End Mill Selection for Metal Cutting — Raptorex Knowledge Base

1. Quick Summary

Three rules you can apply without reading the full article:

Aluminum and non-ferrous metals: a 2-flute, uncoated / bright polished carbide bit. Chip evacuation is generous and metal does not stick to the bit.
Steel and hard materials: a 4-flute, TiAlN/AlTiN coated carbide bit — with step-down passes (see the machine table).
Do not choose a smaller bit over a larger one: Always pick the largest diameter the job allows; a thin bit deflects, vibrates and breaks.

Safety Metal chips are sharp and hot; wear protective goggles, always clamp the workpiece to the table and never work with gloves.

2. Know Your Machine First

Three machine values guide your bit selection: spindle power (how much chip it can remove), maximum spindle speed (the ceiling of your cutting speed) and collet system (which shank diameters it can grip). These values across the Raptorex series are:

Raptorex series — values critical for metal cutting
Machine	Spindle	Max spindle speed	Collet chuck	Practical bit diameter	Metal capability
Mini V2	180 W	≈ 12,000 RPM	ER16	Ø3.175 – 6 mm	Aluminum + non-ferrous — clean, precise results with step-down passes
Mini V3	500 W	≈ 12,000 RPM	ER16	Ø3.175 – 6 mm	Aluminum + brass/bronze
Pro	1.4 kW	18,000 RPM	ER20	Ø4 – 10 mm	Aluminum with ease + mild steel (step-down passes)
Pro V2	2.3 kW	18,000 RPM	ER20	Ø4 – 10 mm	Aluminum + steel (comfortable material removal)

Collet system and shank diameter

Mini series (ER16): grips shanks from ≈ 1–10 mm; collets are available for standard 3.175 mm (1/8") bits.
Pro series (ER20): grips shanks from ≈ 1–13 mm; end mills with 6 and 8 mm shanks are used comfortably.
It is the bit's shank diameter, not its cutting diameter, that must fit the collet. E.g., a bit with a Ø10 cutting diameter but an 8 mm shank fits an ER20.

Why it matters? Every bit performs well only when it fits your machine's power budget. For example, a Ø10 end mill for steel is too large for a 180 W spindle: the motor cannot sustain the cutting force, the spindle stalls, and the bit rubs and burns. Scaling the bit diameter and stepdown to your machine's power is the first rule of efficient cutting.

3. Tool Material: HSS or Carbide?

End mills come in two main body materials:

HSS vs carbide bits comparison
Property	HSS (High Speed Steel)	Carbide (Sintered Tungsten)
Hardness / wear	Softer, wears quickly	Very hard, long lasting
Heat resistance	Loses its edge at ≈ 600 °C	Stays sharp up to ≈ 1000 °C
Fragility	Flexible, impact resistant	Hard but brittle — breaks on impact
Price	Cheap	Expensive
Ideal use	Low spindle speed, low power, soft material, one-off jobs	High spindle speed, series production, hard material, long life

Carbide demands high spindle speed. A sharp edge cuts properly only at sufficient surface speed; if the spindle speed stays too low, it rubs, heats up and dulls. On machines with 12,000–18,000 RPM spindles, carbide bits are advantageous. HSS can be more forgiving at low spindle speeds and on low-power machines (especially the Mini V2) — but in aluminum its edge dulls quickly.

Recommendation General rule for this series: use bright/polished carbide for aluminum and brass, and coated carbide for mild steel. Keep HSS as a backup/deburring bit. In particular, never push HSS in aluminum — the cutting edge sticks to the chip and can break the bit.

4. Flute (Channel) Count

The number of cutting flutes on the side of the end mill is the most critical decision of the selection. Flute count determines two things: chip evacuation area (fewer flutes = larger gullets = easier evacuation) and number of cutting edges (more flutes = more edges = better surface finish and higher feed rates).

