LATHE TURNING

AND CNC
MACHINING

Dr Scott Millen
MEE2034: Manufacturing Technology
LEARNING OUTCOMES AND OVERVIEW
Outcomes
• You should be able to differentiate drilling, turning and milling,
• You should understand what numerical control is and how it relates to machining or manufacturing,
• You should understand the three metrics to determine how well the programme is doing,
• You should be aware of programming languages,
• You should be able to calculate speeds and feeds for a given process.

Overview
• Lathe turning,
• CAD/CAM programming,
• CNC milling and tooling.
 LATHE TURNING I
• A single point cutting tool removes material from a rotating workpiece to generate a cylindrical shape,

Simple Turning Operation

https://www.hubs.com/knowledge-base/cnc-machining-manufacturing-technology-explained/
 LATHE TURNING II
• Variations of turning that are performed on a lathe:
• Facing, Step turning, Grooving, Chamfering, Parting, and more…

https://msvs-dei.vlabs.ac.in/mem103/Unit5lesson4.html
LATHE TURNING III
Facing - Tool is fed radially inward to remove material from the front of the stock,

Step Turning - creates two surfaces with an abrupt change in diameters between them. The final
feature resembles a step.

Chamfering - cuts an angle on the corner of the cylinder, forming a "chamfer"

Grooving - creates a narrow cut, a "groove" in the workpiece. Multiple tool passes
are necessary to machine wider grooves.

Parting (Cutting Off) - results in a part cut-off at the end of the machining cycle.

Others include: Taper turning, Contour Turning, Threading, Knurling, Drilling, Reaming, Boring and
Tapping.

https://turntechprecision.com/clueless-machinist/2020/8/25/10-machining-operations-performed-on-a-lathe
https://www.youtube.com/@TomsTechniques
https://www.youtube.com/@YorkIndustrialTech
https://www.youtube.com/@SecoToolsAB
 INTRODUCTION TO CNC MACHINING/MILLING
• CNC machining is the most common subtractive manufacturing technology today,

• Using CAD models, CNC machines precisely remove material from a solid block with a variety of
cutting tools,
• High speed spindle (> 40,000 rpm),

• High feed rate drive ( > 15 m/min),

• High precision ( < 0.002 mm accuracy),

Degrees of freedom (DOF) in milling. NB: rotation around the x-

axis is the A-axis DOF; rotation around the y-axis is the B-axis
DOF.

Manufacturing and Design: Understanding the Principles of How Things Are Made by Bruno Ninaber van Eyben, Erik Tempelman, and Hugh Shercliff
CNC MACHINES
• Generally, CNC machines share a common layout:

• A flat working table,

• A milling cutter holding the cutting tool,

• The tool rotates at high speeds with considerable down force,

• There are also control and electronics involved.

 CNC MACHINING - 3-AXIS vs 5-AXIS
• 3-Axis Machining - the workpiece is fixed in a single position – the spindle can move in X, Y and Z linear
directions,
• Typically used for machining of 2D and 2.5D geometry. Machining of all 6 sides of a part is possible in 3-axis machining
but a new fixturing set-up is required for each side,

• 5-Axis Machining – the spindle/workpiece can also rotate in the A-axis and C-axis, or in the B-axis and C-axis,
• Typically, capable of highly complex 3D shapes and surfaces.

https://www.cloudnc.com/blog/cnc-best-practices-3-whats-the-difference-between-3-axis-4-axis-5-axis-milling
CNC MACHINING - COORDINATE SYSTEMS
• CNC motion is based on the Cartesian coordinate system,

• Machine Coordinate System (MCS) - the XYZ position with respect to the
home position (start position),

• Part Coordinate System (PCS) - establishes the Orientation, Alignment and

Origin of your part,

• Fixture Coordinate System (FCS) - a previously measured coordinate system

saved away for recall and used in repeated part programs.
NC PROGRAMMING LANGUAGES
• There is no standard NC programming language,
• Every CNC machine manufacturer has a special language for programming their machines,
• The closest to a standard language are G/M codes,
• A G/M code CNC program is made up of a series of commands. Each command or block is
made up of words,
• Each word is composed of a letter address (X,Y,Z,R, etc.) and a numerical value.

