CNC Speeds and Feeds: The Complete Guide for Machinists (2026)
Table of Contents
What Are Speeds and Feeds?
Speeds = how fast the cutting tool rotates. Measured in RPM (revolutions per minute) at the spindle, or SFM/m/min (surface feet per minute / metres per minute) at the cutting edge.
Feeds = how fast the tool moves through the material. Measured in mm/min or IPM (inches per minute) at the machine, or chip load (mm/tooth or inch/tooth) at each cutting edge.
Get either one wrong, and you either burn the tool, scrap the part, or both. Get them right, and you hit your cycle time, hold tolerance, and maximise tool life. It really is that binary.
The good news: the math is simple. Two formulas cover 90% of what you need. The rest is knowing which numbers to plug in — and that's what the charts and calculator on this page are for.
The Core Formulas Every Machinist Needs
1. Spindle Speed (RPM)
This is the most-used formula in CNC machining. You pick the SFM based on your material and tool type (see chart below), then calculate RPM. A ½" carbide end mill in 4140 steel at 450 SFM: (450 × 3.82) / 0.5 = 3,438 RPM.
2. Feed Rate
Chip load is how much material each tooth removes per revolution — typically 0.002-0.012 inch/tooth depending on material and operation. Same ½" 4-flute end mill at 3,438 RPM with 0.004" chip load: 3,438 × 4 × 0.004 = 55 IPM.
3. Material Removal Rate (MRR)
MRR tells you how fast you're removing cubic inches (or cm³) of material per minute. Higher MRR = shorter cycle time, but also higher cutting forces and heat. Balance MRR against tool life for your specific operation.
Surface Speed (SFM) Chart by Material
Surface speed is the single most important number to get right. Too high, the tool burns. Too low, it rubs. Here are starting values for carbide tooling. Reduce by 20-30% for HSS.
| Material | Carbide SFM | Carbide m/min | Notes |
|---|---|---|---|
| Aluminium 6061 | 600–1,200 | 180–365 | Use sharp polished tools; avoid built-up edge |
| Aluminium 7075 | 400–800 | 120–245 | Harder grade; reduce SFM by 30% vs 6061 |
| Mild Steel 1018 | 350–600 | 105–180 | Good starting point for all carbon steels |
| Alloy Steel 4140 | 250–450 | 75–135 | Reduce as hardness increases above 30 HRC |
| Tool Steel D2 | 150–300 | 45–90 | Hard and abrasive; use AlTiN-coated carbide |
| Stainless 304 | 150–350 | 45–105 | Work-hardens rapidly; never dwell |
| Stainless 316 | 120–300 | 35–90 | Harder than 304; reduce by 15-20% |
| Cast Iron (Grey) | 300–600 | 90–180 | Can machine dry; graphite self-lubricates |
| Titanium 6Al-4V | 100–200 | 30–60 | Low speeds essential; sharp tools, high-pressure coolant |
| Inconel 718 | 60–150 | 18–45 | Very low speeds; tough carbide grade; 70+ bar coolant |
| Brass C360 | 500–1,000 | 150–300 | Free-machining; can run fast; chips break easily |
| Copper C110 | 200–500 | 60–150 | Ductile; sharp tools essential to avoid smearing |
Chip Load: The Most Overlooked Parameter
Chip load (feed per tooth) is where most machinists get it wrong — and where the biggest tool life gains hide. A chip that's too thin doesn't cut; it rubs. A chip that's too thick overloads the cutting edge.
Recommended Chip Load Ranges (Carbide)
| Tool Diameter | Aluminium | Steel | Stainless | Titanium |
|---|---|---|---|---|
| 1/8" (3mm) | 0.001–0.003 | 0.0005–0.0015 | 0.0005–0.001 | 0.0005–0.001 |
| 1/4" (6mm) | 0.003–0.006 | 0.0015–0.003 | 0.001–0.002 | 0.001–0.002 |
| 3/8" (10mm) | 0.005–0.008 | 0.0025–0.005 | 0.002–0.004 | 0.0015–0.003 |
| 1/2" (12mm) | 0.006–0.012 | 0.003–0.006 | 0.002–0.005 | 0.002–0.004 |
| 3/4" (20mm) | 0.008–0.015 | 0.005–0.008 | 0.004–0.007 | 0.003–0.005 |
| 1" (25mm) | 0.010–0.020 | 0.006–0.012 | 0.005–0.010 | 0.004–0.008 |
Carbide vs HSS: Different Rules
Carbide and HSS tools use completely different speed ranges. Running carbide at HSS speeds wastes the tool's capability. Running HSS at carbide speeds destroys it instantly.
Key Differences
| Property | Carbide | HSS |
|---|---|---|
| Typical SFM in Steel | 250–600 | 60–120 |
| Max Temperature | ~800°C (coating dependent) | ~600°C |
| Hardness Retention | Excellent to 500°C+ | Softens above 500°C |
| Best For | Production, hard materials, high speeds | Prototypes, interrupted cuts, low-RPM ops |
| Cost per Edge | Higher purchase, lower per-part cost | Lower purchase, higher per-part cost in volume |
| Chip Load Range | 0.002–0.012 in/tooth | 0.001–0.006 in/tooth |
Rule of thumb: carbide runs 3-5× faster than HSS in the same material. If you're switching from HSS to carbide, multiply your RPM by 3 and your feed by 2 — then fine-tune from there.
