Complete CNC Drilling Feeds & Speeds Guide
Charts, formulas and real shop examples for calculating drill RPM and feed rate — plus how to choose HSS vs carbide, handle deep holes, set coolant, and fix broken or burning drills. Backed by our production CNC engineers.
On this page
Quick Answer What Are Feeds & Speeds? Key Parameters RPM Formula Feed Rate Formula Feed per Revolution vs per Tooth Material Charts (Al / SS / Ti / Brass / Copper / Cast Iron / Plastic) Tool Material: HSS vs Carbide Hole Depth Rules Coolant Strategy Machine Rigidity & Tuning Common Problems & Adjustment Guide Interactive Drill Calculator Worked Example: Ø10 in 6061 How Goldcattle Optimizes Drilling FAQ Machining Parameters Hub Get a CNC Drilling QuoteWhat are CNC drilling feeds and speeds?
CNC drilling feeds and speeds define the relationship between spindle speed (RPM), feed rate, drill diameter, tool material, workpiece material, coolant strategy, and hole depth. RPM comes from the cutting speed and drill diameter RPM = (1000 × Vc) ÷ (π × D), and feed rate = RPM × feed per revolution. Published charts are starting points — always adjust for chip formation, machine rigidity, tool geometry, and cutting conditions.
What Are Feeds & Speeds in Drilling?
Most "speeds and feeds" pages dump a table and stop. To actually run a drill well you need to understand the four quantities behind every number in that table.
Vc Cutting Speed (Surface Speed)
How fast the drill's cutting edge travels relative to the workpiece, measured in m/min (metric) or SFM (surface feet per minute, imperial). It depends mainly on tool and workpiece material — not on diameter.
n Spindle Speed (RPM)
How many revolutions per minute the spindle makes. It is derived from cutting speed and drill diameter. RPM is not "higher is better" — too high burns the tool, too low makes it rub and break.
ƒ Feed Rate
How fast the tool advances into the material, in mm/min (or IPM, inches per minute). The drill advances along its axis; this is the total linear feed.
ƒr Feed per Revolution
The axial distance the drill moves in one spindle turn (mm/rev or IPR). This is the value drill charts actually recommend — not feed per tooth. See the next section for why.
Key Parameters at a Glance
The variables that decide your final numbers, and which ones you control on the machine.
| Parameter | Symbol | Unit | Set by | You tune it for |
|---|---|---|---|---|
| Cutting speed | Vc | m/min · SFM | Tool + workpiece | Heat, tool life |
| Spindle speed | n / RPM | rev/min | Formula from Vc & D | Calculated, then fine-tuned |
| Feed per rev | fr | mm/rev · IPR | Tool + workpiece | Chip shape, rigidity |
| Feed rate | vf | mm/min · IPM | RPM × fr | Throughput |
| Drill diameter | D | mm · inch | Engineering drawing | — |
| Hole depth | L | × diameter (D) | Drawing | Peck cycle, feed % |
How to Calculate Drill RPM
RPM keeps the cutting edge moving at the target surface speed regardless of drill size. A small drill must spin much faster than a large one for the same Vc.
How to Calculate Feed Rate
Once RPM is known, feed rate is simply how far the drill moves each turn, times how many turns per minute.
Feed per Revolution vs Feed per Tooth
This is the detail most pages get wrong or skip — and it is one of the highest-value points for a machinist.
ƒr Feed per Revolution (IPR / mm/rev)
The standard unit for drills. A drill has one cutting edge per flank, so "per tooth" and "per revolution" are effectively the same. Drill charts list this value. This is what you type into the control as the feed.
ƒz Feed per Tooth (IPT / mm/tooth)
The standard unit for mills (end mills, face mills). With multiple flutes, total feed = RPM × fz × number of teeth. Never apply a mill's per-tooth value directly to a drill — the drill would feed far too slowly.
Material Charts: Cutting Speed & Feed
Starting-point values for common engineering materials. These are ranges, not laws — revise them after the first article (see Machine Rigidity below). HSS on the left, carbide on the right of each pair.
