Drilling speeds and feeds

Drilling is a machining process by chip removal that uses a rotary multi-cutting tool (twist drill) to generate cylindrical holes. The cutting speed (Vc) is typically between 20 m/min and 150 m/min (66 ft/min and 492 ft/min) depending on the workpiece material, while the feed per revolution ranges from 0.02 mm/rev (0.0008 in/rev) for drill diameters under 1.5 mm (0.06 in) to 0.60 mm/rev (0.024 in/rev) for diameters over 25 mm (1 in). Proper cooling, chip evacuation, and spindle dynamic stability determine the final hole quality.

Operating parameters

The drilling regime is defined by cutting speed (Vc), feed (fn), and rotation speed (n). The following table summarizes the reference values for high-speed steel (HSS) twist drills in roughing operations.

Rotation speeds (RPM) by diameter and material

Drill diameter (mm)	Drill diameter (in)	Aluminum (RPM)	Mild steel (RPM)	Brass (RPM)	Softwood (RPM)	Hardwood (RPM)
1.6 – 4.8 mm	1/16 – 3/16 in	3 000	3 000	3 000	3 000	3 000
6.4 – 9.5 mm	1/4 – 3/8 in	2 500	1 000	1 200	3 000	1 500
11.1 – 15.9 mm	7/16 – 5/8 in	1 500	600	750	1 500	750
17.5 – 25.4 mm	11/16 – 1 in	1 000	350	400	750	500

Cutting speed (Vc) by material

Material	Recommended Vc (m/min)	Recommended Vc (ft/min)
Wrought aluminum alloys	100 – 150 m/min	328 – 492 ft/min
Cast aluminum alloys	60 – 100 m/min	197 – 328 ft/min
Brass and bronze	50 – 80 m/min	164 – 262 ft/min
Gray cast iron	20 – 40 m/min	66 – 131 ft/min
Carbon steel (0.15–0.30 %C)	25 – 35 m/min	82 – 115 ft/min
Alloy steel (4130, 4140)	15 – 25 m/min	49 – 82 ft/min
Austenitic stainless steel	10 – 20 m/min	33 – 66 ft/min
Titanium and alloys	8 – 15 m/min	26 – 49 ft/min
Softwood (pine)	300 – 600 m/min	984 – 1969 ft/min
Hardwood (oak, maple)	150 – 300 m/min	492 – 984 ft/min

Recommended feeds by material

The feed per revolution (fn) depends on the drill diameter and material. The values given are for HSS drills with standard sharpening.

Drill diameter (mm)	Drill diameter (in)	Feed in aluminum (mm/rev)	Feed in aluminum (in/rev)	Feed in steel (mm/rev)	Feed in steel (in/rev)	Feed in brass (mm/rev)	Feed in brass (in/rev)
1.5 – 3.0 mm	0.059 – 0.118 in	0.02 – 0.05 mm/rev	0.0008 – 0.0020 in/rev	0.02 – 0.04 mm/rev	0.0008 – 0.0016 in/rev	0.03 – 0.06 mm/rev	0.0012 – 0.0024 in/rev
3.0 – 6.0 mm	0.118 – 0.236 in	0.05 – 0.10 mm/rev	0.0020 – 0.0039 in/rev	0.04 – 0.08 mm/rev	0.0016 – 0.0031 in/rev	0.06 – 0.12 mm/rev	0.0024 – 0.0047 in/rev
6.0 – 12.0 mm	0.236 – 0.472 in	0.10 – 0.20 mm/rev	0.0039 – 0.0079 in/rev	0.08 – 0.15 mm/rev	0.0031 – 0.0059 in/rev	0.12 – 0.25 mm/rev	0.0047 – 0.0098 in/rev
12.0 – 25.0 mm	0.472 – 0.984 in	0.20 – 0.40 mm/rev	0.0079 – 0.0157 in/rev	0.15 – 0.30 mm/rev	0.0059 – 0.0118 in/rev	0.25 – 0.50 mm/rev	0.0098 – 0.0197 in/rev
25.0 – 50.0 mm	0.984 – 1.969 in	0.40 – 0.60 mm/rev	0.0157 – 0.0236 in/rev	0.25 – 0.40 mm/rev	0.0098 – 0.0157 in/rev	0.35 – 0.60 mm/rev	0.0138 – 0.0236 in/rev

Typical tolerances

The dimensional quality achievable in conventional drilling with a sharp twist drill corresponds to IT11–IT13. With a center drill and subsequent reaming, IT8–IT9 can be achieved. In high-precision orbital drilling, controlled eccentricity allows tolerances up to 0.01 mm (0.0004 in) on medium diameters, with axial force up to 80% lower than in conventional drilling, which eliminates delamination in composite materials.