Selection logic by flute count
Flutes	Advantage	Disadvantage	Best use
1 flute	Maximum chip clearance, lowest cutting force	Single edge wears fast, lower surface quality	Deep slots in aluminum/plastic; low-power machines
2 flutes	Wide chip gullets + balanced cutting	Feed capacity stays limited in steel	Aluminum and non-ferrous metals (the most common choice)
3 flutes	Very good evacuation + surface balance	—	High feed rate in aluminum, general purpose
4 flutes	High feed capacity, good finish, rigid	Narrow gullet → chips clog in aluminum (BUE)	Steel, stainless, hard materials
5–6 flutes	Best surface quality, high feed rate	Very narrow gullets, low chip clearance	Finishing passes, hardened steel (rarely on these machines)

The most common mistake Using a 4-flute "steel" bit in aluminum. Aluminum chips fill the gullets, the chips get re-cut, heat rises and the bit either clogs or aluminum welds to the bit (BUE). Choose bits with wide gullet openings (1–2–3 flute) for aluminum.

Single-flute bits are especially advantageous on low-power spindles like the Mini V2 (180 W): a single cutting edge means the least friction and the least motor load. A 1/8" (3.175 mm) single-flute carbide bit is the best-known starting point for aluminum on the Mini series.

5. Coating and Helix Angle

Coating

Coatings protect the bit from heat and wear; however, they can hurt when mismatched with the material. A short guide:

Coating-to-material matching
Coating	Appearance	Best material
Uncoated / bright polished	Bright gray	Aluminum and non-ferrous — so aluminum does not stick
TiN	Golden yellow	General-purpose steel
TiCN	Gray-blue	Stainless steel, cast iron
TiAlN / AlTiN	Dark gray-purple	Steel, alloy steel — withstands high temperatures

Pro tip Bits sold as "TiAlN coated, fits everything" give poor results in aluminum; the coating roughness makes aluminum stick to the bit. Look for special "bright/uncoated or DLC/ZrN" bits for aluminum.

Helix angle

High helix (40–50°): Smoother cutting, excellent chip evacuation → aluminum, plastic, thin-walled work.
Medium helix (30–38°): General-purpose balance.
Low helix (10–20°): High edge strength → steel, hard materials, less "pushing" on thin walls.
Variable helix: Breaks vibration (chatter) → a lifesaver on long reach and small diameters.

When buying, the catalog must state the "cutting length" and "helix angle". Avoid "generic" bits that list no technical values; without them you have no starting data for the speed/feed calculation.

6. Diameter and Length Selection

Diameter = not the smallest inner radius / narrowest pocket the job requires, but the largest diameter rigidity allows. E.g., for a 10 mm pocket the bit that fits is Ø6, not Ø4.
A thin bit deflects under cutting force → dimensional error, vibration and breakage. The smaller the bit diameter, the geometrically smaller the stepdown it can carry.
Reach/diameter ratio: When the bit's stick-out length from the holder exceeds ~4× its diameter, vibration risk rises sharply. If 3D surface work forces you beyond this ratio, reduce the stepdown significantly.
Corner form: Sharp-corner (square) bits break at the corner. Slightly radiused (corner radius) bits are far more durable and leave no marks on the surface — prefer radiused bits in metal whenever possible.
Short cutting length: Do not buy a bit with a longer cutting length than the job depth; rigidity drops as length grows.

A practical rule for desktop CNCs In metal, scale the stepdowns with the bit diameter: the axial depth of cut (Ap) is ~10–30% of the diameter in roughing, and the radial stepover (Ae) is ~20–40% of the diameter (e.g., Ø6 bit → Ap ≈ 0.6–1.8 mm, Ae ≈ 1.2–2.4 mm). In finishing passes both shrink; in a full slot, Ae equals the bit diameter and the feed rate is reduced. The examples below and the Section 7 tables are built on this logic. (In wood/plastic these ratios are much higher — this guide is for metal.)