7 Common Speeds and Feeds Mistakes
1. Running Too Slow (Seriously)
The number one mistake. Carbide needs heat and pressure to cut properly. At low speeds, the edge rubs instead of shearing, generating friction heat that stays in the tool instead of leaving with the chip. A silver, shiny chip in steel = you're rubbing. You want straw to light blue chips.
2. Chip Load Too Low
Below about 0.001" chip thickness, you're burnishing, not cutting. This is especially deadly in stainless and titanium where rubbing causes instant work hardening. Every subsequent tooth then tries to cut hardened material.
3. Ignoring Radial Chip Thinning
At stepovers under 50%, your actual chip is thinner than programmed. A 30% stepover needs roughly 40% higher programmed feed to maintain the same actual chip thickness. Failing to compensate means you're rubbing — see mistake #2.
4. Wrong SFM for the Material Hardness
4140 at 28 HRC cuts very differently from 4140 at 40 HRC. The SFM chart values assume annealed material. For hardened steel (35+ HRC), reduce SFM by 30-40%. For pre-hardened mould steels (P20 at 30 HRC), split the difference.
5. Not Adjusting for Tool Stick-Out
Every machinist knows a long tool chatters more, but few adjust speeds accordingly. Rule: for every 1× diameter of stick-out beyond 3×D, reduce SFM by 8-10%. A ½" end mill sticking out 3" (6×D) needs roughly 25% lower SFM than the same tool at 1.5" stick-out (3×D).
6. Using Coated Tools at HSS Speeds
AlTiN and TiAlN coatings need temperature to activate — they form a protective aluminium oxide layer at the cutting edge above 700°C. Run them too cold and you don't get this benefit. If your chips aren't at least golden in steel with AlTiN, you're leaving tool life on the table.
7. Trusting the Tool Catalog Blindly
Tool manufacturers publish ideal-condition numbers. Your 15-year-old VMC with 5µm spindle runout and 8% coolant concentration is not ideal conditions. Start at 70% of catalog speeds, prove the process, then increase. A tool that lasts 60 minutes at 80% speed makes more money than one that lasts 12 minutes at 100%.
Free Speed and Feed Calculator
Stop Guessing. Start Calculating.
Enter your tool diameter, number of flutes, material, and operation. Get starting RPM, feed rate, and chip load — no mental math required.
Open Speed & Feed Calculator →More calculators to dial in your entire machining process:
- SFM / Surface Speed Calculator — convert between RPM, SFM, and m/min
- Chip Load Calculator — verify your feed per tooth isn't rubbing
- MRR Calculator — calculate material removal rate for cycle time estimates
- Spindle Horsepower Calculator — make sure your machine can handle the cut
- Milling Force Calculator — calculate cutting forces and torque
- Cycle Time Calculator — estimate machining time for quoting
Frequently Asked Questions
What is the formula for speeds and feeds?
The two core formulas are: RPM = (SFM × 3.82) / tool diameter for speed, and Feed Rate = RPM × number of flutes × chip load for feed. Everything else — chip thinning compensation, ramp angle adjustment, trochoidal engagement — builds on these two equations.
What SFM should I use for 304 stainless steel?
Start at 150–350 SFM for carbide tooling in 304. If you have through-coolant and a rigid setup, push toward 300-350. Without through-coolant, stay at 150-200. HSS tools: 40-80 SFM. Always use positive rake geometry and never dwell on the surface — 304 work-hardens instantly.
How do I calculate feed rate from RPM?
Feed rate (IPM) = RPM × number of flutes × chip load. Example: 3,500 RPM, 4-flute end mill, 0.004" chip load = 3,500 × 4 × 0.004 = 56 IPM. For metric: feed rate (mm/min) = RPM × flutes × chip load (mm/tooth).
What is a good chip load for aluminium?
For carbide in aluminium: 0.005-0.012 inch/tooth depending on tool diameter. Smaller tools (under 1/4") use the low end; larger tools (1/2"+) use the high end. For HSS: reduce by 30%. Aluminium needs aggressive chip loads — going too light causes built-up edge.
Why does my carbide tool wear out so fast?
The most common causes: (1) running too slow (rubbing, not cutting), (2) chip load too low (burnishing), (3) wrong coating for the material, (4) excessive runout (over 0.0004" TIR), (5) inadequate coolant or wrong concentration. Check these five things before blaming the tool quality.
Can I use the same speeds for roughing and finishing?
Generally no. Roughing: use 70-80% of max SFM with aggressive chip loads to maximise MRR. Finishing: use 100% SFM with light chip loads for best surface finish. Some shops use the exact opposite logic — there's no single right answer. The key is that roughing and finishing have different goals (speed vs quality), so parameters should differ.