Flow / Friction Drilling: Principle, Parameters and Design for Threading in Thin-Wall Materials
Neutral, educational guide to flow (friction) drilling: principle, parameters, materials, DFM, QA & safety, case studies, plus an interactive calculator.
Overview
Flow drilling, also known as friction drilling or thermal drilling, is a chipless hole-forming process used to create reinforced holes and functional threads in thin-wall metal sheets or tubes. Instead of cutting, a conical tool rotating at high speed locally heats and plasticizes the material by friction. The displaced material forms a bushing (boss) that increases the effective wall thickness, providing sufficient depth for tapping or thread forming.
This method is widely used when mechanical fasteners such as rivet nuts or weld nuts are undesirable due to weight, cost, or contamination.
1) Principle of Operation
During flow drilling, a solid carbide conical tool is pressed axially into the workpiece while rotating at high speed. Friction generates intense localized heat, softening the material without melting it. The material flows plastically around the tool, forming a collar and bushing.
Process sequence (four stages)
- Penetration: tool tip contacts the surface and frictional heat builds up.
- Cone formation: material begins to soften and flow downward.
- Through-flow: tool penetrates, displacing material to form a bushing.
- Calibration: tool shoulder smooths the surface and defines final boss height.
2) Typical Applications
Flow drilling is suitable for components requiring strong threaded joints in thin metals:
- Packaging machinery and assembly lines: brackets, frames, housings.
- Automotive and automation equipment: body structures, fixtures.
- Metal furniture, HVAC systems, appliances.
Not recommended for
- Brittle materials, previously heat-treated or coated surfaces that degrade under frictional heat.
- Components sensitive to heat discoloration.
3) Recommended Materials and Thicknesses
| Material type | Typical grade | Wall thickness (mm) | Hole Ø (mm) | Boss height (mm) |
|---|---|---|---|---|
| Low-carbon steel | S235–S355 | 1.0–3.0 | 4–10 | 1.5–3.5 |
| Stainless steel | 304 / 316 | 0.8–2.5 | 3–8 | 1.2–2.8 |
| Aluminium alloys | 5052 / 6061 / 6082 | 1.0–4.0 | 4–12 | 1.8–4.0 |
| Copper / Brass | CW508L / CW614N | 0.8–2.5 | 3–8 | 1.0–2.5 |
Notes: Aluminium’s higher thermal conductivity requires higher spindle speeds and lower torque. Stainless steels need greater axial force and lubrication due to higher strength and lower conductivity.
4) Process Parameters (Practical Guide)
| Tool Ø (mm) | Material | Spindle speed (rpm) | Feed rate (mm/min) | Approx. torque (Nm) |
|---|---|---|---|---|
| 4 | Mild steel | 4 500–5 500 | 200–300 | 3–5 |
| 6 | Aluminium | 5 500–7 000 | 250–350 | 2–3 |
| 8 | Stainless steel | 3 000–4 000 | 150–250 | 8–10 |
| 10 | Brass | 3 500–4 500 | 200–300 | 4–6 |
- Lubrication: light oil or paste to minimize tool wear and improve finish.
- Tool geometry: included angle 45–60°, short pilot, polished shoulder.
- Tool material: tungsten carbide, TiN/TiCN coating recommended.
5) Post-Process: Thread Forming
After the bushing is formed, a thread can be created by:
- Form tapping (roll tapping): preferred for ductile materials; stronger threads, no chips.
- Cut tapping: for harder materials or small diameters.
Quality control: check threads using go/no-go gauges. Recommended tolerance class: ISO 6H (cut) or 6H–7H (form).
6) Design for Manufacturability (DFM)
| Design aspect | Recommended value |
|---|---|
| Minimum distance from edge | ≥ 2× hole diameter |
| Minimum distance between holes | ≥ 3× hole diameter |
| Minimum wall flatness deviation | ≤ 0.1 mm |
| Clamping stiffness | rigid, minimal vibration |
- ☑ Proper tool alignment
- ☑ Rigid clamping
- ☑ Use consistent feed & rpm
- ☑ Verify boss height and concentricity after drilling
7) Advantages and Limitations
Advantages
- Eliminates nuts, welds, and inserts
- Fast cycle time (1–2 s per hole)
- Strong, chipless thread
- Lower assembly cost
Limitations
- Generates local heat-affected zone (HAZ)
- Surface oxidation/discoloration possible
- Not suitable for brittle/hard materials
- Coated parts may require re-finishing
Comparison with Alternatives
| Method | Additional part | Cycle time | Joint strength | Cost |
|---|---|---|---|---|
| Friction drilling + thread forming | none | 1–2 s | High | Low |
| Rivet nut | yes | 10–15 s | Medium | Medium |
| Weld nut | yes | 8–12 s | High | High |
| Cut tapping in thin sheet | none | 3–5 s | Low | Low |
8) Quality Assurance and Safety
- Inspect boss height, hole roundness, thread concentricity, pull-out strength.
