CNC Lathe Training Lesson 3: Cutting Tools, Tool Holders and Machining

In a CNC lathe program, knowing which coordinate the tool goes to is not enough on its own. Send two tools of different characteristics to the same coordinate and the result can change completely: one tool suits external turning while another only cuts grooves; one insert works well in steel while the same insert leaves a poor surface in aluminium; a tool suited to roughing may not deliver the size and finish expected in a precision finishing cut. So when learning CNC, it is wrong to separate programming from cutting-tool knowledge. The program defines the tool’s motion; but the element that actually removes material, carries the cutting force and forms the surface is the cutting tool.

On CNC machines, cutters are exposed to high cutting forces, impacts and very high temperatures; the temperature in the cutting zone can reach roughly 600–1300 °C. One of the factors that most affects machining quality and production time is the cutting tool and clamping system. The aim of this lesson is not to make the student a catalogue expert, but to reach the level where, looking at a part, they can understand which operations will be done and what kind of tool each operation needs.

xF0x9Fx93xB7 IMAGE AREA — Cutting insert + tool holder + cutting-tool system, labelled overview
Suggested alt text: “CNC lathe cutting insert, holder and cutting-tool system”

1. How Are Chips Formed on a Lathe?

In turning, the workpiece rotates about its own axis; the cutting tool contacts it at a set depth and feeds. The material in front of the cutting edge is compressed, its strength limit is exceeded, and it separates by curling over the cutting face; the separated material becomes a chip. Three important effects arise on the tip: cutting force, friction and heat. Cutting is not merely “the tool scratching the part”; the tool separates the material by plastically forcing it.

The cutting tip must therefore be hard enough, heat-resistant, tough against impact, of the correct geometry and firmly mounted. If not hard enough, the tip wears quickly; a tip that is too hard but brittle can crack in interrupted cutting. A tool’s success depends not only on its material but also on tip geometry, mounting, feed, cutting speed and depth of cut.

2. Cutting Tool vs. Insert vs. Tool Holder

In the shop the words “tool,” “bit,” “insert” and “holder” are sometimes used interchangeably, but technically their roles differ.

• Cutting insert: the part that directly contacts the workpiece and removes the chip. In indexable systems it can be square, triangular, rhombic, round or hexagonal. When the tip dulls, usually the whole tool is not replaced – only the insert is indexed or changed.
• Tool holder: the body that holds the insert at the correct angle, transmits cutting forces to the turret and clamps the insert firmly. External holders are usually square/rectangular; internal (boring) holders are cylindrical boring bars.
• Cutting tool: the system formed by insert plus holder (e.g. CNMG insert + external holder, grooving insert + grooving holder, threading insert + threading holder, boring insert + boring bar).

In tool selection, looking only at the insert is not enough. Even with the right insert, if the holder is the wrong hand, wrong approach angle, insufficient rigidity or wrong size, the machining result can be spoiled.

3. Why Is the Cutting Tool So Important?

A precise CNC machine does not guarantee a good part with a wrongly chosen tool. The cutting tool directly affects the part’s diameter/length, surface quality, tool life, machining time, chip form, vibration, cutting force, energy consumption, scrap amount and production cost. A good cutter can increase output while lowering tool cost.

When choosing a tool, ask not only “does this tool fit the part?” but also: what is the part material; is the operation roughing or finishing; external or internal; continuous or interrupted cutting; is the part rigid or thin-walled; how far will the tool overhang; what surface quality, cutting speed and feed are required; will coolant be used; do the chips need to break short.

xF0x9Fx93xB7 IMAGE AREA — Basic turning operations (facing, OD, ID, grooving, parting, threading) visual
Suggested alt text: “CNC lathe basic machining operations diagram”

4. Basic Machining Operations on a CNC Lathe

A part usually reaches its final form not in one operation but through a series of operations by different tools.