7. Starting Values by Machine and Material

The tables below give starting values of spindle speed (S), feed rate (F), axial stepdown and radial stepover for each Raptorex model and the materials it can machine. The F value is the table feed entered directly into the CAM program (mm/min); the stepdown and stepover values are the stepdown / stepover settings in CAM. You can push the values up by listening to the chips and the sound. (Note: the maximum feed rate on all Raptorex models is 2,500 mm/min — the upper values in the tables respect this limit.)

Axial stepdown or radial stepover? Axial stepdown (Ap) is the Z (vertical) depth: how deep the bit sinks into the material per pass. If the total depth is 6 mm and the axial stepdown is 1 mm, the job finishes in 6 passes. Radial stepover (Ae) is horizontal: how far the bit shifts sideways per parallel pass (overlap depends on it; the ratio of stepover to bit diameter is the radial engagement). For roughing both are large; for finishing both are small. Axial stepdown is driven mainly by machine power, radial stepover by type of operation.

What is fz, and why does it look so small? fz (feed per tooth) is the chip thickness a single flute removes in a single revolution; that is why it looks as small as 0.02–0.08 mm. The feed entered into the machine is fz × spindle speed × number of flutes. Example: fz 0.04 × 12,000 RPM × 2 flutes = 960 mm/min. So a small-looking fz actually corresponds to roughly one meter of feed per minute. In this section we give spindle speed + feed directly so you don't have to calculate fz yourself (details of the calculation are in Section 8).

Assumption: The values below are for peripheral milling and pocketing (part outer contour / pocket clearing). If the bit cuts a full slot — i.e., a channel as wide as the bit diameter is opened in a single pass — the radial stepover already equals the bit diameter (100% radial engagement); in that case, drop the feed to about half the table value.

Mini V2 (180 W · ~12,000 RPM · ER16) — starting values
Material / operation	Recommended bit	Spindle (RPM)	Feed (F)	Axial stepdown	Radial stepover
Aluminum — roughing	Ø3.175 mm · 1–2 flute · polished carbide	12,000	1,000–1,500 mm/min	0.2–0.5 mm (0.25 ideal)	0.4–1.0 mm
Brass / bronze — roughing	Ø3.175 mm · 2-flute · polished carbide	12,000	800–1,200 mm/min	0.2–0.5 mm	0.4–0.9 mm

Mini V3 (500 W · ~12,000 RPM · ER16) — starting values
Material / operation	Recommended bit	Spindle (RPM)	Feed (F)	Axial stepdown	Radial stepover
Aluminum — roughing	Ø3.175–4 mm · 2-flute · polished carbide	12,000	1,200–2,000 mm/min	0.5–1.0 mm	0.6–1.4 mm
Brass / bronze — roughing	Ø4 mm · 2-flute · polished carbide	12,000	900–1,400 mm/min	0.4–0.8 mm	0.5–1.0 mm

Pro (1.4 kW · 18,000 RPM · ER20) — starting values
Material / operation	Recommended bit	Spindle (RPM)	Feed (F)	Axial stepdown	Radial stepover
Aluminum — roughing	Ø6 mm · 3-flute · polished carbide	14,000–18,000	1,500–2,200 mm/min	0.8–2.0 mm	1.2–2.4 mm
Aluminum — finishing	Ø6 mm · 3-flute · polished carbide	16,000–18,000	800–1,200 mm/min	0.1–0.3 mm	0.2–0.5 mm
Mild steel (St37, C45)	Ø6 mm · 4-flute · TiAlN carbide	5,000–5,500	450–650 mm/min	0.2–0.5 mm	0.3–0.7 mm

Pro V2 (2.3 kW · 18,000 RPM · ER20) — starting values
Material / operation	Recommended bit	Spindle (RPM)	Feed (F)	Axial stepdown	Radial stepover
Aluminum — roughing	Ø6–8 mm · 3-flute · polished carbide	14,000–18,000	1,800–2,500 mm/min	1.0–2.5 mm	1.5–3.0 mm
Aluminum — finishing	Ø6–8 mm · 3-flute · polished carbide	16,000–18,000	1,000–1,500 mm/min	0.1–0.3 mm	0.3–0.6 mm
Mild steel (St37, C45)	Ø6–8 mm · 4-flute · TiAlN carbide	5,500–6,500	600–900 mm/min	0.3–0.8 mm	0.5–1.2 mm
Stainless 304 — advanced	Ø6 mm · 4-flute · special geometry	4,000–5,000	250–400 mm/min	0.2–0.4 mm	0.3–0.6 mm