Applicable materials

All engineering materials can be drilled with the appropriate combination of tool and parameters. Highlights:

• Wrought aluminum alloys (6061, 7075)
• Carbon and low-alloy steels (AISI 1018, 4140)
• Austenitic stainless steels (304, 316)
• Gray cast iron (GG20, GG25)
• Brass C360 and tin bronzes
• Titanium alloys (Ti-6Al-4V)
• Carbon fiber reinforced composites (CFRP)
• Softwoods (pine, fir) and hardwoods (oak, maple)
• Thermoplastic polymers (acrylic, polycarbonate)

For composite materials, orbital drilling with helical motion is recommended, which avoids interlaminar delamination.

Advantages and limitations

Drilling is compatible with most machine tools, supports a wide range of diameters from 0.1 mm (0.004 in) to over 80 mm (3.15 in), and provides holes with defined edges and sufficient precision for subsequent tapping or reaming operations.

Among the main limitations are the formation of conical holes at the bottom (inherent to the drill point), difficulty in evacuating chips in deep holes when the length/diameter ratio exceeds 3, possible drill deflection when entering oblique surfaces, and generation of irregular burrs at the exit. In conventional drilling, geometric tolerances are usually not less than 0.05 mm (0.002 in) without finishing operations.

Selection guide

The selection of parameters follows this logical sequence:

1. Determine the appropriate cutting speed (Vc) according to the workpiece material and drill material, using the cutting speed table.
2. Calculate the spindle rotation speed n (RPM) using the formula n = (Vc × 1000) / (π × D) with Vc in m/min and D in mm, or n = (Vc × 12) / (π × D) with Vc in ft/min and D in in.
3. Choose the feed per revolution (fn) according to drill diameter and material, consulting the feed table.
4. Verify that the spindle power is sufficient for the torque demanded by the operation, especially in large diameters and materials with low machinability.
5. Adjust the coolant flow rate: for aluminum, soluble emulsion 5‑7% is recommended; for steels, cutting oil or semi-synthetic emulsion; and for composite materials, dry drilling or with dust extraction is preferred.

Frequently Asked Questions (FAQ)

What is the recommended cutting speed for drilling stainless steel 304?

For stainless steel 304 with a high-speed steel (HSS) drill, a cutting speed between 10 m/min (33 ft/min) and 18 m/min (59 ft/min) is recommended, using abundant cooling to avoid work hardening of the material in the cutting zone.

What feed per revolution should be used for a 10 mm (0.394 in) drill on aluminum 6061?

In aluminum 6061 with a 10 mm (0.394 in) HSS drill, the recommended feed per revolution is between 0.12 mm/rev (0.0047 in/rev) and 0.18 mm/rev (0.0071 in/rev), which is equivalent to a penetration rate of approximately 180‑360 mm/min (7‑14 in/min) at a rotation speed of 2,500‑3,000 RPM.

How does the length/diameter ratio affect drilling parameters?

When the length/diameter ratio exceeds 3:1, the feed should be reduced by 20% to 40% to minimize drill deviation and risk of breakage. For ratios exceeding 10:1, the use of peck drilling cycles with retractions every 1.5 to 2 diameters is essential.

How many revolutions per minute does a 6 mm (0.236 in) drill need to drill carbon steel?

For a 6 mm (0.236 in) drill in carbon steel with a Vc of 28 m/min (92 ft/min), the calculated rotation speed is approximately 1,485 RPM, which in practice is adjusted to the nearest spindle step, normally 1,500 RPM.

What diametral tolerance can be achieved in conventional drilling without reaming?

In drilling with a properly sharpened twist drill, the diametral tolerance is in the IT11‑IT13 range, which for a nominal diameter of 10 mm (0.394 in) means an allowable variation of 0.09 mm (0.0035 in) to 0.22 mm (0.0087 in).

When is orbital drilling preferable to conventional drilling?

Orbital drilling is especially advantageous when machining composite materials (such as CFRP) or multi-material stacks (for example, titanium‑composite), where axial force is reduced by 70% to 80%, allowing tolerances below 0.02 mm (0.0008 in) and eliminating interlaminar delamination.

References

• engineeringtoolbox.com: https://www.engineeringtoolbox.com/drill-bit-speed-hardwood-softwood-d_1451.html
• efunda.com: https://www.efunda.com/processes/machining/drill_design.cfm
• manufacturingguide.com: https://www.manufacturingguide.com/en/orbital-drilling