CNC Lathe Training Lesson 2: Axes, Coordinate System and Reference Points

The foundation of CNC lathe programming is not memorising G and M codes, but being able to correctly describe where the cutting tool is relative to the part and where it will move. Without understanding what the values X40 Z-30 in a program line mean, it is impossible to use commands like G00, G01, G71 or G76 correctly – because in the end all of these commands move the tool to specific coordinates.

The CNC control unit does not see or interpret the part visually; it only processes the numerical data it is given. So the programmer must set a suitable zero point on the part, know the directions of the X and Z axes, break the part profile into coordinate points, calculate the diameter and length value of each point, and define safe start and retract positions for the tool. In this lesson we will learn the axis directions on a CNC lathe, the machine and workpiece zeros, the reference point, the absolute and incremental coordinate systems, diameter programming, and extracting coordinates from a technical drawing.

xF0x9Fx93xB7 IMAGE AREA — CNC lathe X–Z coordinate plane and workpiece zero overview
Suggested alt text: “CNC lathe X-Z coordinate system and workpiece zero point”

1. Why Is a Coordinate System Needed?

When giving directions in a city, saying only “a bit right, then straight on” is not enough; the start point, direction and distance must be known. On a CNC machine the tool position is defined by the same logic. The control unit needs to know: on which axis the motion happens, whether the direction is positive or negative, which point the tool goes to, relative to which zero it is measured, whether the given X is diameter or radius, and whether the value is written relative to the current position or the part zero.

A coordinate system lets us define a point’s location numerically. On a standard two-axis CNC lathe, tool movements mostly occur in the X–Z plane. A coordinate system generally consists of three elements: the zero point (origin), the axes, and the positive/negative directions of the axes. Coordinates written without a defined zero have no meaning; for example Z-30 describes a real position only when it is known where Z zero is.

xF0x9Fx93xB7 IMAGE AREA — X and Z axis directions (Z+ away from chuck, X+ outward from centre) labelled diagram
Suggested alt text: “CNC lathe X and Z axis directions diagram”

2. Basic Axes on a CNC Lathe

A standard CNC lathe has two main linear axes: the Z axis and the X axis. Some advanced machines also have Y and C axes, a second turret or a second spindle; but the beginner level is learned through X and Z.

2.1. Z Axis

The Z axis is parallel to the rotation axis of the spindle and workpiece; that is, it is the tool’s motion along the length of the part. On a standard horizontal CNC lathe, the direction away from the chuck/part is usually Z+ and the direction toward the chuck and into the part is Z−. When the face of the part is chosen as Z zero, points outside the part are generally positive and points within the machined length are generally negative Z. For example, with the face as zero, Z5 means the tool is 5 mm in front of the face and Z-30 means 30 mm inside from the face.

You can think of the Z axis as the length axis of the part: Z0 the face, Z-10 10 mm in, Z-40 40 mm in, Z5 5 mm in front. But if the zero is chosen on another surface, the Z values change accordingly. So instead of “Z always starts from the front face,” the correct statement is: Z coordinates are calculated relative to the workpiece zero defined for the program.

2.2. X Axis

The X axis is perpendicular to Z and represents the tool’s motion in the diameter direction: it determines the tool approaching/retreating from the part centre and the machined diameter growing/shrinking. General rule: the tool moves X+ away from the centre and X− toward the centre. So the positive direction is the one that increases the machined size.

Where is X0? On a standard CNC lathe the X0 point of the workpiece coordinate system is the rotation centre of the part. When the tool tip reaches the centre line, the X value is zero. In diameter programming, X50 is the tool tip’s position on a 50 mm diameter, X30 on a 30 mm diameter, and X0 the part centre.

xF0x9Fx93xB7 IMAGE AREA — Diameter vs. radius programming (Ø40 = X40, radial 20 mm) visual
Suggested alt text: “CNC lathe diameter programming vs radius difference diagram”

3. Why Is X Usually Written as Diameter on a Lathe?

One of the most important topics in CNC lathe programming is diameter-programming logic. On a technical drawing, cylindrical parts are usually dimensioned by diameter (Ø50, Ø40, Ø30). So the programmer does not have to keep converting these to radius, most CNC lathes program X values as diameter. For example if the part diameter is 40 mm, the program usually says X40; even though the tool’s real physical distance from the centre is 20 mm, the diameter value 40 mm is entered into the control unit. Because the X axis on FANUC controls can be configured as diameter or radius, you must know how the actual machine is set. In Mentor CNC’s basic lathe examples, in line with common industry practice, X values are used in diameter terms.