Note: Steel appears only under Pro / Pro V2 in the tables — steel machining is done with these models' powerful spindles. A multi-pass (step-down) strategy instead of one deep pass both improves surface quality and extends bit life. The second factor that decides the result in steel is cooling: cut quality, tolerances and bit life depend directly on cooling — see Section 9.

8. Spindle Speed and Feed Rate Calculation

You calculate two numbers for the bit you have chosen: spindle speed (n) and table feed rate (Vf). The formulas in metric units are:

n (RPM) = (Vc × 1000) / (π × D)
Vf (mm/min) = fz × n × number of flutes

Vc: cutting speed (m/min) — taken from the bit manufacturer's catalog table according to material and bit material (the values in Section 7 are based on these tables)
D: bit diameter (mm)
fz: feed per tooth (mm/tooth) — the "chip load" value recommended by the bit manufacturer; in the examples below, fz is chosen first and the feed is then calculated with this formula
Number of flutes: the number of cutting flutes on the bit

Example 1 — Mini V3: Aluminum, Ø3.175 mm 2-flute carbide

Spindle speed

Thin bits like Ø3.175 mm need high spindle speeds: for Vc = 200 m/min you need n = (200 × 1000) / (3.14 × 3.175) ≈ 20,000 RPM. Since the machine ceiling is ~12,000, use n = 12,000 (actual Vc ≈ 120 m/min — on thin bits the spindle ceiling naturally becomes the limiting factor).

Feed rate

fz = 0.04 mm/tooth → Vf = 0.04 × 12,000 × 2 = 960 mm/min. Practical starting point: 600–800 mm/min, increased according to the chips.

S12000 F700 · axial stepdown 0.4–0.6 mm · radial stepover 0.6–1.3 mm

The Mini V2 (180 W) cuts the same job with a 1–2 flute bit, 0.25 mm step-down passes and ~1,000–1,500 mm/min feed (see the Mini V2 table in Section 7) — same quality, longer time.

Example 2 — Pro: Aluminum, Ø6 mm 3-flute carbide

Spindle speed

Vc = 300 m/min → n = (300 × 1000) / (3.14 × 6) ≈ 15,900 RPM → use n = 16,000; you can go up to the 18,000 RPM ceiling.

Feed rate

fz = 0.05 mm/tooth → Vf = 0.05 × 16,000 × 3 = 2,400 mm/min. Practical starting point: 1,800–2,200 mm/min, axial stepdown 0.5–1 mm, radial stepover 1.5–2.5 mm.

S16000 F2000 · radial stepover ~30% (1.8–2 mm) — roughing

Example 3 — Pro V2: Mild steel, Ø6 mm 4-flute TiAlN

Spindle speed

Vc = 100 m/min → n = (100 × 1000) / (3.14 × 6) ≈ 5,300 RPM → n = 5,500.

Feed rate

fz = 0.03 mm/tooth → Vf = 0.03 × 5,500 × 4 ≈ 660 mm/min. Practical starting point: 500–700 mm/min.

S5500 F600 · axial stepdown 0.3–0.5 mm · radial stepover 0.5–1 mm · spray lubrication recommended

Listen to the chips The calculated value is a starting point. In healthy cutting you hear a steady, solid sound and the chips come out curled/shiny. A high-pitched "whistle" = rubbing (increase feed or lower the spindle speed); rattling/vibration = chatter (lower the spindle speed, then reduce the stepdown). Do not make changes larger than 10–15% at once.

