CNC Milling Training Lesson 5: Cutting Tools, Tool Holders, the Magazine and Cutting Parameters

📷 IMAGE AREA — Basic cutting tools in CNC milling: face mill, end mill, drill, reamer, tap and boring tool
Suggested alt text: CNC milling face mill end mill drill reamer tap and boring tools

In CNC milling, choosing the right cutting tool is as important as writing a correct program. Even with perfect coordinates, a wrong tool, an unsuitable holder, an over-extended cutter, a wrong speed or an unsuitable feed spoils the dimension/surface, breaks the tool or causes a crash. Since CNC mills run at high speeds and feeds, the cutting tool, the holder and the cutting parameters must be evaluated together.

1. Aim of the lesson

By the end of this lesson the student will be able to recognise the basic cutting tools; choose a tool by operation; understand the differences between end mill/face mill/drill/reamer/tap; explain the properties of tool materials; distinguish the tool holders and taper systems; understand the tool magazine and ATC logic; relate cutting speed, spindle speed and feed; and calculate speed/feed.

2. Why is the cutting tool important?

The cutter does not only cut; it must form the required dimension, provide surface quality, remove chips, withstand the cutting forces and keep its cutting ability at high temperature. A tool’s suitability cannot be judged by diameter alone; the tool type, diameter, number of flutes, cutter material, coating, helix angle, tip geometry, total length, extension, workpiece material, coolant and roughing/finishing must be evaluated together.

3. Choosing a tool by operation

Tool selection starts with “what operation will be done on the part?”: a wide flat surface → face mill; a narrow slot → end mill or slot mill; a hole → drill; finishing a precise hole → reamer; a thread → tap; a large-diameter precise hole → boring tool. Several tools can be used on the same part; this is exactly why the ATC and tool magazine matter.

4. Basic cutting tools

• Face mill: for wide/flat surfaces; usually with indexable carbide inserts. A large diameter machines a wide area in one pass but needs high torque, rigid clamping and a balanced tool. At large diameter, the rpm needed for the same cutting speed decreases.
• End mill: the most used; slots, pockets, contours, steps, chamfer/radius. Can be two/three/four or more flutes; more flutes mean more cutting edges but smaller chip flutes.
• Two-flute end mill: wide chip space; helps chip evacuation in long-chip materials like aluminium and in slotting. Four-flute: more rigid for steel, side and contour work; more limited chip space in a full slot. (“Two flutes in aluminium, four in steel” should not be memorised; modern geometry/coating and builder advice may require different choices.)
• Ball nose: mould surfaces, 3D surfaces, curved geometry, finishing. Its centre has a very low real cutting speed; continuous cutting from the exact centre spoils surface and life.
• Corner-radius: a small tip radius instead of a sharp corner; increases corner strength and surface quality. Roughing (rippled) end mill: chip-splitting geometry; high stock, lower force; a finishing tool follows.
• Chamfer mill: chamfers, countersinks, deburring (45/60/90°). The programmer must know the real tip geometry and reference diameter, or the chamfer width comes out wrong. T-slot / disc-slot mills: T-shaped or narrow/deep slots; runout and rigidity are critical, not plunged directly into solid material.

5. Hole-making tools

• Centre drill/spot drill: reduces drill wander, improves hole position accuracy; must be short/rigid.
• Drill: a cylindrical hole. Diameter, depth, material, blind/through, coolant and chip evacuation are considered; deep holes use peck-drilling cycles. Indexable drill: high feed/fast drilling; precise holes may need extra finishing.
• Reamer: brings a pre-drilled hole to a precise size/surface; does not drill from scratch, needs a pre-hole. The pre-hole diameter must not be too small/large.
• Countersink: conical/cylindrical countersink, screw-head seat, deburring. Boring tool: brings an existing hole to a precise diameter/position; balance and setup are critical at high rpm.
• Tap: internal thread in a hole. The hole diameter must be correct, spindle-Z feed synchronised, pitch correct and coolant/lubrication suitable; tap breakage is a frequent, serious problem.