Diameter vs. radius: for a part of 40 mm diameter, the diameter value is 40 mm and the radius value is 20 mm. In diameter programming you write X40, in radius programming X20. If the wrong system is used, the tool can move twice or half the expected amount. So before running, confirm whether the machine programs in diameter or radius.

4. Relationship Between X-Axis Motion and Diameter Change

Diameter programming is one of the things beginners confuse most. If an outside diameter is reduced from 50 mm to 46 mm, a total of 4 mm is removed from the diameter; but the tool’s real radial movement is 2 mm, because material is removed from around the circumference:

Radial depth of cut = (Start diameter − Final diameter) ÷ 2
(50 − 46) ÷ 2 = 2 mm

Because the diameter value is used in the program, you write X46; the machine calculates internally that the tool must physically move 2 mm toward the centre. Another example: if the part diameter is reduced from Ø60 to Ø50, the diameter change is 10 mm and the tool’s real radial plunge is 5 mm. This distinction matters especially for depth of cut, tool offset correction, dimensional correction and incremental X motion.

xF0x9Fx93xB7 IMAGE AREA — Machine zero, reference point and workpiece zero shown on the machine
Suggested alt text: “CNC lathe machine zero, reference and workpiece zero points”

5. Zero and Reference Points on a CNC Lathe

A CNC lathe does not have a single zero; there are several important points used for different purposes: machine zero, reference point, workpiece zero, tool reference point and program start/park point. Their roles differ.

5.1. Machine Zero

Machine zero is a fixed point set by the machine builder according to the machine’s structure. It is the origin of the machine’s own coordinate system, cannot be changed arbitrarily by the operator, is related to the machine’s physical travel limits, and forms the basis of the machine coordinate system. It is not used to make programming easy; so the operator does not have to compute every part’s dimensions relative to machine zero, a workpiece zero is created separately on the part.

5.2. Machine Coordinate System

The coordinate system whose origin is machine zero is called the machine coordinate system. It depends on the machine’s physical structure, does not fundamentally change even if the part changes, and shows the real position of the axes on the machine. The X and Z values seen in the “MACHINE” section of the control screen are according to this system. On FANUC screens the tool position can be shown at the same time in absolute work coordinates, relative coordinates, machine coordinates and as distance-to-go. Machine coordinates matter especially for tool-change positions, safe retract, stroke limits and maintenance/service.

5.3. Reference Point

The reference point is a predefined point where axis positions are verified and which helps establish the machine coordinate system. When the machine is switched on, especially on machines with incremental position measurement, the real axis position may need to be established; the machine is then sent to the reference point (reference return, zero return, home). The machine coordinate system is established by performing a manual reference return after switch-on.

Are machine zero and reference point the same? In everyday shop language they are sometimes used interchangeably, but technically they need not always be exactly the same point. Machine zero is the origin of the machine coordinate system; the reference point is the physical point the axis goes to for position verification. The machine builder can set the reference point’s machine-coordinate value with parameters. So in training their roles should be explained separately rather than treating them as identical.

5.4. Workpiece Zero

Workpiece zero is the point on which dimensions are based when writing the program. To use the drawing dimensions easily, the programmer chooses a suitable zero on the part. The most common workpiece zero on a CNC lathe is the part’s centre axis in X and the part’s face in Z. In this case X0 Z0 is the centre point on the face of the part, and the diameter/length dimensions from the drawing can be transferred directly into the program.

Why is it needed? If we based everything on machine zero, since each new part’s overhang, length, jaws and tool position can change, computing all dimensions relative to machine zero would be hard and error-prone. Thanks to workpiece zero the programmer can say “in this program the front face is Z0 and the centre line is X0,” and all diameter/length dimensions are written relative to that point.

5.5. Workpiece Coordinate System

The coordinate system whose origin is workpiece zero is called the workpiece coordinate system; most of the X and Z values in the program are interpreted according to it. For example X40 Z-25, on a lathe using diameter programming, means the tool goes to the point at 40 mm diameter and 25 mm inside from the workpiece zero. Once this system is set, the programmer no longer thinks about the machine’s physical zero on each line, but works from the drawing. FANUC systems can offer several work coordinate options such as G54–G59; some older applications set the work coordinate with the G50 method or machine-specific offset screens. Key distinction: the logic of workpiece zero is universal; the method of registering that zero into the control unit varies by machine.