• Facing: flattens the front face; the tool feeds from the outside diameter toward the centre (X−). Used to create the Z zero and a clean start surface. If the centre height is wrong, a small pip can remain at the centre.
• External (OD) turning: removes material from the cylindrical surface; the tool approaches the cutting diameter in X and feeds along the length in Z. Used for straight cylinders, steps, shoulders, tapers and profiles, as roughing and finishing.
• Internal (ID) turning: enlarging/finishing an existing hole with a boring bar. Since the work area is hidden, more care is needed; the bar must be mounted as short as possible (a long bar vibrates).
• Taper turning: the tool moves in X and Z at the same time. A special tool may not be needed; an OD/ID tool with a suitable approach angle can be used, but the holder geometry must reach the taper.
• Profile turning: machining several shapes in sequence (flat, step, chamfer, taper, concave/convex radius). If insert shape and approach angle are unsuitable, the desired shape cannot physically be formed.
• Grooving: a narrow insert is plunged radially/axially (circlip, seal, oil, thread-relief, belt grooves, etc.). The insert width mostly sets the groove width; the tool must be mounted perpendicular to the axis and short.
• Parting off: separating the machined part from the bar; the cutter is narrow, long and sensitive to side forces. It must be exactly perpendicular to the axis, at centre height and with short overhang; the parted piece must be held safely.
• Drilling: the drill is mounted in the turret’s centre station; the part rotates and the drill feeds in Z. The tip must coincide with the spindle centre; if centre height is wrong, the drill cuts on one side, the hole comes out oversize or the drill breaks. A centre drill can be used first to prevent wandering.
• Threading: a special insert carrying the thread profile is used (metric, Whitworth, trapezoidal, pipe thread…). For a 60° metric thread a suitably profiled insert is chosen; threads are not cut with an ordinary OD tool.
• Chamfering: cuts the sharp corner at an angle; eases assembly and reduces edge chipping. 45° chamfers are easily machined with a suitable OD/profile tool.
• Radius machining: a rounded transition between two surfaces. Because the insert’s nose radius comes into play, precise profiles may need G41/G42 tool nose radius compensation; this is covered in the offsets lesson.

5. Roughing and Finishing Tools

The roughing tool removes excess material safely and fast; a strong cutting edge, resistance to large depth of cut, suitability for high feed, impact resistance, good chip breaking and rigid mounting are sought. Roughing inserts usually have a stronger geometry and a larger nose radius; but “the biggest insert is the best roughing insert” is not true – machine power, part rigidity and holder capacity also matter. The finishing tool brings the part to final size and surface quality; a smaller depth of cut, lower feed, sharp geometry, suitable nose radius and precise offset are used. A dull or coarse-geometry insert, in a small cut, can smear the part or leave a poor mark.

xF0x9Fx93xB7 IMAGE AREA — Insert geometry: insert shape, nose radius, clearance angle, chip breaker labelled
Suggested alt text: “Indexable cutting insert geometry and nose radius”

6. Cutting Tool Materials

For beginner level the two most important groups are HSS (high-speed steel) and carbide (cemented carbide) inserts; there are also advanced cutters such as ceramic, CBN and PCD.

• HSS: grindable, relatively tough, can be given special shapes; used in small drills, taps and special-profile tools. Advantages: easy grinding, toughness, low cost. Disadvantages: lower cutting speed than carbide, loses hardness faster at high temperature. It is no longer the main option for OD turning in modern CNC.
• Cemented carbide: very common on CNC lathes. Keeps hardness at high temperature, reaches high cutting speeds, is indexable and can be coated/uncoated. Coated carbide inserts are common in large-batch production. Disadvantage: more brittle than HSS, can break on impact or wrong mounting.
• Ceramic: works at very high speeds and temperatures (hardened material, cast iron, high-speed finishing); but is brittle and may be unsuitable for interrupted cutting.
• CBN (cubic boron nitride): for hardened steel, hard turning and precision finishing instead of grinding; expensive.
• PCD (polycrystalline diamond): for aluminium, copper, brass, composites and abrasive non-ferrous materials; unsuitable for steel due to high temperature and chemical interaction.

Coated and Uncoated Inserts

Carbide inserts can be coated to reduce friction, increase heat resistance, slow wear and allow higher cutting speeds. Uncoated, sharp-geometry inserts can give better results in some aluminium and non-ferrous applications. Do not decide the exact material/coating by the tool’s colour; check the manufacturer code and catalogue.

7. Basic Geometry of Indexable Inserts

An insert is not just its shape; its performance is set by insert shape and corner angle, clearance angle, tolerance, insert type, edge length, thickness, nose radius, cutting-edge form, cutting direction and chip-breaker geometry.

Insert Shape

Common shapes: round, square, triangular, 80° / 55° / 35° rhombic. Shape affects two things: the strength of the cutting edge and access to narrow areas. Wide corner-angle inserts (e.g. 80°) are strong in roughing and general OD but may not enter a narrow profile; narrow-angle inserts (e.g. 35°) give access in fine profiles and finishing but do not show the same strength in heavy roughing.

Positive and Negative Inserts

Positive insert: there is a clearance angle below the cutting edge; gives low cutting force, softer cutting and advantage in thin-walled parts, aluminium and finishing; but the edge section can be weaker and the number of usable edges is usually lower. Negative insert: the body is usually double-sided; offers a strong edge, suitability for heavy roughing and more usable edges; but the cutting force can be higher and it may cause vibration in thin or weakly clamped parts.