6. Cutting tool materials

The cutter must be harder than the part and keep its hardness under temperature. HSS (high-speed steel): tough, impact-resistant, easy to grind; drills, taps, reamers, some end mills; low/medium speed. Carbide: very common; high hardness/cutting speed, hot hardness, good wear resistance; but more brittle, sensitive to impact/vibration. Coated carbide: higher wear resistance and life, less friction/chip adhesion (do not choose by coating colour). Ceramic/CBN/PCD: special uses — ceramic for cast iron/hard materials, CBN for hardened steel, PCD for aluminium/copper/composite (not always suitable for ferrous materials).

7. Indexable cutting inserts

Face mills and some bodies use indexable inserts: the whole tool need not be changed, a worn insert is rotated/renewed, and different grades are used for different materials. When fitting an insert, the seat must be clean, no chip underneath, the screw/clamps sound, the insert in the right orientation and tightened to the right torque. Even a small chip under the insert causes runout, a surface mark, load on one insert and insert breakage.

8. Tool holder and taper systems

The system that fixes the cutter to the spindle and carries it safely is the tool holder; it holds the cutter centred, transmits rotation, withstands cutting forces, reduces runout and provides an ATC-compatible connection. The top of the holder fits the spindle’s tapered bore; common standards are BT, CAT, SK, HSK — they look similar but are not interchangeable. Selection must match the spindle standard, taper size, pull-stud type, ATC, permitted rpm and balance class. A wrong holder is never forced into the spindle. Pull stud: the part the spindle’s drawbar grips; it must be suitable for the machine, sound and fitted as the builder recommends.

9. Types of holder

• Collet holder: for cylindrical-shank tools (end mill, drill, countersink, small reamer). The collet must suit the shank diameter, not be forced into an oversize collet, and the collet/holder taper must be clean (chips/dirt cause runout). The nut is tightened with the proper wrench; no hammering, pipe extension or excessive force.
• Weldon (side-lock): a side screw presses on the flat of the shank; high torque, resistance to axial slip, solid clamping in roughing; runout accuracy may not be as good as collet/precision holders.
• Hydraulic holder: low runout, good vibration damping, easy tool change, high precision in finishing. Shrink-fit: heated to expand, the tool is inserted, and grips firmly on cooling; high runout accuracy/rpm suitability. Needs a heating device; touching a heated holder by hand risks serious burns.
• Morse sleeve: for Morse-taper drills/reamers; the surfaces must be clean/undamaged. Arbor: an adapter fixing bored/special-connection cutters (disc, slot, some face heads) to the spindle; the key, drive face and clamp screw must be placed correctly.

10. Tool extension and runout

Extension: the tool should be extended from the holder only as much as needed; the shortest safe extension is preferred. An over-extended tool loses rigidity, increases deflection/vibration, spoils the surface and can break; too short and the holder can hit the part or a deep pocket cannot be reached. Runout: the cutting edge deviating from the true axis of rotation; the flutes do not carry equal load, life falls, the hole can grow and the surface is spoiled. Causes: dirty collet, damaged holder, bent shank, wrong tightening, dirt in the spindle taper. Checked with a dial indicator.

11. Tool magazine and ATC

The section where different tools are kept ready is the tool magazine (disc, umbrella, chain, drum; 16–40+ capacity). Fixed pocket: each tool is tied to a specific pocket (T01→pocket 1). Random pocket: to reduce change time, the tool is left in an empty pocket and the control tracks it; the tool number and physical pocket may not always be the same — the operator must know the tool-management screen and the builder procedure.

12. Tool number, change and safety

In the program the tool is called with T and changed with M06 (T01 M06;); on some systems T01; and a separate M06;. The exact use must be verified from the builder manual. Tool-change safety: the spindle must be stopped, the axes at the safe change position, the part/fixture clear of the area and the magazine cover closed. ATC moves are very fast; do not touch the tool arm, put a hand in the magazine, try to catch a falling tool or disable the door lock.