5.6. Tool Reference Point

The lengths and tip positions of the tools mounted in the turret differ from each other: the external turning tool tip is in one place, the grooving tool tip in another, the boring bar has a different length, the drill tip may be further forward. For the control unit to recognise each tool’s real cutting tip, tool dimensions are recorded in the offset system. The tool reference point is the base point used to measure tool positions. What to grasp at this stage: the coordinates in the program refer not to the tool body but, when the correct offset is defined, to the position the cutting tip must reach. Tool geometry and offsets will be covered in detail in a later lesson.

5.7. Park or Safe Standby Point

The park point is where the tool can wait at program start, retract at the end of an operation and safely change tools. It is set by the programmer according to the structure of the part and tool; there is no fixed universal park coordinate. For example on a small part X100 Z100 may look safe, but on another machine with a long boring bar, tailstock or large chuck the same coordinate may not be safe. When choosing a park point, the jaws, part overhang, tailstock, tool length, turret indexing envelope and machine stroke limits must all be considered together.

6. Difference Between Machine and Workpiece Coordinates

These two systems can show the same physical tool position with different numbers. For example while the tool is at one position the screen may show, at the same time, machine coordinate MACHINE X-320.000 Z-450.000 and workpiece coordinate ABSOLUTE X60.000 Z5.000. The tool is physically at the same point; what differs is the zero from which measurement starts. Think of it as two different rulers: one starts from the machine’s fixed point, the other from the part’s face. The programmer mostly uses the workpiece coordinate system; the machine coordinate system matters for tracking the machine’s real position and limits.

7. Absolute Coordinate System

In the absolute coordinate system all target points are described relative to the same fixed zero; on a CNC lathe this is usually the workpiece zero. In FANUC lathe programming, absolute coordinates are given with X in the diameter direction and Z in the length direction. For example X50 Z0 is the point at 50 mm diameter and on the face; X40 Z-20 at 40 mm diameter and 20 mm inside; X30 Z-50 at 30 mm diameter and 50 mm inside – all relative to workpiece zero.

Key feature of the absolute system: even if the tool’s previous position changes, the target point’s coordinate does not. For example if point B is X40 Z-30, then whether the tool comes from A, from C or from the safe start point, B’s absolute coordinate is still X40 Z-30. This makes writing a program from the drawing easier.

8. Incremental Coordinate System

In the incremental coordinate system the target point is described relative to the tool’s current position, not the fixed workpiece zero. In FANUC-based lathe programming, incremental moves are commonly written with U in the X direction and W in the Z direction. For example U-10 W-20 means the tool, from its current position, reduces 10 mm in diameter and moves 20 mm negative in Z. In short, X–Z give the absolute position, U–W give the incremental move from the current point to the next.

Example: let the tool’s current position be X60 Z5. The command U-20 W-35 gives the new position X40 Z-30:

X_new = 60 − 20 = 40  |  Z_new = 5 − 35 = −30

9. Diameter-Programming Detail in the U Value

The U address (incremental X motion) can also be interpreted on a diameter basis, depending on the control and parameter setup. In the common FANUC application using diameter programming, U-4 means the target diameter decreases by 4 mm; the tool’s physical radial movement is 2 mm. For example if the current position is X50, after U-4 the target is X46. This detail is very important for depth-of-cut calculation: saying “U-4 means the tool plunged 4 mm toward the centre” can be wrong on a machine using diameter programming. Since control and machine settings can differ, the actual machine’s programming setup must be checked.

10. Can Absolute and Incremental Be Used Together?

In many FANUC lathe applications, absolute and incremental axis addresses can be used together in the same block. For example G01 X40 W-20: go to 40 mm diameter in X absolutely, and advance 20 mm negative in Z from the current position. Similarly G01 U-4 Z-30: reduce 4 mm from the current diameter in X, and go to absolute -30 in Z. This flexibility is useful in some programs; but in beginner training, to avoid confusion, it is better to work first with fully absolute or fully incremental examples.