Nose Radius

The tip is not perfectly sharp; it has a nose radius (e.g. 0.2 / 0.4 / 0.8 / 1.2 mm). This affects edge strength, surface quality, permissible feed, cutting force and vibration tendency. Small radius: low cutting force, suits thin parts and small details; but weaker edge and less resistance to high feed. Large radius: strong edge, suits larger feeds and roughing; but higher radial force and vibration in thin parts. A large radius does not always give a better surface; if the system is not rigid, vibration increases.

Chip Breaker

The chip breaker is the special geometry on the insert’s top face; it curls the chip, breaks it into short pieces, reduces wrapping around the part and helps coolant reach the cutting zone. There are separate chip breakers for finishing, medium and roughing, plus aluminium, stainless and groove/parting geometries. A roughing chip breaker may fail to break the chip in a very small cut; a finishing geometry can break under a heavy chip. Chip-breaker type must also be considered in insert selection.

8. Insert Material Groups (ISO)

Manufacturers classify workpiece materials into general groups:

These letters do not give a single cutting speed; even within the same group, hardness, alloy content, operation type, interrupted/continuous cutting and coolant change the values. For example, machining aluminium with a general steel insert may look possible but can cause chip sticking and a poor surface. A tool unsuited to the workpiece material directly affects tool life and machining quality.

xF0x9Fx93xB7 IMAGE AREA — External, internal (boring bar), grooving and threading tools visual
Suggested alt text: “CNC lathe external, internal, grooving and threading tools”

9. Tool Groups: OD, ID, Grooving, Parting, Threading, Drilling

OD tools are the most common group; used for rough/finish OD, facing, profile, chamfer and taper. Right-hand and left-hand tools are for different feed directions; before writing a program you must know which way the tool can cut – feeding the wrong way causes the back face to rub, a poor surface and edge breakage. Some tools are neutral and can work in both directions to a limited extent.

ID tools (boring bars) are thinner and longer. In selection, the smallest hole diameter, hole depth, bar body diameter, overhang, insert shape, chip evacuation and coolant are considered together. The largest possible body diameter (more rigid) is preferred; but the bar must enter the hole and leave room for chips. The longer the bar overhangs, the more it vibrates; some bars deliver coolant internally to the tip. Grooving and parting tools work with thin blades and are sensitive to side force; they must be mounted perpendicular to the axis, at centre height, with minimum overhang. Threading tools require knowing not only the pitch but the profile (a full-profile insert gives a more controlled thread; a partial-profile insert can be used at different pitches). Drills and axial tools (centre drill, drill, reamer, tap, countersink) must be exactly centred in the turret; a centre error spoils the hole diameter and can break the tool.

Driven tools: on a standard CNC lathe the tool is fixed and the part rotates. On lathes with driven tools, some turret tools can be rotated for side drilling, face/slot milling, bolt-circle drilling and so on; these machines have a C and sometimes a Y axis. This course first takes the basic two-axis logic as its basis.

10. Turret, Tool Stations and T-Code Logic

The turret carries tools prepared for different operations; its capacity can be 8, 10, 12 or more stations. Each station is assigned a tool number and the tool order is prepared per the operation plan. On FANUC-based lathes the T address is used to call a tool. Common usage:

In short: the T code is used to select a tool and, in most FANUC lathe applications, to call the related offset.

11. Basic Logic of ISO Insert and Holder Codes

Cutting inserts carry a code of letters and numbers. For example, the main parts of CNMG 120408:

Another example, CCMT 09T304, may have a different shape, a positive clearance angle and a 0.4 mm nose radius. External holders also use an ISO code (e.g. PCLNR 2525M12): it defines the clamping method, insert shape, approach angle, clearance angle, right/left hand, body dimensions and length. Because manufacturers add their own chip-breaker and grade codes on top of the ISO system, the exact match must come from the manufacturer’s catalogue. The student should first read three points: which insert the holder works with; right, left or neutral; and whether it physically suits the turret and the operation.

12. Correct Tool Mounting: Centre Height, Overhang and Rigidity

On a lathe the cutting tip should ideally be at the workpiece rotation centre. Above centre: a pip can remain at the face, the tool can rub, size/surface can suffer; below centre: the cutting angle is disturbed and the tip can break (a serious risk especially in parting). On turret machines, with correctly made holders, centre height is mostly ensured mechanically; but a wrong seat, unsuitable shim, wrong holder size or turret misalignment can cause an error.

Tool overhang: the further the holder projects, the more it bends; excessive overhang causes vibration, taper, dimensional change, poor surface and edge breakage. General rule: the tool should project only as far as needed for the operation, not unnecessarily long; but too short a mounting can block access to a shoulder – the right overhang is the balance between access and rigidity.