Components of a G/M Code Program

• Sequence number (N-words) • Spindle speed (S-words)
• Preparatory work (G-words) • RPM -rev./min.

• Coordinates (x-, y-, z-words) • Tool selection (T-words)

• Feed rate (F-words) • Tool length offset (H-words)
• Feed rate - mm/min. • Tool radius offset (D-words)
• Specifies Miscellaneous functions (M-words)
G- and M- Words
Miscellaneous function (M-words) Instructions to the controller (G-words)
M00 Stop program G00 Point-to-point operation (rapid speed)
M03 Start spindle on CW direction G01 Linear interpolation
M04 Start spindle on CCW direction G02 Circular interpolation -clockwise
M05 Stop spindle G03 Circular interpolation -counterclockwise
M06 Tool change G04 Dwell (wait) for programmed duration
M07 Turn coolant on (mist mode) G90 Absolute mode
M08 Turn coolant on (flood mode) G91 Incremental mode
M09 Turn coolant off
M30 End of program
G- and M- Words Example 1
N015 G00 X5.0Y5.0

Statement Number 15 (N015)

G- and M- Words Example 2
N0027 G01 X175.25 Y325.00 Z136.50 F125 S800 T1712 M03 M08
-----------------
N0027 - Statement Number 27,
G01 - a linear-interpolation motion to a position defined by:
X175.25 Y325.00 Z136.50)
F125 - with a feed rate of 125 mm/min,
S800 - and a spindle speed of 800 rpm,
T1712 - using a tool Number 1712,
M03 - performing a clockwise turn of the spindle,
M08 - and having the coolant on.
ACCURACY IN NUMERICAL CONTROL
• ACCURACY, REPEATABILITY & RESOLUTION
• Accuracy = “correctness”. Closeness to required value,

• Repeatability = Ability to repeat the same result,

• Resolution = Smallest increment that can be read.

LOW ACCURACY LOW ACCURACY HIGH ACCURACY HIGH ACCURACY

LOW REPEATABILITY HIGH REPEATABILITY LOW REPEATABILITY HIGH REPEATABILITY
CNC CAM PROGRAMMING
• Once the part has been designed using conventional mechanical design methods (structural
analysis, FEA, fatigue study, etc.), the part is manufactured using the following method:
1. Create a solid 3D model of the part to be produced. Any standard CAD format is acceptable,

2. Import the solid model into the CAM (computer aided manufacturing) software,

3. Input the raw material stock size and set the part’s coordinate origin,

4. Input the necessary information for each tool used in machining the part features,

5. For each part feature, select the appropriate tool from the library and set the parameters necessary for machining that
feature. Typical parameters include spindle speed, depth of cut, feed rate, number of passes, tool path pattern, etc.

6. Verify the programmed tool path(s) by running the CAM software’s virtual machining cycle.
 CNC MILLING TOOLS
Peripheral milling
• Cutter axis is parallel to surface being machined,
• Cutting edges on outside periphery of cutter,
Face milling
• Cutter axis is perpendicular to surface being milled,
• Cutting edges on both the end and outside periphery of the cutter.

Peripheral Milling
Face Milling

https://www.xometry.com/resources/machining/face-milling-vs-peripheral-milling/ *Supplementary material covering milling on Canvas

 CNC MILLING TOOLS II

End Mills

https://www.xometry.com/resources/machining/types-of-milling-in-machining/
https://www.hubs.com/knowledge-base/cnc-machining-manufacturing-technology-explained/
 CNC MILLING TOOLS
Roughing and Finishing

• Roughing (or rough milling)

• The removal of larger amounts of material to quickly convert stock to the approximate final shape,

• Utilizes larger cutting tools, deeper and broader cuts, typically resulting in a coarser surface finish,

• Designed for efficiency and speed.