9. Why Is Cooling Critical When Cutting Steel (Carbon Steel)?

In aluminum, cooling/lubrication makes the job easier; in carbon steel it decides the result. When machining steel on the Pro and Pro V2, the heat at the cutting edge directly governs surface quality, part dimension (tolerance) and bit life. Because steel has low thermal conductivity, the heat released by the cutting energy does not dissipate into the workpiece — it accumulates at the cutting edge. Machining steel without controlling the heat produces bad results no matter how correct the bit selection is.

How does heat wear the bit?

Carbide starts losing hardness above ~800 °C; TiAlN/AlTiN coatings also work near that limit. If the heat is not removed, the edge softens, wears rapidly and dulls quickly.
The most important factors determining tool life are cutting speed and temperature; as temperature rises, wear accelerates almost exponentially. Proper cooling lowers the bit temperature and significantly extends bit life.
Cutting fluid also flushes chips away from the cutting zone. Re-cutting chips damages both the bit and the machined surface.

Cut quality and surface

Stable temperature = stable cutting: chip adhesion decreases, surface roughness (Ra) improves and the cutting sound stabilizes.
No burn / blue discoloration marks form on the workpiece; the cut surface stays clean and uniform.
The lubricating effect reduces friction; the cutting edge cuts instead of rubbing and smearing.

Tolerances and thermal expansion

Steel's coefficient of thermal expansion is ≈ 12 µm/m·°C. For example, a 100 mm long part that heats only 20 °C during machining grows about 0.02–0.03 mm; when the part cools later, the dimension changes again. In a job demanding ±0.05 mm tolerance, this difference approaches half the tolerance. Cooling keeps the part and tool at a steady temperature, providing dimensional repeatability: every part produced with the same program comes out the same size. In addition, a heated tool grows in length — this also shifts dimensions, especially in deep pockets and jobs requiring Z accuracy.

Which cooling method?

Cooling approach by material
Material	Adequate cooling	Why
Aluminum / non-ferrous	Spray oil, isopropyl alcohol, WD-40	Prevents sticking to the bit (BUE); since the heat load is low, spray is enough
Carbon steel (Pro / Pro V2)	Flood coolant (emulsion) or strong jetting	Continuously removes heat; cut quality, tolerance and bit life depend on it
Stainless — advanced	Chlorine-free cutting fluid + generous flow	Prevents work hardening and corrosion

Flood coolant is recommended for the Pro series If you seriously machine carbon steel (parts, molds, fixtures), spray is not enough; continuous-flow flood coolant protects both bit life and job quality. Raptorex's Automatic Liquid Cooling Module (Pro) and Pro V2 versions are ready for long steel jobs with a 50 Lt stainless tank, a 90 W pump and a chip separator system. If you mostly work aluminum, spray is sufficient — the module becomes indispensable mainly when machining steel. For which fluid to put in the tank and mixing ratios, see the Cutting (Coolant) Fluid Preparation Guide.

Do not interrupt the coolant If cold fluid suddenly hits a heated carbide bit, thermal shock can crack the bit. Turn on the coolant before the cut starts, keep it flowing throughout the cut, and do not shut it off before the spindle stops.

10. Your First Bit Set and Cooling

The starting bit set you need to try metal cutting as soon as you take the machine out of the box:

Starter set recommendation
Machine	Set contents (recommended)
Mini V2 / Mini V3	Ø3.175 mm (1/8") 1-flute polished carbide ×2 · Ø3.175 mm 2-flute polished carbide ×2 · ER16 3.175 mm collet
Pro	Ø6 mm 3-flute polished carbide ×2 · Ø6 mm 4-flute TiAlN (steel) ×1 · Ø3.175 mm 2-flute (detail work) ×2
Pro V2	Ø6–8 mm 3-flute polished carbide ×2 · Ø8 mm 4-flute TiAlN (steel) ×1 · Ø3.175 mm 2-flute (detail work) ×2

Which spindle speed/feed/stepdown for which material? → the machine tables in Section 7.