13. Organising the T, H and D numbers

A tidy plan can use T01→H01→D01, T02→H02→D02 (T tool number, H tool length compensation, D radius compensation). They need not be identical on every system but this reduces confusion. Example tool list:

14. What is cutting speed?

Cutting speed (Vc) is the linear distance a point on the cutter’s circumference travels relative to the workpiece per minute; its unit is m/min. Cutting speed and spindle rpm are not the same: cutting speed is the linear speed at the cutter’s circumference, rpm is the number of revolutions per minute. When the tool diameter changes, the rpm for the same cutting speed changes too.

15. Factors affecting cutting speed

When choosing the cutting speed, the material and its hardness, tool material/coating, roughing/finishing, depth of cut, machine power, clamping rigidity, extension, coolant and builder advice are considered. Vc should first be taken from the tool builder’s catalogue (by material and cutter).

16. Spindle speed calculation

n = (1000 × Vc) / (π × D)

n  = spindle speed (rpm)
Vc = cutting speed (m/min)
D  = tool diameter (mm)
π  ≈ 3.14

Example: D = 20 mm, Vc = 100 m/min → n = (1000 × 100) / (3.14 × 20) = 100000 / 62.8 ≈ 1592 rpm. The machine value is rounded suitably: S1590 or S1600. At the same cutting speed, as the tool diameter decreases the rpm increases and as it increases the rpm decreases; rpm should not be memorised by material alone.

17. Feed per tooth and table feed calculation

Milling tools are multi-flute; the amount each cutting tooth advances per pass is the feed per tooth (fz, mm/tooth), taken from the catalogue. With G94, F is usually in mm/min:

Vf = fz × z × n

Vf = table feed rate (mm/min)
fz = feed per tooth (mm/tooth)
z  = number of flutes
n  = spindle speed (rpm)

Example 1: fz = 0.05, z = 4, n = 1600 → Vf = 0.05 × 4 × 1600 = 320 mm/min → F320.. Example 2: 25 mm diameter, 6 inserts, fz 0.1, n 1500 → Vf = 0.1 × 6 × 1500 = 900 mm/min → F900..

18. Plunge feed vs horizontal feed

They are not always the same. When an end mill plunges into the part in Z, its centre geometry, chip evacuation and axial cutting ability differ from horizontal cutting; so the plunge feed is usually lower (e.g. G01 Z-3. F100.; plunge, G01 X80. F320.; horizontal). The exact ratio is set by the builder recommendation.

19. Depth of cut, stepover and roughing/finishing

Speed and feed are not enough; two more values exist: axial depth of cut (ap) the depth along the tool axis, and radial width of cut (ae) how much of the tool diameter is in the material. A Ø10 tool is under high radial load in a 10 mm full slot but under low load in a 1 mm-stepover finish; the same speed/feed does not give the same result. Roughing: fast stock removal, leaving finish allowance, high ap, a strong tool. Finishing: small allowance, controlled feed, low runout, a sharp tool.

20. Cutting direction: climb and conventional milling

Climb milling: the motion at the contact point is the same as the feed direction; on CNC it is often preferred thanks to ball screws and low backlash (good surface, favourable chip formation, longer life in some cases). Conventional milling: the cutter motion and feed are opposite; used in some clamping/surface conditions. The choice considers the tool, material, clamping, machine backlash and surface skin.

21. Coolant, chips and vibration (chatter)

Coolant cools the cutting zone, reduces friction, removes chips and increases life; but heavy coolant is not right for every operation (dry, air, MQL or through-coolant may be preferred). Especially with carbide, irregular coolant can crack the tip via sudden thermal change. Chip shape shows the process state: healthy chips move away and are of reasonable size/shape; very long stringy, sticking, burnt or powdery chips indicate wrong feed/speed, poor evacuation or a dull tool. Chatter (regular vibration/marks): over-long tool, weak clamping, unsuitable speed/feed, high ap, a worn tool or large radial engagement; do not change one parameter randomly — check in order.