Aluminum (e.g. 6061-T6)
| Tool | Vc (m/min) | Feed/rev (mm/rev) | Notes |
|---|---|---|---|
| HSS | 60–90 | 0.08–0.15 | Easy to drill; watch for built-up edge at low speed |
| Carbide | 120–200 | 0.10–0.20 | High speed OK; use through-coolant for deep holes |
Stainless Steel (e.g. 304 / 316L)
| Tool | Vc (m/min) | Feed/rev (mm/rev) | Notes |
|---|---|---|---|
| HSS | 15–30 | 0.05–0.10 | Work-hardens — keep feed up, use peck (G83) |
| Carbide | 50–90 | 0.06–0.12 | Sharp edge, generous coolant; avoid dwelling |
Titanium (Ti-6Al-4V)
| Tool | Vc (m/min) | Feed/rev (mm/rev) | Notes |
|---|---|---|---|
| HSS | 10–20 | 0.04–0.08 | Low speed, high coolant pressure |
| Carbide | 30–60 | 0.05–0.10 | Through-coolant strongly recommended; peck cycle |
Brass & Copper
| Tool | Vc (m/min) | Feed/rev (mm/rev) | Notes |
|---|---|---|---|
| HSS (Brass) | 60–100 | 0.08–0.18 | Free-cutting; can run fast |
| Carbide (Brass) | 150–250 | 0.10–0.22 | Watch for long stringy chips |
| HSS (Copper) | 40–80 | 0.06–0.12 | Soft, gummy — keep speed moderate |
| Carbide (Copper) | 100–180 | 0.08–0.15 | Polished flutes reduce sticking |
Cast Iron (e.g. GG25)
| Tool | Vc (m/min) | Feed/rev (mm/rev) | Notes |
|---|---|---|---|
| HSS | 25–45 | 0.07–0.12 | Abrasive — watch margin wear |
| Carbide | 70–120 | 0.10–0.18 | Often drilled near-dry; chips are powdery |
Engineering Plastics (POM / ABS / PEEK)
| Tool | Vc (m/min) | Feed/rev (mm/rev) | Notes |
|---|---|---|---|
| HSS | 50–100 | 0.08–0.18 | Sharp, high-helix drill; watch melting on PE/ABS |
| Carbide | 150–300 | 0.10–0.25 | PEEK needs coolant or careful dry; avoid heat |
Tool Material: HSS vs Carbide (and beyond)
The right tool changes both the safe speed and how fragile the process is.
H HSS (High-Speed Steel)
Pros: tough, forgiving, cheap, survives vibration and interruption. Cons: low max speed, wears fast on abrasive/hard materials. Best for low-volume, soft materials, or any machine with noticeable runout or flex.
C Carbide
Pros: 2–4× the surface speed of HSS, long life, great finish. Cons: brittle — demands rigidity, low overhang, good holders and coolant. On a stiff setup it is almost always faster and cheaper per hole.
⌀ Indexable Insert Drill
For larger diameters (typically ≥ 12–16 mm) insert drills replace the whole tool less often and handle high material removal. Slower surface speed than solid carbide but very economical per hole in production.
💧 Through-Coolant Drill
Internal channels deliver coolant straight to the cutting edge. Essential for deep holes, titanium, stainless, and high feed rates — it evacuates chips and controls heat where a flood nozzle cannot reach.
Hole Depth Rules (1D → 10D)
Depth expressed as multiples of diameter (D). The deeper the hole, the harder chips escape and the more heat builds — so you reduce feed and switch to peck drilling.
| Depth | Feed % | Strategy | Coolant |
|---|---|---|---|
| 1D – 3D | 100% | Standard drilling (G81) | Flood OK |
| 3D – 5D | ~80% | Short peck optional | Flood / mist |
| 5D – 8D | ~60% | Peck (G83) | Through-coolant preferred |
| 8D – 10D | 40–50% | Peck (G83), small Q steps | Through-coolant required |
| >10D | ~30% | Deep-hole / gun drill, peck | Through-coolant, high pressure |
Coolant Strategy
💧 Flood
Standard for shallow holes in most materials. Cools and flushes, but struggles to reach the bottom of deep holes.
➤ Through-Coolant
Best for deep holes, titanium, stainless. Delivers fluid at the edge, evacuates chips, extends tool life dramatically.