• Finishing
• Typically, the final stage of the machining process,

• Utilizes delicate, exact cuts using refined tools,

• Precise dimensions, stringent tolerances, and a superior surface finish can be achieved.

https://www.youtube.com/watch?v=l1C34QmGuIA
 MILL/TURN OR TURN MILLING
• Turn milling is defined as the milling of a curved surface while rotating the workpiece around its
centre point,
• A mill/turn machine is a hybrid CNC machine that combines both milling (tool rotating) and turning
(workpiece rotating) functions,
• Can complete complex operations faster and with potentially greater accuracy than traditional machining
technologies,
• While other machines perform a single function, mill/turn machines can accomplish up to four
operations at the same time.

Representation of milling (a), turning (b) and turn-milling (c) operations

https://www.mastercam.com/news/blog/milling-turning-and-mill-turn-what-are-the-differencesmilling-turning-and-mill-turn-what-are-the-differences/
https://www.sandvik.coromant.com/en-gb/knowledge/milling/turn-milling Comak, Alptunc. (2018). MECHANICS, DYNAMICS AND STABILITY OF TURN-MILLING OPERATIONS. 10.14288/1.0368954.
THE MATHEMATICS OF METAL CUTTING I
• Speeds, feed rates and depth of cut are the three major variables that must be considered for
successful and economic machining and must be established for any metal-cutting operation.

• A number of factors need to be considered when choosing the speeds, feed rates and depth of cut:
• The work material - may be too hard, the wrong size, or even the wrong material,

• Cutting tool material - may be too soft to complete the cut,

• Cutting tool geometry - the angles on the cutting tool may be incorrect for the desired cut,

• Cutting fluid (coolant) - may not be mixed correctly, or there may be too little,

• Condition of the machine – may be old, worn or damaged so cannot achieve the sizes or surface finish
required.
 THE MATHEMATICS OF METAL CUTTING II
Speed

• Speed can refer to either cutting speed (Vc) or spindle speed (n),
• Spindle speed (n) is how fast our spindle/tool rotates and is measured in revolutions per minute (RPM),

• Cutting speed (Vc) is the tangent velocity on the cutting edge measured in meters per minute (m/min),

• Most cutting tool manufacturers supply a list of “recommended” cutting speeds for their cutting tools on a range of
materials:

Making Your CAM Journey Easier with Fusion 360 by Fabrizio Cimò
 THE MATHEMATICS OF METAL CUTTING III
Speed Equation Derivation 𝑉𝑐 = 𝑟 × 𝜔
• S m/min mm rad/s

n rev/min
Vc m/min
D mm
𝜋 3.14
𝑉𝑐 × 1000
𝑛=
𝐷 ×𝜋
Making Your CAM Journey Easier with Fusion 360 by Fabrizio Cimò
THE MATHEMATICS OF METAL CUTTING IV
Speed

• When programming a machine to cut material we typically specify the spindle speed,

• So, we need to get from cutting speed (Vc) to spindle speed (n):

Cutting Speed
n rev/min
𝑉𝑐 × 1000 Vc m/min
𝑛= D mm
𝐷 ×𝜋 𝜋 3.14
RPM
Tool Diameter
 THE MATHEMATICS OF METAL CUTTING V

Task – Calculate the spindle speed for a high alloy steel material using a 20 mm SD99-200 end mill.

ISO 513 Material Group Vc (m/min)

1 150
2 130
3 115
P
4 105
5 100
6 50
1 100

M 2 100
3 85
1 100
K
2 60

https://www.lfc.com.sg/products/detail/WIDIA-GP-Solid-Carbide-End-Mills
https://www.youtube.com/watch?v=gTnkNHB7dss
 THE MATHEMATICS OF METAL CUTTING VI

Task – Calculate the spindle speed for a high alloy steel material using a 20 mm SD99-200 end mill.
ISO 513 Material Group Vc (m/min)
1 150 𝑉𝑐 × 1000
2 130 𝑛=
P
3 115 𝐷 ×𝜋
4 105
5
6
100
50
100 × 1000
1 100 𝑛=
M 2 100
20 × 𝜋
3 85
1 100
𝑛 = 1592 𝑟𝑝𝑚
K
2 60

https://www.lfc.com.sg/products/detail/WIDIA-GP-Solid-Carbide-End-Mills
 THE MATHEMATICS OF METAL CUTTING VII
Feed

