liminfoCNC Feeds and Speeds Complete Guide
A comprehensive, practical guide to mastering the most critical CNC milling parameters: SFM (Surface Feet per Minute), RPM (spindle speed), Feed Rate, Chip Load, and MRR (Material Removal Rate). Includes formulas, material-specific reference tables, and worked examples for aluminum, steel, stainless, and titanium.
Problem
Required Tools
A 3-axis or higher CNC mill. You must know your machine's maximum spindle RPM range (typically 100-24,000 RPM) and maximum feed rate capability.
Carbide or HSS endmills. Tool diameter, flute count (2-4 flutes), and coating type (TiAlN, ZrN, etc.) directly affect cutting parameters.
Online CNC feed and speed calculator at liminfo.com. Input material, tool diameter, and flute count to automatically calculate RPM, feed rate, and MRR.
Recommended SFM and chip load data from manufacturers like Kennametal, Sandvik, or OSG. Provides detailed parameters based on coating type and tool geometry.
Solution Steps
Understand SFM (Surface Feet per Minute) by Material
SFM (Surface Feet per Minute) is the speed at which the cutting edge of the tool travels across the workpiece surface. It is the starting point for all feed and speed calculations, and the recommended range varies significantly by material. If SFM is too high, the tool overheats and wears rapidly. If SFM is too low, the tool rubs instead of cutting, which paradoxically accelerates wear and can cause work hardening in certain alloys. Recommended SFM ranges for carbide endmills: | Material | SFM Range | Notes | |---------------------|----------------|-------------------------------| | Aluminum (6061) | 500 - 1,000 | Higher with coated tools | | Mild Steel (1018) | 60 - 100 | General purpose | | Alloy Steel (4140) | 40 - 80 | Adjust for hardness | | Stainless (304) | 40 - 80 | Watch for work hardening | | Stainless (316) | 35 - 65 | Lower than 304 | | Titanium (6Al-4V) | 30 - 60 | Low speed, high feed strategy | | Brass (C360) | 200 - 400 | Free machining alloy | | Plastic (Acetal) | 300 - 800 | Watch for melting | For HSS tools, reduce these values by approximately 40-50%. For metric (SMM - Surface Meters per Minute): SMM = SFM x 0.3048
# Recommended SFM Ranges (Carbide Endmill)
#
# Material SFM Low SFM High Notes
# -------------------------------------------------------
# Aluminum 6061 500 1000 Uncoated OK
# Mild Steel 1018 60 100 General purpose
# Alloy Steel 4140 40 80 Adjust for hardness
# Stainless 304 40 80 Watch work hardening
# Stainless 316 35 65 Lower than 304
# Titanium 6Al-4V 30 60 Low speed, high feed
# Brass C360 200 400 Free machining
# Acetal / Delrin 300 800 Watch melting
#
# HSS tools: multiply above SFM by 0.50 ~ 0.60
# Metric conversion: SMM = SFM × 0.3048Calculate RPM (Spindle Speed)
Once you have determined the appropriate SFM for your material, calculate the spindle RPM using the tool diameter. Formula (Imperial): RPM = (SFM x 3.82) / Tool Diameter (inches) Formula (Metric): RPM = (SMM x 1000) / (pi x Tool Diameter in mm) The constant 3.82 is the approximation of 12 / pi (precisely 3.8197...). If the calculated RPM exceeds your machine's maximum spindle speed, set the RPM to the machine's maximum and back-calculate the feed rate accordingly. Example 1: Aluminum 6061, 1/2" (0.5") carbide endmill, SFM = 800 RPM = (800 x 3.82) / 0.5 = 6,112 RPM Example 2: Stainless 304, 3/8" (0.375") carbide endmill, SFM = 60 RPM = (60 x 3.82) / 0.375 = 611 RPM Example 3: Titanium 6Al-4V, 10mm carbide endmill, SMM = 15 RPM = (15 x 1000) / (3.14159 x 10) = 477 RPM
