an undercut is not functionally required, redesign it as a chamfer or split the part into two assembled pieces. Every feature that must be reached from a new angle adds a setup — and each setup adds time, cost, and alignment error.
Real-World Redesign Results
These rules are not theoretical. Published case studies consistently show the same pattern: DFM-driven redesigns preserve function while dramatically cutting cost and lead time.
- Industrial automation OEM (Netherlands): A complex aluminum manifold carried tight ±0.006 mm tolerances across the entire body, sharp square inner corners, and five separate clamping setups. Restricting tolerance to sealing surfaces, adding R1.5 fillets, and consolidating to a single 5-axis setup cut total CNC cost by 29% and shortened lead time by 3 working days — with zero impact on function.
- Robotics firm (enclosure bracket): An original design with 18 intricate pockets, ±0.01 mm tolerances everywhere, and titanium was revised to 8 pockets, standard ±0.05 mm commercial tolerances, and 6061 aluminum. Machine time dropped 42%, inspection effort dropped 30%, and total project cost fell 35%.
- General DFM impact: Across documented projects, DFM implementation reduces manufacturing costs by 15–40% and cuts lead times by up to 25%; part designs following DFM rules machine 30–50% cheaper than unoptimized equivalents.
How SOMI Custom Parts Can Help
At SOMI Custom Parts, we review every design against these rules before a single tool moves. Our engineers flag cost-driving geometry — over-tolerancing, sharp corners, deep narrow pockets, thin walls — and propose alternatives that preserve your design intent while lowering cost. We machine with ISO 9001-certified quality systems, hold precision tolerances down to ±0.005 mm where required, and support both prototyping and production runs.
Send us your 3D CAD file or 2D drawing through our inquiry page, and our team will return DFM feedback with your quote. You can also browse our CNC machining parts range or the full product catalog to see what we produce. For more design guidance, visit the SOMI blog or learn about our capabilities on the About Us page.
Frequently Asked Questions
What is the minimum wall thickness for CNC machined parts?
Keep metal walls at least 0.8 mm (0.8–1.0 mm recommended for aluminum and steel, 1.0–1.5 mm for titanium) and plastic walls at least 1.5 mm. Thinner walls vibrate under cutting forces, causing chatter and poor finish.
How deep can a CNC mill cut a pocket?
Standard tools comfortably reach 4x the pocket width (a 10 mm wide pocket up to 40 mm deep). Deeper pockets need long-reach tooling that costs 2–4x more and cuts slower.
What corner radius should I specify for internal corners?
At least one-third the pocket depth, with a practical minimum of 1 mm. Match the radius to standard end mill sizes (3, 4, 6, or 8 mm radii) for the fastest, cheapest machining.
Can CNC machines cut sharp internal corners?
No — end mills are round, so internal corners always carry a radius. For functionally square mating corners, use a dog-bone or T-bone relief cut, or radius the mating part's external corner instead.
How much can good design save on CNC machining cost?
Effective DFM typically reduces manufacturing costs by 15–40% and lead times by up to 25%. Documented redesigns have cut total project cost by 29–35% without changing part function.
Conclusion
Pocket depths, wall thicknesses, and internal corner radii are the three design dials that control machinability — and machinability controls cost. Keep pockets under 4x their width, keep walls thick enough to resist cutting forces, and give internal corners at least one-third the pocket depth. These rules cost nothing in CAD and save real money on the shop floor.
Designing new parts or looking to optimize an existing design? Contact SOMI Custom Parts through the inquiry form for a free DFM review and a competitive quote.