🌫 Mist / Dry
Cast iron is often drilled near-dry (dust control). Some plastics prefer dry or light mist to avoid heat buildup and absorption.
Machine Rigidity & Why Charts Are Starting Points
A number from a chart is only as good as the machine it runs on. These factors decide whether you can actually hit the book value.
⚙ Machine rigidity
A stiff VMC holds high feed; a worn or lightly-built machine needs lower values to avoid chatter and walking.
🔧 Holder & overhang
Long drill extensions and flexible holders multiply deflection. Keep overhang short and use a quality ER/ hydraulic chuck.
◎ Runout
Excess runout overloads one flute, breaks drills and oversizes holes. Aim for < 0.01 mm at the tool.
🛡 Material hardness
Hardened stock, skins and inclusions shift the safe speed down. Verify hardness before trusting the chart.
Common Problems & How to Adjust
The fastest way to tune parameters is to read what the cut is telling you. Match the symptom, then make the adjustment.
| Symptom | Possible Cause | Recommended Adjustment |
|---|---|---|
| Drill squeals | Feed too low / RPM too high | Raise feed slightly, reduce spindle speed |
| Built-up edge | Speed too low, poor lubrication | Increase cutting speed, improve coolant, use polished drill |
| Oversized hole | Runout, worn drill | Check holder runout, replace drill, shorten overhang |
| Poor chip evacuation | No peck / weak coolant | Use G83 peck cycle, add through-coolant |
| Short tool life | Excessive heat | Reduce speed, verify chip load, improve coolant |
| Blue chips / burnt hole | Too much heat | Lower RPM, raise feed, increase coolant flow |
| Drill breakage | Feed too high, runout, no peck | Lower feed, check runout, add peck on deep holes |
Quick Decision Tree
Drill RPM & Feed Calculator
Pick a material and tool to auto-fill starting values, then edit them to match your machine. The calculator updates RPM and feed rate live.
Inputs
Results
Note: results are theoretical starting points. Always verify on the machine and adjust for rigidity, coolant and chip formation.
Worked Example: Ø10 Carbide Drill in 6061 Aluminum
Why the final production number is rarely the textbook number — and how we get there.
Start from the chart: carbide in 6061 → Vc ≈ 180 m/min, feed/rev ≈ 0.16 mm.
RPM = (1000 × 180) ÷ (π × 10)
= 180000 ÷ 31.416
≈ 5730 RPM (theoretical)
Feed = 5730 × 0.16 ≈ 917 mm/min
On the floor we measured chatter at the collet and a slightly flexible fixture, so we stepped RPM down to 5400 and held feed near 860 mm/min. Hole quality, size and tool life all improved.
| Step | Value |
|---|---|
| Material | Al 6061-T6 |
| Tool | Ø10 solid carbide, Al TiN |
| Chart Vc | 180 m/min |
| Theoretical RPM | 5730 |
| Used RPM | 5400 |
| Feed/rev | 0.16 mm/rev |
| Used feed | ~860 mm/min |
| Coolant | Flood + through |
How Goldcattle Optimizes Drilling for Production
We do not ship the tooling catalog's first number. Every production drilling process goes through the same engineering loop.
1 First-article check
We drill the first part, measure diameter, position and finish, and confirm the process hits the print before any volume runs.
2 Chip & sound read
Engineers watch chip shape and listen for squeal or rubbing, then nudge RPM and feed toward the stable window.
3 Tool-life validation
For aerospace, medical, automotive and robotics parts we log tool life and lock the tuned parameters as the production standard.
Frequently Asked Questions
Machining Parameters Hub
This page is the core reference of our Machining Parameters knowledge cluster. Explore the connected guides to build the full picture.
Need Optimized CNC Drilling for Production Parts?
From prototypes to 100,000+ pieces — our manufacturing engineers tune feeds, speeds, tooling and coolant for your exact material and tolerance.
- Aluminum, steel, stainless, brass, titanium, plastics
- Prototype → production, no MOQ
- Deep-hole & micro drilling
- Precision hole machining (±0.005 mm)
- Process optimization by engineers
- Dimensional & inspection reports
