Whether you're cutting soft aluminum or hardened tool steel, having the right numbers before you press start saves tools, time, and scrap. The chart gives you the complete GP series end mill speeds and feeds reference, straight from the CGS Tool data sheet, with guidance on how to read it and apply it correctly.
How to Use This Chart
The GP series end mill speeds and feeds chart lists two things for each material: surface speed in feet per minute (SFM) and feed per tooth in inches (IPT). You use those two values together to calculate your actual spindle RPM and table feed rate for any given end mill diameter.
Here's the quick workflow:
- Find your material in the chart below.
- Pick the SFM value, use the higher end for light cuts, the lower end for heavier engagement.
- Read the feed per tooth column that matches your end mill diameter (≤¼", ≤½", or ≤1").
- Calculate RPM and then feed rate using your number of flutes.
RPM formula: RPM = (SFM × 3.82) ÷ End Mill Diameter (inches)
Feed rate formula: Feed Rate (IPM) = RPM × Feed Per Tooth × Number of Flutes
These values are starting points, not hard limits. Fine-tuning based on your machine rigidity, coolant type, and tooling condition is always required before pushing to full production rates.
Recommended Surface Speeds (SFM) by Material
The carbide end mill speeds and feeds chart below covers 25 material families. The SFM column tells you how fast the cutting edge should move according to the material. Hard materials can tolerate much higher surface speeds and heat-sensitive materials need slower speeds to prevent edge failure.
higher surface speeds and heat-sensitive materials need slower speeds to prevent edge failure.
|
Material |
SFM Range |
Feed/Tooth ≤¼" |
Feed/Tooth ≤½" |
Feed/Tooth ≤1" |
|---|---|---|---|---|
|
Aluminum / Alloys |
600–1300 |
.0002–.002 |
.002–.004 |
.004–.008 |
|
Magnesium / Alloys |
800–1400 |
.0005–.002 |
.002–.004 |
.004–.010 |
|
Plastics |
600–1200 |
.0006–.003 |
.003–.006 |
.006–.015 |
|
Plastics – Glass Filled |
300–800 |
.0006–.003 |
.003–.004 |
.004–.012 |
|
Brass / Soft Bronze |
400–700 |
.0005–.002 |
.002–.003 |
.003–.005 |
|
Bronze / High Tensile |
250–400 |
.001–.002 |
.002–.003 |
.004–.006 |
|
Copper / Alloys |
350–900 |
.0005–.002 |
.002 |
.002–.006 |
|
Iron – Cast (Soft) |
200–500 |
.0005–.002 |
.002–.003 |
.003–.008 |
|
Iron – Cast (Hard) |
100–450 |
.0003–.001 |
.0008–.002 |
.003–.005 |
|
Iron – Ductile |
80–400 |
.0002–.001 |
.001–.002 |
.002–.006 |
|
Iron – Malleable |
250–600 |
.001–.002 |
.001–.003 |
.003–.008 |
|
Steel – Low Carbon |
250–550 |
.0002–.001 |
.001–.003 |
.003–.007 |
|
Steel – Medium Carbon |
100–250 |
.0004–.0015 |
.0015–.002 |
.002–.005 |
|
Steel – Up to Rc35 |
150–250 |
.0005–.001 |
.001–.002 |
.002–.003 |
|
Steel – Rc35 to Rc50 |
80–150 |
.0002–.0007 |
.0007–.001 |
.002–.003 |
|
Steel – Rc50 to Rc60 |
25–120 |
.0002–.0005 |
.0005–.001 |
.002–.003 |
|
Steel – Mold |
200–350 |
.0002–.001 |
.001–.002 |
.002–.006 |
|
Steel – Tool |
100–300 |
.0002–.001 |
.001–.002 |
.002–.006 |
|
Stainless Steel – Soft |
250–400 |
.0002–.001 |
.001–.002 |
.002–.006 |
|
Stainless Steel – Hard |
50–250 |
.0002–.001 |
.001–.002 |
.001–.005 |
|
Monel / High Nickel Steel |
150–300 |
.0002–.001 |
.001–.002 |
.002–.004 |
|
Nickel Base Hi-Temp Alloys |
20–100 |
.0003–.0008 |
.0008–.001 |
.001–.002 |
|
Titanium – Soft |
120–350 |
.0002–.001 |
.001–.002 |
.002–.006 |
|
Titanium – Hard |
30–150 |
.0002–.0005 |
.0005–.001 |
.001–.004 |
|
Refractory Alloys |
80–400 |
.0002–.001 |
.001 |
.001–.002 |
The SFM chart for end mills above intentionally uses ranges, as not every aluminum cut passes in the same way. Deeper axial cuts, tight pockets, or worn spindle bearings when used correctly all push productivity towards the higher number.