11. Important: G90 Is Not “Absolute Mode” on Every Lathe

In milling, G90 is commonly used for absolute and G91 for incremental programming. But in G-code system A used on FANUC lathes, G90 can be not an absolute-mode selection but an outside/inside diameter turning cycle. So in FANUC lathe programming, absolute targets are mostly given directly with X and Z, and incremental moves with U and W. The “G90 = absolute, G91 = incremental” information seen online or in various books should not be applied directly to every control system. The right approach: first check the control unit’s G-code system and the machine builder’s programming setup. In Mentor CNC’s FANUC lathe examples, at beginner level, X–Z is emphasised for absolute position and U–W for incremental motion.

12. Determining Coordinate Signs

In coordinate calculation not only the numeric value but also the sign matters: + shows the positive direction, − the negative. For positive values the + is usually omitted; Z5 equals Z+5. The negative sign must always be written: Z-25. With the face as Z0, the outer side of the part is Z+ and the section machined toward the chuck is Z−. For example Z2 is the approach point 2 mm in front of the part and Z-40 is a point 40 mm into the part. In standard external turning, X values are mostly positive (X60, X40, X20, X0); crossing into the negative X region means the tool passes the centre line, which is usually not required in beginner external-turning programs.

xF0x9Fx93xB7 IMAGE AREA — Stepped part profile and A–E coordinate points (Ø50→Ø40→Ø30) labelled drawing
Suggested alt text: “Stepped lathe part profile points and coordinates”

13. Extracting Coordinates from a Technical Drawing

When writing a CNC lathe program, the part profile is thought of not as a single shape but as connected points. The programmer determines the part’s diameter changes, length changes, corner points, chamfer and radius start/end points, and groove positions; and finds an X and Z coordinate for each transition point. The transition points of lathe parts are extracted as a table with diameter and length values; this reduces the chance of error before writing the program.

14. Extracting Coordinates on a Simple Stepped Part

Consider this part: raw diameter Ø50; first step Ø40, length 20 mm; second step Ø30, total length 50 mm; workpiece zero at the front-face centre. Profile points: A centre and face X0 Z0; B face of the first diameter X40 Z0; C end of the first step X40 Z-20; D start of the second diameter X30 Z-20 (at the same Z the diameter drops from 40 to 30); E end of the second step X30 Z-50.

15. Incremental Coordinates of the Same Part

On the same profile, starting from point B, let us compute the incremental moves. B→C: X unchanged (U0), Z 20 mm negative (W-20). C→D: diameter reduces 10 mm (U-10), Z unchanged. D→E: X unchanged, Z change −50 − (−20) = −30, i.e. W-30.

16. Advantages of the Absolute System

Absolute coordinates are mostly preferred in CNC lathe programs. Reasons: drawing diameters can be used directly; each point is independent relative to workpiece zero; an error in a previous line does not shift the following coordinates; the program is easier to read; profile points can be compared with the drawing; restarting from the middle of the program is clearer. For example a programmer seeing the line X40 Z-30 immediately understands where the target point is.

17. Advantages and Risks of the Incremental System

Incremental programming is useful for repeated equal-distance moves, retracting a set amount from a point, stepped approaches, subprograms and when relative motion from the current position is needed. For example to move the tool 2 mm in diameter and 1 mm in length away from its current position, U2 W1 can be used. But it has an important risk: if the previous position is wrong, the next incremental move also starts from the wrong point. Also, without knowing the current position, it can be hard for a reader to work out which absolute position the U and W values end at. At beginner level, writing the main profile in X–Z absolute and short retracts in U–W when needed improves readability.

xF0x9Fx93xB7 IMAGE AREA — Start/end coordinates for chamfer, taper and radius transitions
Suggested alt text: “Lathe chamfer, taper and radius coordinate points diagram”

18. Calculating Chamfer Coordinates

Suppose a part has a 2 × 45° chamfer at the corner and the main diameter is Ø40. If the front face is Z0, the 45° chamfer produces an equal radial distance in the diameter and length directions. But because X is written as diameter, a radial 2 mm change corresponds to a 4 mm change in diameter. For an external chamfer, two key points: the small diameter at the face Ø36 (Z0) and the chamfer end at the main diameter Ø40 (Z-2). Because 40 − (2 × 2) = 36. Coordinates: X36 Z0 and X40 Z-2. This example shows why diameter programming must be well understood: subtracting the chamfer’s radial size directly as just 2 mm from X leads to a wrong profile. Chamfer dimensioning on drawings can vary; whether the given value is axial length, radial length or the value between two diameters must be read carefully.