# RPM Calculation Formula
#
# === Imperial (inches) ===
# RPM = (SFM × 3.82) / Tool Diameter (inches)
#
# === Metric (mm) ===
# RPM = (SMM × 1000) / (π × Tool Diameter in mm)
#
# -------------------------------------------------------
# Worked Examples
# -------------------------------------------------------
#
# Example 1: Aluminum 6061, 1/2" carbide endmill, SFM=800
# RPM = (800 × 3.82) / 0.500 = 6,112 RPM
#
# Example 2: Stainless 304, 3/8" carbide endmill, SFM=60
# RPM = (60 × 3.82) / 0.375 = 611 RPM
#
# Example 3: Titanium 6Al-4V, 10mm carbide endmill, SMM=15
# RPM = (15 × 1000) / (3.14159 × 10) = 477 RPM
#
# -------------------------------------------------------
# NOTE: If calculated RPM exceeds machine maximum,
# clamp to machine max and recalculate feed rateCalculate Feed Rate (IPM / mm per min)
The Feed Rate is the linear speed at which the table (and workpiece) moves relative to the cutter. It is calculated from RPM, flute count, and chip load per tooth. Formula: Feed Rate (IPM) = RPM x Number of Flutes x Chip Load per Tooth (inches) Chip Load is the thickness of material each flute removes per revolution. Consult your tool manufacturer's catalog for recommended values based on material and tool diameter. Typical chip load reference values for carbide endmills: | Tool Diameter | Aluminum | Mild Steel | Stainless | Titanium | |----------------|---------------|--------------|--------------|---------------| | 1/8" (3mm) | 0.001-0.003 | 0.0005-0.001 | 0.0004-0.0008| 0.0003-0.0006 | | 1/4" (6mm) | 0.002-0.005 | 0.001-0.003 | 0.001-0.002 | 0.0008-0.0015 | | 1/2" (12mm) | 0.004-0.008 | 0.002-0.005 | 0.002-0.004 | 0.001-0.003 | | 3/4" (20mm) | 0.005-0.010 | 0.003-0.006 | 0.003-0.005 | 0.002-0.004 | Example: Aluminum 6061, 1/2" 3-flute endmill, SFM = 800 RPM = 6,112 Chip Load = 0.005 in/tooth Feed Rate = 6,112 x 3 x 0.005 = 91.7 IPM To convert to metric: mm/min = IPM x 25.4
# Feed Rate Calculation Formula
#
# Feed Rate (IPM) = RPM × Number of Flutes × Chip Load per Tooth
#
# Units:
# IPM = Inches Per Minute
# Chip Load = inches/tooth
# mm/min = IPM × 25.4
#
# -------------------------------------------------------
# Worked Examples
# -------------------------------------------------------
#
# Aluminum 6061, 1/2" 3-flute carbide endmill, SFM=800
# Step 1: RPM = (800 × 3.82) / 0.5 = 6,112
# Step 2: Chip Load = 0.005 in/tooth (from catalog)
# Step 3: Feed = 6,112 × 3 × 0.005 = 91.7 IPM
# Step 4: Metric = 91.7 × 25.4 = 2,329 mm/min
#
# Stainless 304, 3/8" 4-flute carbide endmill, SFM=60
# Step 1: RPM = (60 × 3.82) / 0.375 = 611
# Step 2: Chip Load = 0.0015 in/tooth
# Step 3: Feed = 611 × 4 × 0.0015 = 3.67 IPM
# Step 4: Metric = 3.67 × 25.4 = 93.1 mm/minOptimize Chip Load — Finding the Sweet Spot
Chip Load is one of the most critical variables determining CNC machining quality. It represents the thickness of material each cutting edge removes per revolution. When chip load falls outside the optimal range, distinct problems arise. When chip load is too low (rubbing): - Friction rather than cutting generates excessive heat at the tool edge. - Tool wear actually accelerates, and the surface develops a polished "burnished" appearance. - Stainless steel and titanium undergo work hardening, making each subsequent pass harder to cut. - BUE (Built-Up Edge) forms as workpiece material welds onto the cutting edge. When chip load is too high (overload): - Excessive cutting forces risk tool breakage or edge chipping. - Chatter vibration intensifies and surface finish degrades dramatically. - The spindle motor may overload, triggering machine alarms or stalling. - Chips become too thick for proper evacuation, causing recutting and packing. Tips for finding the optimal range: 1. Start at the midpoint of the manufacturer's recommended chip load range. 2. Observe chip shape — for aluminum, a "6" or "9" curl shape indicates healthy cutting. 3. Listen to the cutting sound — consistent, steady sound indicates stability. 4. Adjust in 10% increments, changing only one variable at a time to isolate the effect.
# Chip Load Optimization Diagnostic Guide
#
# === Signs of Chip Load Too LOW ===
# - Chips are dust/powder → rubbing, not cutting
# - BUE (built-up edge) forming on tool
# - Burnished/polished surface appearance
# - Stainless/Ti: subsequent passes become harder (work hardening)
#
# === Signs of Chip Load Too HIGH ===
# - Severe chatter vibration and noise
# - Tool breakage or edge chipping
# - Spindle overload alarm
# - Chips packing or not evacuating
#
# === Signs of OPTIMAL Chip Load ===
# - Consistent curl-shaped chips
# - Steady, even cutting sound
# - Clean, uniform surface finish
# - Gradual, even tool wear pattern
#
# === Adjustment Strategy ===
# 1. Start at midpoint of manufacturer range
# 2. Adjust in 10% increments
# 3. Change ONE variable at a time
# 4. Monitor chip shape, sound, surface quality
# 5. Log results to build your own material/tool databaseMRR (Material Removal Rate) and Depth of Cut Adjustment
MRR (Material Removal Rate) is the volume of material removed per unit time — the key metric for machining efficiency. Higher MRR means shorter cycle times, but it must stay within the limits of your machine and tooling. MRR Formula: MRR = WOC x DOC x Feed Rate WOC (Width of Cut): Radial engagement — how wide the tool engages the material DOC (Depth of Cut): Axial engagement — how deep the tool plunges into the material Feed Rate: Table feed speed (IPM or mm/min) MRR units: in^3/min or cm^3/min General depth of cut guidelines (relative to tool diameter D): - Conventional machining: DOC = 1xD, WOC = 0.25-0.50xD - High Speed Machining (HSM): DOC = 2-3xD, WOC = 0.05-0.15xD (light radial, deep axial) - Finishing: DOC = 0.5-1xD, WOC = 0.05-0.10xD (precision surface) - Slotting (full-width cut): WOC = 1xD, DOC = 0.5-1xD Example: Aluminum 6061, 1/2" 3-flute endmill Feed Rate = 91.7 IPM WOC = 0.25" (50% of tool diameter) DOC = 0.5" (1x tool diameter) MRR = 0.25 x 0.5 x 91.7 = 11.5 in^3/min HSM / Adaptive strategies reduce WOC while increasing DOC, maintaining constant tool engagement and achieving high MRR with less stress on the tool.
# MRR (Material Removal Rate) Calculation
#
# MRR = WOC × DOC × Feed Rate
#
# WOC = Width of Cut (radial engagement)
# DOC = Depth of Cut (axial engagement)
# Feed Rate = IPM or mm/min
#
# -------------------------------------------------------
# Worked Examples
# -------------------------------------------------------
#
# === Conventional Machining ===
# Aluminum 6061, 1/2" 3-flute, SFM=800
# Feed Rate = 91.7 IPM
# WOC = 0.250" (50% of D)
# DOC = 0.500" (1×D)
# MRR = 0.250 × 0.500 × 91.7 = 11.46 in³/min
#
# === High Speed Machining (HSM / Adaptive) ===
# Aluminum 6061, 1/2" 3-flute, SFM=1000
# RPM = (1000 × 3.82) / 0.5 = 7,640
# Chip Load = 0.005 → Feed = 7640 × 3 × 0.005 = 114.6 IPM
# WOC = 0.075" (15% of D)
# DOC = 1.000" (2×D)
# MRR = 0.075 × 1.000 × 114.6 = 8.60 in³/min
#
# === Depth of Cut Guidelines (relative to D) ===
# Conventional: DOC = 1.0×D, WOC = 0.25~0.50×D
# HSM/Adaptive: DOC = 2.0~3.0×D, WOC = 0.05~0.15×D
# Finishing: DOC = 0.5~1.0×D, WOC = 0.05~0.10×D
# Slotting: DOC = 0.5~1.0×D, WOC = 1.0×DCommon Mistakes
Not accounting for machine rigidity when applying theoretical values
Manufacturer-recommended SFM and chip load values assume optimal conditions: a rigid machine, short tool stick-out, and solid workholding. On desktop CNCs, with long tool overhangs, or when machining thin walls, reduce SFM and DOC by 30-50% as a starting point. Increase gradually while monitoring for chatter. A smaller machine running at 60% of theoretical values will often outperform one pushed to chatter.
Ignoring chip evacuation while increasing depth of cut
In slotting (full-width cuts) and deep pocket operations, re-cutting packed chips causes rapid tool wear and potential breakage. Use air blast, through-tool coolant, and appropriate flute count (2-flute recommended for aluminum slotting to maximize chip pocket size). For deep pockets, use helical ramp entry or peck drilling strategies. In blind holes, consider ramping at 2-3 degrees rather than plunging.
Running stainless steel and titanium too slowly, causing work hardening
Stainless steels (304, 316) and titanium alloys work-harden when the tool rubs instead of cuts. If the chip load is too low, the surface hardens, making the next pass even more difficult — creating a destructive cycle. Always maintain SFM at or above the lower end of the recommended range, and use adequate chip load to ensure the tool is "biting" into fresh material. Chips should form curls, not dust or powder.
Using the wrong flute count and tool coating for the material
Soft materials like aluminum need 2-3 flute endmills with large chip pockets for evacuation. Hard materials like steel benefit from 4+ flutes for higher feed rates. Using a 4-flute endmill in aluminum risks chip packing and re-cutting; using 2 flutes in steel yields unnecessarily slow feed rates. Coating matters too: uncoated or ZrN for aluminum, TiAlN for steel, and AlCrN for titanium are standard recommendations.
Changing SFM and feed rate simultaneously, making it impossible to diagnose issues
When troubleshooting or optimizing cutting parameters, change only one variable at a time. Set RPM (via SFM) first, then adjust chip load (feed rate). If you change both simultaneously, you cannot determine which variable caused the improvement or degradation. Keep a log of your settings and results to build a material/tool combination database — this becomes your most valuable shop floor reference over time.