Threaded holes in CNC machining need to balance strength, manufacturability, tool life, and assembly reliability. The best practices depend on the material, thread size, production volume, and whether the thread is cut, formed, or inserted.
Common Methods for Creating Threads
Tapping
Most common for internal threads.
- Fast and economical
- Best for standard thread sizes
- Can be rigid tapped or floating tapped
- Risk of tap breakage increases in deep or small holes
Thread Milling
Uses a CNC interpolated toolpath.
- Excellent for large holes and hard materials
- One tool can create multiple thread sizes
- Better chip evacuation
- Easier recovery if tool breaks
- Slower than tapping
Form Tapping (Roll Tapping)
Creates threads by deforming material rather than cutting.
- Stronger threads in ductile materials
- No chips generated
- Requires larger tap drill size
- Not suitable for brittle materials like cast iron
General Design Guidelines
1. Thread Engagement Depth
A common rule:
- Steel: engagement ≈ 1× nominal diameter
- Aluminum: engagement ≈ 1.5× nominal diameter
- Plastics: engagement ≈ 2× nominal diameter
Examples:
- M6 in steel → 6 mm engagement
- 1/4-20 in aluminum → ~0.375 in engagement
Beyond these ranges, additional strength gains are usually minimal because the fastener tends to fail before the threads strip.
2. Blind Hole Depth
For blind tapped holes:
Recommended depth
- Thread depth + chamfer + drill point allowance
Typical formula:
Total hole depth ≈ required thread depth + 0.5×D to 1×DWhere D = drill diameter.
This extra depth prevents bottoming out.
Example
Need 12 mm of M8 thread:
- Drill depth may need ~16–18 mm
3. Minimum Wall Thickness Around Threads
Thin walls can crack or distort during tapping.
Guideline:
- Maintain wall thickness ≥ 0.5× thread diameter
- More for softer materials
For high-load applications:
- Prefer ≥ 1× diameter surrounding material
4. Thread Relief / Runout
Avoid forcing full threads to the bottom of blind holes.
Add:
- Relief groove
- Extra drill depth
- Bottoming tap only when necessary
This improves:
- Tool life
- Assembly consistency
- Thread quality
Tap Drill Size Selection
Standard Percentage of Thread
Typical design targets:
| Thread % | Usage |
|---|---|
| 50–60% | Easier tapping, softer materials |
| 65–75% | General-purpose |
| 75–85% | High holding strength |
| >85% | Usually unnecessary; increases torque dramatically |
Most production shops target ~65–75%.
Hole Types
Through Holes
Advantages:
- Easier chip evacuation
- Faster tapping
- Better for production
Preferred whenever possible.
Blind Holes
Require:
- Controlled depth
- Chip management
- Careful bottom clearance
More difficult and expensive.
CNC Machining Best Practices
Spot Drilling
Always spot drill before tapping for positional accuracy, especially:
- Small taps
- Hard materials
- Deep holes
Chamfer the Hole Entrance
Add a small chamfer:
Typical:
- 0.25–0.5 mm × 45°
- Or ~0.010–0.020 in
Benefits:
- Easier fastener starting
- Prevents burrs
- Protects first thread
Coolant and Lubrication
Critical for tap life.
Material-specific examples:
| Material | Recommended Lubrication |
|---|---|
| Aluminum | Kerosene / aluminum fluid |
| Steel | Sulfurized oil |
| Stainless | High-pressure tapping fluid |
Peck Tapping
Useful in:
- Deep holes
- Sticky materials
- Difficult chip evacuation
Reduces tap breakage risk.
Thread Milling vs Tapping
| Feature | Tapping | Thread Milling |
|---|---|---|
| Speed | Faster | Slower |
| Flexibility | One tap per size | One tool for many sizes |
| Tool break risk | Higher | Lower |
| Large threads | Difficult | Excellent |
| Blind holes | Harder | Easier |
| Hard materials | Challenging | Better |
Deep Thread Guidelines
Deep threaded holes are challenging.
Typical practical limits for tapping:
| Condition | Recommended Limit |
|---|---|
| Standard tapping | ≤ 2×D depth |
| Specialized deep tapping | 3–4×D |
| Beyond 4×D | Consider inserts or redesign |
Thread Inserts
Use inserts like Heli-Coil or Keenserts when:
- Material is soft
- Threads see repeated assembly
- Repairing damaged threads
- High-strength fastening required
Especially common in:
- Aluminum
- Magnesium
- Aerospace components
GD&T and Tolerancing
Important callouts include:
- Thread class (e.g., 6H, 2B)
- Thread depth
- Through/blind designation
- Positional tolerance
- Perpendicularity for sealing surfaces
Example:
M8 × 1.25 – 6H THRUor
1/4-20 UNC-2B × 0.500 DPCommon Mistakes
Overly Deep Threads
Adds cycle time and tap risk without meaningful strength gains.
Too High Thread Percentage
Creates excessive torque and broken taps.
No Chip Clearance
Major cause of tap failure in blind holes.
Tiny Threads in Production
Threads smaller than:
- M2
- #2-56
become increasingly fragile and costly.
Material-Specific Notes
Aluminum
- Easy to machine
- Threads strip more easily
- Use longer engagement or inserts
Stainless Steel
- Work hardens
- Requires aggressive feeds and proper lubrication
Titanium
- Difficult tapping
- Thread milling often preferred
Plastics
- Coarse threads work better
- Avoid excessive torque
Recommended Design-for-Manufacturing (DFM) Rules
Good Practice Checklist
- Prefer through holes
- Keep thread depth near 1×D
- Add chamfers
- Allow chip clearance
- Use standard thread sizes
- Avoid extremely fine pitches unless necessary
- Consider inserts in soft metals
- Use thread milling for large or critical holes
Typical Hole Stack Example
For an M10 × 1.5 blind tapped hole in aluminum:
| Feature | Typical Value |
|---|---|
| Thread engagement | 15 mm |
| Tap drill | 8.5 mm |
| Drill depth | 20–22 mm |
| Chamfer | 0.5 × 45° |
Industry Standards
Useful standards include:
- ISO metric thread standards
- ASME B1.1 Unified threads
- ANSI fastener standards
- SAE International aerospace/mechanical standards