19. Coordinate Logic on Tapered Surfaces

On a tapered surface the tool moves in both X and Z at the same time. For example if the taper starts at Ø30 at Z-20 and ends at Ø40 at Z-50, the start is X30 Z-20 and the end X40 Z-50. When the tool makes a linear cut between these two points, a tapered surface is formed. You do not always need the angle to program a taper; if the start and end X–Z coordinates are known, the control unit forms the line between them. If the angle, large/small diameter or length is missing, a geometry calculation may be needed; this is covered in advanced applications.

20. Coordinate Logic on Radiused Surfaces

When programming a radius, not only the radius value but also the arc’s start point, end point and direction must be known. For example on a profile the arc start could be X30 Z-20 and the end X40 Z-25. Later in the program an arc between these two points is created with G02 or G03. We do not go into G02–G03 detail in this lesson; but the key idea is important: a radius, too, is a geometric move with start and end points from the coordinate-system perspective.

21. How Is a Safe Approach Point Chosen?

The cutting tool should not be sent by rapid directly to the finished profile point of the part. For example if the raw diameter is Ø50, going to X40 Z2 with G00 causes a crash, because X40 corresponds to inside the raw material. The safe approach point must be chosen outside the raw diameter; for example X52 Z2 or, with enough safety margin, X55 Z3. If the raw diameter is Ø50, X50 is right on the raw surface, X52 is 2 mm in diameter (1 mm radial) outside, and X55 is 5 mm in diameter (2.5 mm radial) outside. In Z, too, a positive start distance is left so the tool does not hit the face. Suitability depends on raw diameter, part runout, workholding, tool geometry and the machining operation.

22. Reference Return Logic with G28

One command often seen in FANUC lathe programs is G28 U0 W0. G28 is used to return the tool to the reference point; but its travel path, intermediate-point logic and the offsets in use must be carefully evaluated. When U0 W0 is used, the current position is taken as the intermediate point and the axes go to reference. Even so, on a real machine, a long tool, chuck, tailstock, part and turret must be evaluated for collision risk. The presence of G28 does not mean the command is automatically safe in every case; the path the tool follows to reference must be checked. On some machines G53 machine coordinate can also be used for safe return; G53 selects the machine coordinate system only in the block where it is written and is used with absolute values.

23. Two Different Uses of the G50 Command

In older, common FANUC lathe programs, G50 can appear in two contexts: setting the coordinate system, and limiting the maximum spindle speed. For example G50 S2500 usually limits the maximum spindle speed to 2500 rpm. In some older methods G50 X... Z... can be used to set a workpiece coordinate system relative to the tool’s current position. So G50 in a program should not be interpreted by its code number alone; the addresses next to it and the control’s G-code setup must be evaluated. On modern machines the workpiece zero is mostly managed through offset screens and work coordinates like G54; but in older programs you may encounter setting coordinates with G50.

24. ABSOLUTE, RELATIVE and MACHINE Values on the Control Screen

• ABSOLUTE: shows the tool’s current position relative to the workpiece coordinate system. For example X 40.000 / Z -30.000 means the tool is at X40 Z-30 relative to part zero.
• RELATIVE: a relative position display the operator can zero when needed; used to track a certain distance moved or for temporary measurement in manual settings. Zeroing the relative display does not always change the workpiece coordinate system; the two zeros must not be confused.
• MACHINE: shows the tool’s position relative to machine zero; it relates to the machine’s physical position even if the workpiece zero changes.
• DISTANCE TO GO: shows how far the axes still need to move to reach the target in the running block (the remaining distance).

25. Most Common Mistakes About Coordinates

• Mistaking X for radius: when Ø40 is seen on the drawing, in diameter programming X40 must be written; writing X20 takes the tool to the wrong diameter.
• Confusing the Z sign: with the face at Z0, machining into the part is usually negative Z; for 30 mm of length you write Z-30.
• Thinking machine zero and workpiece zero are the same: machine zero is set by the builder, workpiece zero is defined on the part to suit the program.
• Thinking reference return means workpiece zeroing: sending the machine to reference does not automatically make the face Z0; the workpiece zero must be registered separately.
• Thinking U is physical radial motion: in diameter programming U-4 can be a 4 mm change in diameter, not a 4 mm radial plunge.
• Thinking G90 is absolute on all lathes: in some FANUC lathe G-code systems G90 is a turning cycle.
• Thinking a safe point is just a large coordinate: X100 Z100 may not be safe on every machine; a long tool, tailstock or turret geometry can cause a crash.
• Running an old program after changing the zero without checking: a small error in the zero can affect all Z dimensions or diameters; a wrongly set coordinate system can cause dangerous tool motion.