Feed Per Tooth (IPT) by End Mill Diameter
The feed per tooth end mill values in this chart scales with cutter diameter; a larger end mill can remove a thicker chip per flute without deflecting. For the greater results, three diameter bands are used:
- Up to ¼" (0.250"): These are small-sized chips that have the highest deflection risk, so you need to work carefully when starting work on the low-end work.
- Up to ½" (0.500"): this size range is commonly used.
- Up to 1" (1.000"): Larger end mills can handle the heaviest chip loads in the table.
For milling speeds for aluminum with a ¼" GP end mill, the feed per tooth range is .0002–.002 IPT. At ½", that jumps to .002–.004, and at 1", you can push .004–.008. This is why running the right diameter for your application matters just as much as picking the right SFM because an undersized cutter running heavy chip loads can deflect, chatter, and break early.
Note on flute count: These values apply to standard 2–4 flute GP end mills. If you're running a high-flute-count finisher, reduce chip load per tooth proportionally.
Special Notes: Slotting, Plunge, and Radial Depth
The end mill feed rate by material figures assumes a standard radial engagement. When the tool is cut, its condition changes significantly, and the numbers need to be updated accordingly.
- Plunge Cuts
Reduce feed per tooth by 50–65% for any plunge operation. The GP end mill is not a drill plunging at full chip load that breaks corner edges fast. - Slotting
Drop surface speed by approximately 20% below the lowest, which is the recommended SFM value. Full-width engagement traps chips and builds heat, which is why slower speed helps manage both. - Light Radial Depth (less than 0.5× diameter)
Use the higher end of the SFM range. Less engagement means less heat, so you can push speed. - Heavy Radial Depth (greater than 0.5× diameter)
Use the lower end of the SFM range. More engagement means more heat and faster wear if you run fast.
Axial depth limit: Do not exceed 1.5× the end mill diameter for axial depth. If you must go deeper, switch to conventional (up) milling and cut feed per tooth by 50%. Climb milling at deep axial cuts risks tool pull-out and breakage.
Download the Full GP Speeds & Feeds PDF
Get the original CGS Tool reference sheet as a printable PDF and keep it at the machine or where you need it.
FAQs
What materials does the GP series speeds and feeds chart cover?
The chart covers 25 material families, including aluminum, steel grades from low carbon to Rc60, stainless, titanium, Monel, nickel hi-temp alloys, cast iron, copper, brass, plastics, and refractory alloys.
How do I calculate RPM from SFM for my end mill?
Use RPM = (SFM × 3.82) ÷ diameter in inches. For example, aluminum at 800 SFM with a ½" end mill gives 6,112 RPM. Then multiply RPM × feed per tooth × flutes to get the table feed rate.
When should I reduce the feed rate for slotting operations?
In slotting, reduce surface speed by ~20% below the lowest recommended SFM for your material. Full-width engagement traps chips and builds heat faster than partial radial cuts.
What is the recommended feed per tooth for aluminum with a ¼" GP end mill?
The feed per tooth range for aluminum at ¼" diameter is .0002–.002 IPT. Start low if your setup has limited rigidity or you're running a longer reach.
Can I use these speed and feed values for titanium and Inconel?
Yes, titanium runs 30–350 SFM, and Inconel-type alloys run 20–100 SFM. Both are prone to work hardening, so always start at the bottom of the range with sharp tooling and a consistent chip load.