How to Design Parts for CNC Machining: DFM Guide
—
Introduction
A well-designed part can cost half as much to machine as a poorly designed one — with better quality and faster delivery. Design for Manufacturing (DFM) is the practice of optimizing your CAD model so it can be produced efficiently.
This guide covers DFM principles specifically for CNC machining, with actionable rules you can apply to your next design.
1. The Golden Rules of CNC DFM
Rule 1: Design Internal Corners with Radii
Sharp internal corners cannot be created with a rotating cutting tool. They require EDM or broaching — adding significant cost.
| Tool Diameter | Minimum Internal Radius |
|---|---|
| 3mm end mill | R1.5mm (minimum) |
| 6mm end mill | R3mm (recommended) |
| 10mm end mill | R5mm |
| 12mm end mill | R6mm |
Good: Internal corner R ≥ 3mm
Better: R ≥ ⅓ × cavity depth
Best: R ≥ 6mm for deep pockets
Rule 2: Respect Cavity Depth Limits
Deep, narrow cavities are difficult or impossible to machine because long tools deflect and vibrate.
| Cavity Width | Maximum Depth |
|---|---|
| 3mm | 12mm (4:1) |
| 6mm | 30mm (5:1) |
| 12mm | 60mm (5:1) |
| 25mm | 100mm (4:1) |
If depth exceeds these ratios: Consider splitting the part or using 5-axis machining to tilt the tool.
Rule 3: Maintain Minimum Wall Thickness
Thin walls vibrate during machining, causing poor surface finish and dimensional inaccuracy.
| Material | Minimum Wall | Recommended |
|---|---|---|
| Aluminum | 0.5mm | 1.5mm |
| Stainless Steel | 0.8mm | 2mm |
| Brass | 0.5mm | 1.5mm |
| POM (Delrin) | 1mm | 2mm |
| ABS | 1mm | 2.5mm |
For walls taller than 10mm: Double the minimum thickness.
Rule 4: Avoid Unnecessary Tight Tolerances
| Feature | Suggested Tolerance |
|---|---|
| Clearance holes | ±0.25mm |
| General dimensions | ±0.125mm |
| Mating surfaces | ±0.05mm |
| Bearing bores | H7 tolerance |
| Dowel pin holes | ±0.01mm |
| Threaded holes (position) | ±0.25mm |
2. Feature-Specific DFM Guidelines
Holes
| Rule | Why |
|---|---|
| Standard drill sizes | Custom sizes require boring/reaming |
| Through holes preferred | Blind holes need flat-bottom end mills |
| Depth ≤ 8× diameter | Longer needs special drills |
| Thread depth 1.5-2× diameter | Extra depth adds cost, not strength |
| Avoid intersecting holes | Creates burrs, weakens tools |
Threads
| Thread Type | Best For |
|---|---|
| Coarse threads | Aluminum, plastics (less likely to strip) |
| Fine threads | Steel, stainless (stronger engagement) |
| Threaded inserts | Frequently assembled joints, soft materials |
| Thread milling | Large diameters, high-value parts |
| Tapping | Standard sizes, high volume |
Pockets
- **Floor radius**: Use corner radius end mill for floor-to-wall transition
- **Draft angles**: Not required (unlike molding), but helps with chip evacuation
- **Floor finish**: Flat end mills leave circular marks — specify if cosmetic finish needed
Slots
| Slot Width | Max Depth |
|---|---|
| 3mm | 9mm |
| 6mm | 24mm |
| 10mm | 40mm |
| 15mm | 60mm |
Undercuts
Undercuts require special T-slot or dovetail cutters. Design them to match standard cutter geometries:
| Undercut Type | Standard Cutter Widths |
|---|---|
| T-slot | 3mm, 4mm, 6mm, 8mm |
| Dovetail | 45°, 60° standard |
3. Material-Specific DFM Tips
Aluminum
- Generous radii (≥ R3mm) — aluminum cuts easily but gummy chips stick to tools
- Coarse threads — fine threads strip easily in aluminum
- Reinforcement around tapped holes — minimum 2mm wall around threads
Stainless Steel
- Larger radii than aluminum — higher cutting forces
- Avoid very thin walls (<0.8mm) — work hardening makes them brittle
- Deep holes: peck drilling essential
Plastics
- Allow for thermal expansion — plastics expand 5-10× more than metals
- Avoid sharp corners — stress concentrations cause cracking
- Relaxed tolerances for non-critical features — ±0.2mm is often fine
- Consider annealing stress relief before final machining
4. Common DFM Mistakes
| Mistake | Problem | Fix |
|---|---|---|
| Sharp internal corners | Can't be milled, requires EDM | Add radius ≥ R1.5mm |
| Tall thin walls (>10:1 H:W) | Vibration, poor finish, breakage | Thicken walls or add ribs |
| Blind tapped holes too shallow | Stripped threads | Minimum 1.5×Ø engagement |
| Text/engraving too small | Illegible after machining | Minimum 2mm character height |
| No fixturing surfaces | Hard to clamp, inaccurate | Add parallel pads or holes |
| Tolerancing all features tight | Unnecessary cost | Only tolerance critical features |
| Ignoring tool access | Unreachable features | Check from all approach angles |
5. The DFM Checklist
Before submitting your design, verify:
- [ ] All internal corners have radii ≥ R1.5mm
- [ ] Cavity depth ≤ 4× width
- [ ] Wall thickness meets minimums for material
- [ ] Hole diameters match standard drill sizes
- [ ] Thread depths are 1.5-2× diameter
- [ ] Tolerances specified only on critical features
- [ ] All features accessible from standard tool directions
- [ ] Undercuts match standard cutter sizes
- [ ] Material specified with grade and temper
- [ ] Surface finish specified (or default to as-machined)
Free DFM Review from Our Engineers
Send your CAD file to Leland CNC and our engineers will review it for manufacturability — pointing out cost-saving opportunities and potential issues before machining begins. Free, no obligation, response within 24 hours.
Published: July 2026 | Leland CNC — Precision Manufacturing Since 2009