- Record torque and temperature during trials for process validation.
- Provide adequate ventilation and fume extraction.
- Wear eye protection and heat-resistant gloves.
- Avoid flammable lubricants at high rpm.
9) Case Studies (Examples)
Case 1 – Mild steel bracket (2 mm): Ø6 mm hole, 4 800 rpm, 250 mm/min feed. Boss height 2.8 mm. Thread M6 form-tapped. Pull-out strength +230% vs rivet nut.
Case 2 – Aluminium 6061 (3 mm): Ø8 mm hole, 6 500 rpm, 300 mm/min feed. Boss height 3.5 mm. Thread M8 form-tapped. Visual finish smooth, minimal burrs.
Case 3 – Stainless steel 304 (1.5 mm): Ø5 mm hole, 3 200 rpm, 180 mm/min. Boss height 1.9 mm. Thread M5 cut-tapped. Required molybdenum disulfide lubrication.
10) Video Demonstration
11) Calculator (Interactive Tool)
Estimate rpm, feed and boss height
Values are approximate and depend on tool design, lubrication, and machine stiffness. Use for design guidance only.
How this calculator works (help)
Inputs
- Material – affects speed/torque targets.
- Wall thickness (t) – used for boss height estimation.
- Hole diameter (D) – drives rpm, feed and torque.
- Thread (optional) – only influences the tapping suggestion.
Outputs
- Spindle speed (rpm) – computed from a target surface speed
Vcby material. - Feed (mm/min) – simple heuristic proportional to diameter.
- Boss height (mm) – estimated multiple of
tby material. - Torque (Nm) – coarse estimate proportional to diameter.
Formulas
| RPM | n = (Vc × 1000) / (π × D) → shown as a ±15% range (clamped 1500–15000 rpm) |
| Feed | Feed ≈ k_material × D |
| Boss height | h ≈ f_material × t |
| Torque | T ≈ c_material × D |
Material constants (defaults)
| Material | Vc (m/min) | k_feed | f_boss | c_torque (Nm/mm) |
|---|---|---|---|---|
| Steel | 180 | 40 | 1.2 | 0.8 |
| Stainless | 120 | 30 | 1.1 | 1.2 |
| Aluminium | 240 | 45 | 1.4 | 0.35 |
| Brass/Copper | 160 | 35 | 1.0 | 0.5 |
Good practice & limits
- Use a light oil/paste; stainless needs careful lubrication.
- Ensure rigid clamping and correct alignment.
- The calculator is a starting point; fine-tune on trials for your tool geometry and machine.
- Consider cut tapping for stainless or D ≤ 4 mm; otherwise prefer form tapping.
Example (steel, t=2.0 mm, D=6.0 mm)
RPM ≈ 9 550 → range ~ 8 120–10 980 rpm; Feed ≈ 240 mm/min; Boss ≈ 2.4 mm; Torque ≈ 4.8 Nm; Suggestion: form tap.
12) References
- A. M. “Thermal Drilling of Metals,” Journal of Manufacturing Processes, Vol. 12 (2019).
- ISO 2768 – General tolerances for linear dimensions.
- DIN 8593-11 – Non-cutting manufacturing processes – Friction drilling.
- Smith, R. “Chipless Hole Forming by Friction,” Modern Machine Shop, 2020.
- J. K. Gupta – Manufacturing Processes Handbook, Springer, 2018.
- ASTM E646 – Standard Test Method for Tensile Strain-Hardening Exponent n of Metallic Sheet.
- Toolmaker Data Sheets – Kennametal, Flowdrill, etc.
- L. Zhao et al., “Experimental Study on Friction Drilling Parameters of Aluminium 6061,” Procedia Manufacturing, 2021.
This page is an educational resource and contains no commercial calls to action.