Correct seating in the turret: before mounting, the turret and holder surfaces must be cleaned, no chips in the seat, bolts sound and tightened to the correct torque. Even a small chip trapped between tool and turret can change the tool’s height, angle and offset value. The cutting force is transmitted from the tip to the seat, holder, turret and machine body; if any link in the chain is weak, the system flexes or vibrates. Firm, balanced mounting, precise insert seating and easy tool change are the fundamentals.

Correct Insert Seating

Before fitting an indexable insert, clean the seat; check for chips in the pocket, the soundness of the shim, the state of the clamping screw, the insert direction and the integrity of the cutting edge. A very small chip under the insert can raise or tilt it, cause vibration and lead to the insert breaking during cutting. Over-tightening the insert screw can damage the screw or insert; under-tightening lets the insert move.

13. Tool Selection by Workpiece and Operation

One of the first things to look at is the workpiece material. Low-carbon steel gives soft/ductile chips and needs a suitable chip breaker. Alloy steel needs a more durable insert grade and suitable cutting values. Stainless steel can show work hardening, high temperature and sticky chips; sharp but durable geometry and steady feed are needed. Cast iron forms short/brittle chips and an abrasive dusty environment. Aluminium chips can stick to the tip; bright, sharp, wide-channel positive inserts are preferred. Hardened steel may require certain carbide grades, ceramic or CBN.

Even in the same material, the operation changes the tool. Roughing: strong insert, larger nose radius, rough chip breaker, rigid holder; finishing: sharp geometry, small/medium radius, finishing chip breaker, precise offset; interrupted cutting (groove/hole present): tougher grade, strong edge, lower speed, rigid mounting; thin-walled part: positive insert, sharp geometry, small radius, low depth of cut.

14. What Chip Form and Tool Wear Tell You

The chip gives important information about cutting conditions. Long chips wrapping the part: feed too low, depth of cut too small for the breaker, wrong chip breaker or ductile material; risks wrapping, surface scratching and operator hazard. Very small/dusty chips: brittle material, excessively small cut or the tool rubbing instead of cutting. Very dark chips: possibly high temperature, but colour alone is not enough for a firm decision.

An insert wears as it is used; what matters is that the wear is controlled. Main types: flank wear (size change, rising force, poor surface), crater wear (chip flowing over the top face), notch wear (at the depth-of-cut line), built-up edge (material sticking to the edge, size instability) and edge fracture (impact, overload, wrong grade, loose insert, collision). The tool is used not until it fully breaks but up to a controlled wear limit; it is changed when surface/size begins to deteriorate. FANUC systems can have tool-life management functions; when a set life is reached, another tool in the same group can be brought in.

15. Relationship Between Tool Offset and Tool Geometry

The tips of all tools in the turret are not at the same physical point: the T01 OD tip is in one position, the T02 grooving tip further forward, the T03 boring bar longer, the T04 drill tip at a different Z at the centre. The control unit knows each tool’s cutting-tip position via tool offsets; when a tool is called, the program coordinates are corrected so the real tip goes to them. The difference between the tool reference point and the real cutting tip is the offset value. Measuring tool geometry and wear offsets is covered in a separate lesson.

xF0x9Fx93xB7 IMAGE AREA — Example part (Ø50 bar, steps, chamfer, groove, thread, hole) and T01–T07 tool sequence
Suggested alt text: “CNC lathe tool plan and operation sequence for an example part”

16. A Tool-Selection Example for One Part

Consider this part: raw Ø50 steel bar; Ø40 and Ø30 steps; a 2 mm chamfer at the front; a 4 mm-wide groove; an M30 × 2 external thread; a Ø12 centre hole; parting from the bar at the end. A possible tool sequence:

17. Points to Watch When Setting Tool Order

• Build rigidity first: complete heavy roughing before the part gets too thin.
• Do not spoil the workholding: parting is left to the end.
• Prepare the reference surface: facing is usually among the first operations.
• Hole–OD relationship: if concentricity is needed, machine them in the same setup if possible.
• Groove before thread: if there is a thread-relief groove, cut it before threading.
• Protect the finish: finished surfaces are machined in an order that avoids damage from heavy chips.
• Reduce tool changes: operations doable with the same tool are grouped where possible, without compromising size and surface.

18. Tool-Change Safety and Cutting Warnings

When changing a tool/insert in the turret: stop the machine safely, stop the spindle completely, move the turret to a safe position, prevent unintended program start, do not touch sharp edges with bare hands, use the proper key, clean the insert/seat, and check tool tightness after the change. Even if the new insert has the same geometry, there can be a small size difference; measure the first part, correct the wear offset if needed and run the tool path under control.