• Feed rate - how far the tool will travel in one minute (mm),

• For end mills, the feed rate can be calculated using:

𝑉𝑓 = 𝑓𝑍 × 𝑍𝑛 × 𝑛 𝑉𝑓 mm/min
𝑓𝑍 mm
Speed 𝑍𝑛 -
Feed rate Number of 𝑛 rev/min
Feed per tooth
teeth

• What is a tooth? • What is the feed per tooth?

Making Your CAM Journey Easier with Fusion 360 by Fabrizio Cimò
 THE MATHEMATICS OF METAL CUTTING VIII

Task – Calculate the finishing feed for the same material using a 20 mm SD99-200 end mill.

Tool Part D (diameter) Zn (teeth) fz (mm/tooth)

Number Roughing Finishing
SD99-030 3.0 4 0.020 0.013
SD99-060 6.0 4 0.045 0.027
SD99-090 9.0 4 0.070 0.045
SD99-120 12.0 4 0.085 0.055
SD99-160 16.0 4 0.105 0.065
SD99-200 20.0 4 0.130 0.080
SD99-220 22.0 4 0.150 0.090
SD99-250 25.0 4 0.170 0.105
*these values are for teaching and should not be taken as exact

𝑉𝑓 = 𝑓𝑍 × 𝑍𝑛 × 𝑛
https://www.youtube.com/watch?v=gTnkNHB7dss
 THE MATHEMATICS OF METAL CUTTING VIIII

Task – Calculate the finishing feed for the same material using a 20 mm SD99-200 end mill.

Tool Part D (diameter) Zn (teeth) fz (mm/tooth)

Number Roughing Finishing
SD99-030 3.0 4 0.020 0.013
SD99-060 6.0 4 0.045 0.027
SD99-090 9.0 4 0.070 0.045
SD99-120 12.0 4 0.085 0.055
SD99-160 16.0 4 0.105 0.065
SD99-200 20.0 4 0.130 0.080
SD99-220 22.0 4 0.150 0.090
SD99-250 25.0 4 0.170 0.105
*these values are for teaching and should not be taken as exact

𝑉𝑓 = 𝑓𝑍 × 𝑍𝑛 × 𝑛 = 0.08 × 4 × 1592 = 509.44 𝑚𝑚/𝑚𝑖𝑛

https://www.youtube.com/watch?v=gTnkNHB7dss
THE MATHEMATICS OF METAL CUTTING X
Depth of Cut (d)

• The depth of penetration of the cutting tool into the workpiece during cutting (millimetres),

• The depth of cut is dependent on:

• the required surface finish,

• the capacity and rigidity of both the machine tool and the workpiece,

• the horse power of the machine tool.

• Larger depth of cut - rough turning/milling,

• Smaller depth of cut - Finishing cuts,
• Higher depth of cut may break the cutting tool,
• It also influences chip thickness, type etc.
 EXAMPLES
Aerospace Mechanical

www.youtube.com/watch?v=qgd5ta-zwXU https://www.prestigemoto.com/hardcore-tech/blog/cnc-engine-block-machining-service.html
SUMMARY
Outcomes

• You should now be able to differentiate drilling, turning and milling,

• Drilling – creating holes, Turning - generating a cylindrical shapes/profiles, Milling - precisely remove
material from a solid block,

• You should understand what numerical control is and how it relates to machining or manufacturing,
• The language for programming machines and moving and completing actions,

• You should now understand the three metrics to determine how well the programme is doing,
• Accuracy, repeatability & resolution,

• You should now be aware of programming languages,

• G-Code (including G-, M-, S-, T- commands etc.)

• You should now be able to calculate speeds and feeds for a given process.

An interesting turning video: https://www.youtube.com/watch?v=se1PsJwTpiY