Cooling / lubrication In aluminum, avoid dry cutting: the risk of sticking to the bit (BUE) increases. Isopropyl alcohol / WD-40 / light spray oil are the most practical solution on desktop CNCs (do not pour water on the table or electronics). A liquid cooling module option is also available for the Pro series.

11. Common Mistakes and Troubleshooting

Symptom → cause → solution
Symptom	Likely cause	Solution
Dust-like chips	Feed per tooth too low; the bit is rubbing	Increase the feed (raise fz) or lower the spindle speed
Aluminum sticks to the bit	4-flute bit / coated bit / dry cutting	Switch to a 2-flute polished bit + spray lubrication
Vibration, high-pitched sound	Long reach, deep stepdown, mismatched spindle speed	In order: lower the spindle speed by 10% → reduce the stepdown → switch to a shorter bit
Motor stalls / skips steps	Stepdown exceeds the machine's power	Reduce the axial/radial stepdown; switch to a smaller diameter bit
Bit suddenly broke	Impact plunging, chip buildup, thin bit + deep stepdown	Use helical plunging/ramping; choose a chip-clearing toolpath
Rough surface	No finishing pass / dull bit / vibration	Drop the last pass to 0.1–0.2 mm and finish with a climb cut in the same direction

12. FAQ

Can aluminum be cut with the Mini V2? Yes — with a 1-flute polished carbide bit and 0.2–0.5 mm step-down passes, the Mini V2 produces clean, precise results in aluminum. Working in steps protects both surface quality and bit life.
Can steel be cut with the Pro? Yes. Mild steel (St37, C45) is machined on the Pro series with the right bit (4-flute TiAlN) and shallow step-down passes; the Pro V2's 2.3 kW spindle offers more comfortable material removal in steel. Hardened steel and stainless, however, are demanding jobs that need specialized bits and advanced parameter knowledge — start your first steel projects with mild steel.
Why is a 4-flute bit bad in aluminum? Because the chip gullets are narrow, aluminum chips fill the flutes; clogging and welding occur.
Should the spindle speed be high? Yes — if the cutting speed (Vc) is insufficient, carbide rubs. Use your machine's max spindle speed most efficiently by choosing a small-diameter bit.
When should I increase the feed? When the chips curl evenly and the sound is clean, increase by 10–15%. If a high-pitched sound appears, go back.
Are coated bits unusable in aluminum? TiN/TiAlN-type coatings cause sticking in aluminum; however, special DLC- or ZrN-coated bits for aluminum also exist — check that the catalog says "for aluminum".

References

References and further reading

Harvey Tool — General Machining Guidelines (Vc, chip load tables and formulas)
Sandvik Coromant — Milling formulas and definitions
MSC Industrial — End Mills Buying Guide (flute count and coating logic)
Penn Tool Co. — How to Choose the Right End Mill
Two Trees — Dialing In Chip Load for 6061 Aluminum (desktop CNC experiences)

Note: The values here are starting points for educational purposes. For exact parameters, follow the manufacturer catalog data of the bit you use.

1. Quick Summary

2. Know Your Machine First

Collet system and shank diameter

3. Tool Material: HSS or Carbide?

4. Flute (Channel) Count

5. Coating and Helix Angle

Coating

Helix angle

6. Diameter and Length Selection

7. Starting Values by Machine and Material

8. Spindle Speed and Feed Rate Calculation

Example 1 — Mini V3: Aluminum, Ø3.175 mm 2-flute carbide

Spindle speed

Feed rate

Example 2 — Pro: Aluminum, Ø6 mm 3-flute carbide

Spindle speed

Feed rate

Example 3 — Pro V2: Mild steel, Ø6 mm 4-flute TiAlN

Spindle speed

Feed rate

9. Why Is Cooling Critical When Cutting Steel (Carbon Steel)?

How does heat wear the bit?

Cut quality and surface

Tolerances and thermal expansion

Which cooling method?

10. Your First Bit Set and Cooling

11. Common Mistakes and Troubleshooting

12. FAQ

References

References and further reading

Looking for the right bit for your machine?