26. Working Order When Extracting Coordinates

1. Determine the part’s rotation axis (this line is usually the X0 centre line).
2. Choose the Z zero (at beginner level usually the finished face, Z0).
3. Determine the raw material diameter and length.
4. Mark the profile corner points (each point where diameter or direction changes is a separate profile point).
5. Find the X value of each point (in diameter programming, the diameter dimension from the drawing).
6. Find the Z value of each point (the signed length distance from the chosen Z zero).
7. Calculate chamfer and radius transitions (the real tangent start/end points).
8. Create a coordinate table.
9. Add the raw material and safe approach points.
10. Re-check the coordinates against the drawing.

27. Applied Example: Coordinates of a Stepped, Chamfered Shaft

Consider this part: raw diameter Ø60; front section Ø40, length 20 mm; second section Ø50, from Z-20 to Z-55; a 2 × 45° chamfer at the front corner; workpiece zero at the front-face centre. Since the main diameter is Ø40 and the chamfer is 2 × 45°, the small diameter of the chamfer at the face is: 40 − (2 × 2) = 36.

28. The Real Importance of the Coordinate System in Programming

G codes tell the tool how to move (rapid, linear cutting, arc, or with a cycle); coordinates tell the tool where to go. For example in the line G01 X40 Z-30, G01 sets the motion type and X40 and Z-30 the target point. Even if G01 is correct, if X or Z is wrong the tool goes to the wrong place. So coordinate calculation is not a sub-topic of programming but its direct foundation. A good programmer, looking at a part, sees not only the diameter and length dimensions but forms in their mind the workpiece zero, the X–Z axes, the profile points, the approach direction and the safe retract position. All of G00, G01, G02, G03 and the canned cycles we will learn later are built on this coordinate logic.

Lesson Summary

• On a CNC lathe, tool moves are defined in the X–Z plane; Z is the length and X the diameter direction. Z+ is away from the chuck, X+ outward from the centre.
• X values are mostly written as diameter; half of the diameter change is the tool’s real radial movement.
• Machine zero, reference point and workpiece zero have different roles; the programmer mostly uses the workpiece coordinate system.
• Absolute coordinates are relative to a fixed zero (X–Z), incremental to the current position (U–W); at beginner level the absolute system is safer and more readable.
• The drawing is broken into profile points and written into a coordinate table to prepare for programming; chamfer, taper and radius are also defined by start/end points.

Assessment Test

1. On a lathe using diameter programming, when Ø40 is seen on the drawing, what is written in the program? A) X20 B) X40 C) X80 D) R40
2. When an outside diameter is reduced from Ø50 to Ø46, what is the tool’s real radial movement? A) 1 mm B) 2 mm C) 4 mm D) 8 mm
3. (True/False) In the absolute coordinate system, all target points are described relative to the same fixed zero (usually the workpiece zero).
4. With the current position X60 Z5, what is the new position after U-20 W-35? A) X40 Z-30 B) X80 Z40 C) X40 Z-40 D) X20 Z-30
5. (True/False) In some FANUC lathe G-code systems, G90 can be a turning canned cycle rather than absolute mode.
6. On a part with raw diameter Ø50, which is suitable as a safe approach point? A) X40 Z2 B) X50 Z0 C) X52 Z2 D) X30 Z-10
7. Which display shows the tool’s position relative to the workpiece zero? A) MACHINE B) ABSOLUTE C) DISTANCE TO GO D) RELATIVE

Open-Ended Questions

• Explain the differences between machine zero, reference point and workpiece zero.
• Explain the difference between diameter and radius programming with an example.
• Compare the advantages and risks of the absolute and incremental coordinate systems.
• For a part with raw diameter Ø50, why should the tool not be sent directly to X40 with G00?
• List the steps for converting a technical drawing into a coordinate table.

Summary and Next Lesson

In this lesson we learned the axis directions of the CNC lathe, the machine and workpiece zeros, the reference point, diameter programming, absolute/incremental coordinates and extracting coordinates from a technical drawing. This coordinate logic is the foundation of all the following lessons. In the next lesson we will cover cutting tools, tool holders and machining operations and learn how to choose the right tool for each operation on a part.