22. Signs of wrong speed and feed

• Speed too high: fast wear, tip heating, chip adhesion, surface burning. Too low: low efficiency, hammering, poor surface.
• Feed too high: tool breakage, vibration, poor surface, increased spindle load, part slipping. Too low: rubbing instead of cutting, heat rise, surface smearing, early wear, long time.
• Tool wear: dimension change, surface degradation, spindle-load/sound change, burr increase. It must not be hidden by constantly changing the program value; the tool’s real condition must be checked first.

23. Tool presetting

The length, diameter, radius and tip position of tools can be measured before machining and taught to the control. Two methods: on-machine measurement (tool probe/contact sensor/reference surface) and an external presetter (the tool is prepared while the machine runs, length/diameter recorded neatly, setup time reduced). Entering tool lengths into the H offsets is covered in the next lesson.

24. Tool list and a program tool section example

(T2 D12 CARBIDE END MILL)
T02 M06;
G17 G21 G40 G49 G80 G90 G94;
G54;
S2500 M03;
G00 X20. Y20.;
G43 H02 Z50.;
M08;
G00 Z5.;
G01 Z-3. F120.;   (Z plunge)
G01 X80. F700.;   (horizontal cut)
G00 Z50.;
M09;
M05;
G49;

25. The order for selecting a tool

Determine the geometry → decide roughing/finishing → determine the material → choose the tool type, diameter and number of flutes → the cutter material/coating → a suitable holder → the needed extension → check the holder does not hit the part/fixture → take Vc and fz from the catalogue → calculate speed/feed → check the machine max speed/power/torque limit → create the program and tool list → machine the first part at a low override.

26. Tool clamping and magazine checklist

Clamping: is the cutter/diameter correct, does the shank suit the collet, are the collet/holder clean, is the extension unnecessarily long, are there breaks on the edges, are the insert screws tight, is the taper clean, are the pull stud and T/H/D numbers correct, does the total length suit the magazine limit, are the balance/rpm limit suitable? Magazine placement: large-diameter tools can approach neighbouring pockets — leave side pockets empty or define a “large tool”; long tools can hit the cabin/body/part; for heavy tools check the permitted maximum weight.

27. Common tool and parameter mistakes

• Confusing the tool number with the H number (e.g. T03 M06; G43 H02 Z50;): a wrong H takes the tool to an unexpected Z.
• Over-extending the tool: vibration, dimensional error, breakage.
• Mistaking cutting speed for rpm: writing Vc = 150 m/min directly as S150 is wrong; the rpm is calculated from the diameter first.
• Setting the feed by rpm alone: the number of flutes and fz must be considered. Using drill feed like end-mill feed: each tool type has a different geometry.
• Not cleaning the chip under the insert (runout) and forcing the whole collet range.
• Exceeding the machine max speed and starting the first part at full feed: the first run must be watched at a low override (sound, chips, load, surface).

28. Applied calculation and the first part

Ø12, four-flute carbide end mill; from the catalogue Vc = 120 m/min, fz = 0.04, z = 4. Speed: n = (1000 × 120) / (3.14 × 12) = 120000 / 37.68 ≈ 3185 → S3200. Feed: Vf = 0.04 × 4 × 3200 = 512 → F510. (or F500.). This is a starting value; the full slot/side cut, ap/ae, extension, rigidity and coolant must be evaluated. On the first part, watch the spindle load, cutting sound, vibration, chip colour/shape, surface and dimension; parameter changes must not be random and must be recorded.

29. Lesson summary

• The cutter is chosen by operation, material and geometry; the face mill, end mill, drill, reamer, boring tool and tap have different roles.
• HSS is tough/medium speed, carbide hard/high speed; a coating increases life. The holder clamps the cutter centred; the extension must be short, the runout low.
• Cutting speed and rpm are not the same; rpm is n = 1000·Vc / (π·D), feed is Vf = fz·z·n.
• A very low/high feed can damage the tool; the catalogue and machine limits are evaluated together and the first part machined in a controlled way.