During cutting the operator should watch the tool. A sharp squeal, regular wavy vibration, a sudden load rise, a sudden change in chip form, a dulling surface, a gradually changing diameter or chips wrapping the tool can indicate a problem. In these cases, only lowering the feed is not always the right fix; the real cause may be the wrong insert, wrong mounting, excessive overhang, a worn insert, wrong cutting speed or weak workholding.

19. The Right Method for Cutting-Tool Selection

Tool selection is not done by guessing. Suggested order: identify the workpiece material → define the operation (OD/ID, groove, thread…) → decide roughing or finishing → assess part rigidity/workholding → check machine power and speed range → choose insert shape, grade, chip breaker and nose radius → choose a suitable holder → check profile access → take starting cutting values from the manufacturer catalogue → observe chip, surface and spindle load in the first operation → correct the values under control if needed. Inserts are evaluated together with material, operation type, cutting speed, feed, chip breaker, clamping type, cutting direction and holder.

The manufacturer catalogue is not just a product list; it contains the insert’s suitable material group, rough/medium/finish application, cutting-speed/feed/depth-of-cut ranges, coolant recommendation, suitable holders and number of usable edges. So a single cutting-speed value found at random online should not be applied to all inserts.

20. Shop Names vs. Technical Names, and Consequences of Wrong Selection

A student may hear different names for the same tool: holder / tool holder; boring bar; “diamond insert” / carbide insert; parting bit; threading bit; grooving tool. In the shop “diamond insert” is often used for a general indexable carbide insert; but not every carbide insert is diamond – a real diamond-based PCD insert is a different cutting material.

Consequences of wrong tool selection: if the tool cannot enter the profile, the shape is not formed; if the cutting direction is wrong, the tool rubs with its side; if the insert is unsuited to the material, there is fast wear, sticking and breakage; a roughing insert gives a poor surface in finishing; a finishing insert breaks in heavy roughing; too large a nose radius makes a thin part vibrate and spoils profile detail; a boring bar mounted too long causes vibration, taper and dimensional change.

Lesson Summary

• The program defines the tool’s motion; the element that actually removes the chip and forms the surface is the cutting tool. Insert, holder and tool system are distinct concepts.
• Basic operations: facing, OD, ID, taper, profile, grooving, parting, drilling, threading, chamfer and radius. Each needs a suitable tool.
• HSS and carbide are the basic materials; insert shape, positive/negative geometry, nose radius and chip breaker set performance. ISO codes (P/M/K/N/S/H and e.g. CNMG 120408) define the tool.
• Centre height, short overhang and rigid mounting are the basis of a correct result; the T code calls the tool and offset.
• Tools are chosen by material and operation type; chip form and wear types inform cutting conditions; selection is verified with catalogue data.

Assessment Test

1. What is the body that carries the insert and transmits cutting forces to the turret called? A) Insert B) Holder C) Turret D) Tailstock
2. Which operation is used to separate the part from the bar? A) Facing B) Grooving C) Parting D) Radius machining
3. (True/False) In the code CNMG 120408, the last two digits (08) usually mean a 0.8 mm nose radius.
4. In the ISO material grouping, which materials does “N” represent? A) Steel B) Stainless steel C) Cast iron D) Non-ferrous (aluminium, etc.)
5. (True/False) The longer a boring bar is mounted, the higher the rigidity and the lower the vibration.
6. For a thin-walled part, which is generally preferred? A) Negative insert and large radius B) Positive insert, sharp geometry, small radius C) High depth of cut D) Long-overhang mounting
7. What does T0303 mean on most FANUC lathes? A) 3rd tool, 3rd offset B) Station 33 C) 3 mm feed D) 3rd axis

Open-Ended Questions

• Explain the difference between insert, tool holder and cutting tool.
• Compare positive and negative inserts with their advantages/disadvantages.
• Explain the effect of nose radius on surface quality, cutting force and vibration.
• Why should tool overhang be kept as short as possible?
• Propose a suitable tool sequence for an example part (step + groove + thread + hole).

Summary and Next Lesson

In this lesson we learned how chips form in turning, the basic operations, the insert–holder distinction, HSS and carbide inserts, insert geometry (shape, positive/negative, nose radius, chip breaker), ISO codes, and tool mounting and selection. Now, looking at a technical drawing, you can think not only of the dimensions but of the required operations and the tool group for each. In the next lesson we will cover cutting speed, spindle speed, feed, passes and the machining plan and learn under which cutting conditions to run the tools we chose.