CNC Design Guide & Key Considerations
CNC machining is a manufacturing process where cost and outcomes vary greatly depending on the precision of the design. This guide provides essential tips on tolerances, machinability, finishes, and common design mistakes that must be considered when preparing drawings and product designs.
Basic Considerations for CNC Design
Before drafting CNC drawings, make sure to check the following:
1.Tolerance Specification
- Assign tolerances only where absolutely necessary.
- Excessive tolerance requirements increase machining costs and can affect delivery times.
- Standard machining guidelines (see ISO2768 table below for details):
- Minimum allowable tolerance: ±0.05mm
- Recommended general tolerance: ±0.1mm
ISO2768 Standard Table
| Reference Length | General Tolerance | Precision Tolerance |
| Under 6mm | ±0.1mm | ±0.05mm |
| 6mm – 30mm | ±0.2mm | ±0.1mm |
| 30mm – 120mm | ±0.3mm | ±0.15mm |
| 120mm – 400mm | ±0.5mm | ±0.2mm |
| 400mm – 1,000mm | ±0.8mm | ±0.3mm |
*Standard general tolerances applied; precision tolerances upon request.
2. Machinability
- Internal corners cannot be perfectly square due to the nature of cutting tools.
- Avoid complex undercuts to ensure tool accessibility.
- Deep pockets or thin/tall features may be prone to vibration and deflection.
3. Finishing Standards
- Finishing methods (anodizing, bead blasting, etc.) can affect dimensions—adjust tolerances accordingly.
- For assembly areas, base design on pre-finish tolerances.
CNC Machining Considerations
1.Tool Geometry
- Due to cylindrical tools, internal right angles are not possible.
2. Tool Accessibility
- Features deeper than the tool or with limited access cannot be machined.
3. Material Rigidity
- Ensure minimum wall thickness to prevent warping from heat and cutting forces.
4. Tool Length & Vibration
- Longer tools increase vibration, risking tolerance loss and potential breakage.
5. Setup Feasibility
- Complex setups can affect both precision and cost.
Common Design Errors & Improvement Tips
1. Undercut Minimization
- Avoid non-standard reverse features or consider special methods (EDM: Electrical Discharge Machining) if inevitable.
- Design undercuts with standard width and spacing.
- Recommended width: 3mm–40mm
- Max depth: 2× width
- Standard tool cutting depth (D): 2–3× cutting width (W)
2. Undercut Dimensions
- Width (W): 3mm–40mm (recommended)
- Depth (D): up to 2× width (W)
3. Undercut Spacing
- Cutting interval: 4× depth (D)
- Allow enough space for smooth tool movement for internal undercuts.
4. Internal Corner Radius Required
- Cutting tools create rounded corners; always apply fillets (radius) for machinability.
- Recommended fillet: at least 1/3 of pocket depth.
- Floor should match the cutter’s round profile.
*Fillet: Rounding sharp part edges to reduce stress concentration and increase part durability.
5. Hole Design Tips
- Use standard drill diameters; hole depth should ideally be ≤4× diameter (up to 10× maximum).
- Recommended:
- Diameter: ≥1mm
- Depth: up to 4× diameter (max 10×)
6. Minimum Wall Thickness
- Varies by shape and size (values below for walls ≤10mm × 10mm):
- Metal: 0.5mm (min) / 0.8mm (recommended)
- Plastic: 1.0mm (min) / 1.5mm (recommended)
- Thin walls increase vibration and reduce accuracy.
7. Thread
- Diameter: M2 (min) – M6 or larger (recommended)
- Depth: up to 3× nominal size (Mx)
- Refer to standard tap charts.
- Design with the largest practical thread size; exceeding recommended depth adds no functional benefit.
8. Tall Features
- Recommended maximum height: ≤4× width.
- Excessively tall features can vibrate during machining, affecting precision.
9. Maximum Part Size
- Typical production limits vary by CNC machine type:
- Typical milling max: 1,600mm × 670mm × 150mm
- Typical turning max: 460mm × 1,070mm
Considering these factors at the design stage minimizes trial and error during manufacturing and enables faster, more efficient production.
See detailed information on: