Calculate a starting point
Feeds and Speeds Calculator & Starting Chart
Surface speed sets RPM; chip load, flute count, and operating RPM set table feed.
Default example: a ½ in, 4-flute HSS end mill in aluminum at 250 SFM and 0.008 in/tooth calculates to about 1,910 RPM and 61.1 in/min. Use the controls for your starting point.
Source state
UF DML aluminum HSS starting values; chip load midpoint selected for the example.
Starting values, not machine approval
Confirm the actual cutter manufacturer’s recommendations and account for material condition, tool geometry/coating, radial and axial engagement, rigidity, runout, coolant, workholding, and machine limits before cutting.
Source-limited reference
Milling Feeds and Speeds Starting Chart
A limited transformed subset of University of Florida DML guidance for common materials.
Search or filter the chart. Use a row to load its starting values into the calculator; the carbide speed shown is the UF HSS value multiplied by the source-stated 2.5× carbide factor.
No supported material matches these filters. Clear the filter or choose Custom in the calculator and enter your cutter manufacturer’s values.
Scroll horizontally to view additional columns and vertically to view additional rows. Column headers remain visible while scrolling.
| Cutting Speed | End-Mill Chip Load Range | Source Applicability | Use | ||||
|---|---|---|---|---|---|---|---|
| Acetal (Delrin) | Polymer | 250 SFM (76.2 m/min) | 625 SFM (190.5 m/min) | 0.008 IPT (0.2032 mm/tooth) | 0.030 IPT (0.7620 mm/tooth) | UF DML conservative; chip-load range typical for ½–1½ in cutters | |
| Aluminum and its alloys | Aluminum | 250 SFM (76.2 m/min) | 625 SFM (190.5 m/min) | 0.004 IPT (0.1016 mm/tooth) | 0.012 IPT (0.3048 mm/tooth) | UF DML conservative; chip-load range typical for ½–1½ in cutters | |
| Brass (360 high machining) | Copper Alloy | 250 SFM (76.2 m/min) | 625 SFM (190.5 m/min) | 0.004 IPT (0.1016 mm/tooth) | 0.012 IPT (0.3048 mm/tooth) | UF DML conservative; chip-load range typical for ½–1½ in cutters | |
| Cast Iron (medium hard) | Cast Iron | 80 SFM (24.4 m/min) | 200 SFM (61.0 m/min) | 0.002 IPT (0.0508 mm/tooth) | 0.006 IPT (0.1524 mm/tooth) | UF DML conservative; chip-load range typical for ½–1½ in cutters | |
| Mild steel (.2-.3 C) | Steel | 100 SFM (30.5 m/min) | 250 SFM (76.2 m/min) | 0.002 IPT (0.0508 mm/tooth) | 0.008 IPT (0.2032 mm/tooth) | UF DML conservative; chip-load range typical for ½–1½ in cutters | |
| Stainless steel (free machining) | Stainless Steel | 40 SFM (12.2 m/min) | 100 SFM (30.5 m/min) | 0.002 IPT (0.0508 mm/tooth) | 0.006 IPT (0.1524 mm/tooth) | UF DML conservative; chip-load range typical for ½–1½ in cutters | |
| Stainless steel (work hardening) | Stainless Steel | 20 SFM (6.1 m/min) | 50 SFM (15.2 m/min) | 0.0015 IPT (0.0381 mm/tooth) | 0.004 IPT (0.1016 mm/tooth) | UF DML conservative; chip-load range typical for ½–1½ in cutters | |
| Titanium alloys | Titanium | 20 SFM (6.1 m/min) | 50 SFM (15.2 m/min) | 0.0015 IPT (0.0381 mm/tooth) | 0.004 IPT (0.1016 mm/tooth) | UF DML conservative; chip-load range typical for ½–1½ in cutters | |
These are conservative DML starting values, not universal optimum settings. The UF end-mill feed table states its values are typical for approximately ½–1½ in cutters. For other diameters, specialized cutters, coatings, or production machining, use the cutter manufacturer’s application data.
Table actions
Bulk CSV download is intentionally unavailable because the source table’s open-reuse rights were not verified.
How to Read a Feeds and Speeds Chart
A feeds-and-speeds chart provides starting values for two different parts of the machining problem. Cutting speed describes the peripheral speed of the cutting edge relative to the workpiece. Chip load describes the linear advance assigned to each tooth. Cutter diameter converts cutting speed into spindle RPM; flute count converts chip load and RPM into table feed.
- SFM / Vc
- Surface or cutting speed at the cutter circumference.
- RPM / N
- Rotational spindle speed required for the selected diameter and cutting speed.
- IPT / fz
- Chip load, or feed per cutting tooth.
- IPM / mm/min
- Linear table feed produced by RPM × flutes × chip load.
SFM vs RPM: Why Cutter Diameter Changes Speed
RPM is not a material property. It is calculated from the target surface speed and tool diameter. At the same SFM, a smaller cutter must rotate faster because each revolution covers less circumference.
For inch units, use RPM = (12 × SFM) ÷ (π × D). For metric units, use RPM = (1000 × Vc) ÷ (π × D), where Vc is in m/min and D is in millimeters.
The calculator uses exact π and rounds only for display.
Diameter matters
At 250 SFM, a 1 in cutter is about 955 RPM, while a ½ in cutter is about 1,910 RPM. The cutting-edge surface speed is the same.
Chip Load and Feed Rate
For milling, linear feed follows Feed = RPM × flutes × chip load per tooth. If RPM or flute count changes while the target chip load stays the same, feed must change with it. This is why an RPM cap in the calculator also changes the displayed feed rate.
Use IPM with in/tooth, or mm/min with mm/tooth.
Reducing feed without considering RPM can make the actual chip thickness too small, increasing rubbing instead of improving the cut. Manufacturer guidance should take precedence when it is available for the specific cutter, coating, material condition, and engagement.
Worked Milling Examples
1 in HSS end mill in aluminum
Assumptions: 250 SFM, 4 flutes, 0.008 in/tooth, 1.000 in diameter.
RPM = (12 × 250)/(π × 1.000) = 954.9 RPM.
Feed = 954.9 × 4 × 0.008 = 30.6 in/min.
Sanity check: UF’s rounded instructional example reports about 950 RPM and 30 in/min before its lab-specific manual-oil reduction.
½ in carbide end mill with a 4,000 RPM machine limit
Assumptions: aluminum, 625 SFM from the UF 2.5× carbide rule, 3 flutes, 0.004 in/tooth.
Unrestricted RPM is 4,774.6, so a 4,000 RPM machine cap governs.
Feed = 4,000 × 3 × 0.004 = 48.0 in/min; effective cutting speed becomes about 523.6 SFM.
Limitation: the generic source value does not account for a specific carbide grade, coating, radial engagement, or toolholder.
When the Chart Is Not Enough
A generic chart is best used to establish a conservative starting region. Final parameters can move materially when the cutter, operation, machine, or workpiece differs from the source assumptions.
Use manufacturer data first
- Specific carbide grade or coating
- Specialized rougher, finisher, or high-feed geometry
- Small-diameter or micro tooling
- Known radial/axial engagement recommendations
Check the machine setup
- Spindle RPM and power limits
- Toolholder runout and rigidity
- Workholding stiffness
- Coolant delivery and chip evacuation
Check the material condition
- Hardness and heat treatment
- Work-hardening behavior
- Cast skin, scale, or interrupted cuts
- Actual alloy when the generic family is broad
How to Adjust a Starting Point
Treat chatter, rubbing, heat, poor finish, chip packing, and work hardening as different failure modes rather than automatically lowering both speed and feed. A change that helps one problem can worsen another.
- Chatter: verify workholding, tool overhang, holder condition, spindle stability, engagement, and whether speed needs to move away from a resonance.
- Rubbing or heat with tiny chips: check whether feed per tooth is too low for the cutter and whether runout is causing one flute to carry most of the load.
- Chip packing: improve evacuation, reduce engagement or depth where appropriate, and verify coolant/air delivery before simply slowing the spindle.
- Work-hardening materials: avoid dwelling and use the actual toolmaker’s guidance for chip load and cutting speed.
Record stable results from your own machine, tool, holder, material heat/lot, coolant, and engagement. Shop-proven data tied to a controlled setup is more useful than a generic chart once the process is established.
Source Scope, Data Rights & Accuracy
This page uses a limited transformed subset of University of Florida DML guidance and calculates RPM/feed from published machining relationships.
The University of Florida page explicitly describes its surface-speed values as conservative for DML equipment. Its end-mill feed table states that chip-load values are typical for cutters from approximately ½ in to 1½ in. The source also states that carbide cutting tools may use 2.5× the listed HSS surface speed; this page labels that value as derived rather than as independent manufacturer data.
- University of Florida — Speeds and FeedsControlling source for Equation (1), Equation (3), the limited material subset, chip-load ranges, and the 2.5× carbide factor.
- Kennametal — Speeds and Feeds CalculatorIndependent industry confirmation of the RPM and milling-feed relationships; product-specific recommendation tables are not reproduced.
- Sandvik Coromant — Milling Formulas and DefinitionsIndustry reference for milling terminology and the relationship among cutting speed, diameter, spindle speed, feed per tooth, and table feed.
Dataset and Source-Check Details
- Publisher
- Turn2Engineering
- Source checked
- August 19, 2026
- Dataset label
- UF DML limited transformed subset; 8 common material rows
- Source-controlled fields
- HSS SFM and end-mill chip-load ranges
- Calculated fields
- Metric equivalents, 2.5× carbide starting speed, RPM, feed rate, effective cutting speed
- Rights status
- Open-reuse license not verified; bulk reproduction/download disabled
- Bulk CSV
- Disabled
- Primary limitation
- Generic educational starting values do not replace cutter-manufacturer application data
Feeds and Speeds FAQs
Spindle speed is rotational RPM; feed rate is linear tool/workpiece advance and, in milling, depends on RPM, flute count, and chip load per tooth.
For inch diameter, use RPM = 12 × SFM ÷ (π × D); for metric diameter, use RPM = 1000 × Vc ÷ (π × D) with Vc in m/min and D in millimeters.
Multiply the operating spindle RPM by the number of cutting teeth/flutes and the selected chip load per tooth.
No. Tool material and geometry change usable cutting parameters; the carbide speed on this page is specifically the UF source’s 2.5× HSS starting rule, not universal carbide-tool data.
Manufacturer data can account for a specific carbide grade, coating, cutting-edge geometry, diameter, engagement, and intended operation, so it should override a generic starting chart when available.
Use the Chart as a Controlled Starting Point
Start with a source-supported SFM and chip-load range, calculate RPM from the actual cutter diameter, and calculate feed from the operating RPM, flute count, and chip load. If the machine cannot reach the calculated RPM, reduce RPM to the machine limit and recalculate feed so chip load stays consistent. Then validate the starting point against the actual cutter manufacturer and the real machining setup.