Making Your CAM Journey Easier with Fusion 360 E-Book

Fabrizio Cimò

• Herausgeber: Packt Publishing
• Kategorie: Fachliteratur
• Sprache: Englisch

Seitenzahl: 497

Veröffentlichungsjahr: 2023

Beschreibung

Downloading a piece of 3D software and shaping concepts and ideas is quite easy. However, designing feasible and cost-effective real parts from 3D models can be challenging with traditional production technologies, or even additive manufacturing. This book will give you the know-how and skills to develop your projects from ideas to physical products, and overcome these obstacles.
In ‘Making Your CAM Journey Easier with Fusion 360’, you'll discover how to set up a CAM program, pick the right tool, and optimize production. You'll learn the pros and cons of different production technologies, including turning, milling, laser cutting, and 3D printing, and understand how to choose the best option based on your needs. You’ll also explore the important computer-aided manufacturing tools that Fusion 360 offers through the use of examples and best practices.
By the end of this book, you’ll understand the potential issues and drawbacks of different design components and apply workarounds to avoid design flaws.

Leseprobe

Making Your CAM Journey Easier with Fusion 360

Learn the basics of turning, milling, laser cutting, and 3D printing

Fabrizio Cimò

BIRMINGHAM—MUMBAI

Making Your CAM Journey Easier with Fusion 360

Copyright © 2023 Packt Publishing

All rights reserved. No part of this book may be reproduced, stored in a retrieval system, or transmitted in any form or by any means, without the prior written permission of the publisher, except in the case of brief quotations embedded in critical articles or reviews.

Every effort has been made in the preparation of this book to ensure the accuracy of the information presented. However, the information contained in this book is sold without warranty, either express or implied. Neither the author, nor Packt Publishing or its dealers and distributors, will be held liable for any damages caused or alleged to have been caused directly or indirectly by this book.

Packt Publishing has endeavored to provide trademark information about all of the companies and products mentioned in this book by the appropriate use of capitals. However, Packt Publishing cannot guarantee the accuracy of this information.

Group Product Manager: Rohit Rajkumar

Publishing Product Manager: Vaideeshwari Muralikrishnan

Senior Editor: Hayden Edwards

Technical Editor: Joseph Aloocaran

Copy Editor: Safis Editing

Project Coordinator: Sonam Pandey

Proofreader: Safis Editing

Indexer: Tejal Daruwale Soni

Production Designer: Jyoti Chauhan

Marketing Coordinator: Nivedita Pandey

First published: March 2023

Production reference: 1170223

Published by Packt Publishing Ltd.

Livery Place

35 Livery Street

Birmingham

B3 2PB, UK.

ISBN 978-1-80461-257-6

www.packtpub.com

To my grandfather, Gaetano, 99 years old and counting; a living miracle of cleverness and goodness, and a constant source of inspiration throughout my life.

To my girlfriend, Giulia, who was the first to convince me to go back to studying engineering and achieve what remained just a dream for a long time.

To my parents, Francesca and Antonio, for having supported me on such a long and winding journey.

– Fabrizio

Contributors

About the author

Fabrizio Cimò is an Italian engineer who has always had a passion for the world of 3D graphics and design.

During his first degree in industrial design, he started uploading video lessons covering 3D modeling tools such as Rhinoceros, Blender, and Fusion 360 on his YouTube channel.

Sometime later, Autodesk noticed his work and asked him to keep promoting Fusion 360 as an official student ambassador.

During this time, he also joined Dynamis PRC, a racing team from Milano PT competing in the Formula SAE championship; thanks to this experience and his avid curiosity, he improved his knowledge of the manufacturing world.

Today, Fabrizio works as a machine designer for an important company in the laser-cutting sector.

I want to thank all my colleagues from the technical office for teaching me so much, with so much patience and passion, over all these years.

About the reviewers

J Aatish Rao is a dynamic, team-spirited mechanical engineering professional with more than 10 years of industrial experience. Certified to provide training on various software, science, and engineering-related topics, he is an Autodesk Certified Professional, Autodesk Fusion Certified User, ClearFit Certified Team Leader, and industrial consultant. Conducting workshops and engaging in teaching activities are the key ingredients of his life. He is also a keen enthusiast of stargazing.

Prashant Kumar is a graduate mechanical engineer with more than 7 years of industrial work experience. He specializes in engineering design software such as AutoCAD, SOLIDWORKS, and Fusion 360, with a good grasp of engineering subjects and principles.

Prashant currently works as a full-time freelance CAD designer, and he created a brand named 3Diest that provides engineering design and drafting services to companies and individuals across the globe. He also works as a part-time trainer for software such as AutoCAD and Fusion 360.

Nikhil Chaitanya is a mechanical engineer who completed his M.Tech in Machine Design specialization from Andhra University, Visakhapatnam, India. He has 3 years of industrial experience, with most of that time spent working at Tata Consultancy Services. He is currently working as an assistant professor in the Department of Mechanical Engineering at Vignan’s Institute of Information Technology, Visakhapatnam.

Nikhil is passionate about new product development and building the most important manufacturing infrastructure for India with his start-up venture branded as the Namoona Group. He was also nominated for the Times of Startup India’s 40 Under 40 Awards 2023 but has declined the award as he wants to encourage fellow students to become leaders of the future.

Table of Contents

Preface

Part 1 – Implementing Turning Operations in Fusion 360

1

Getting Started with Turning and Its Tools

Technical requirements

Approaching a lathe and its components

Cylindrical coordinate system

Different types of turning operations

Understanding the main parameters

Turning speed

Cutting speed

Cutting depth

Cutting feed

Cutting power

Exploring main machining strategies

Longitudinal operations

Facing operations

Plunging operations

Profiling operations

Understanding tool geometry

Tool edges

Tool surfaces

Tool angles

Summary

2

Handling Part Setup for Turning

Technical requirements

Exploring the main interface of a CAM project

Finding example projects in Fusion 360

Importing our chuck

Understanding how to set up the first part to be machined

Setup tab

Stock tab

The Post Process tab

Summary

3

Discovering the Tool Library and Custom Tools

Technical requirements

Discovering the tool library

Creating a new tool

Getting a sample tool

Creating a new tool

Importing a third-party tool library

Importing new tools with a plugin (CoroPlus)

Summary

4

Implementing Our First Turning Operation

Technical requirements

Setting up a facing operation

Using CoroPlus to calculate cutting parameters

Entering the cutting parameters into Fusion 360

Discovering tool simulation

Checking the generated G-code

Settings

Operations

Summary

5

Discovering More Turning Strategies

Technical requirements

Turning Profile (Roughing)

The Tool tab

The Geometry tab

The Passes tab

Simulation

Turning Profile (Finishing)

The Tool tab

The Geometry tab

The Passes tab

Simulation

Turning Threads

The Tool tab

The Geometry tab

The Radii tab

The Passes tab

Simulation

Drilling

The Tool tab

The Geometry tab

The Cycle tab

Turning Groove

The Tool tab

The Geometry tab

The Passes tab

Simulation

Turning Part

The Tool tab

The Geometry tab

The Radii tab

The Passes tab

Simulation

Summary

Part 2 – Milling with Fusion 360

6

Getting Started with Milling and Its Tools

Technical requirements

Understanding what milling is and how it works

Cartesian machines

Multi-axis machines

Understanding the main cutting parameters

Spindle speed and cutting speed

Cutting depths

Feed step

Cutting power and torque

Introducing the most common milling operations

Face milling

Shoulder milling

Slot milling

Profile milling

Other

Summary

7

Optimizing the Shape of Milled Parts to Avoid Design Flaws

Technical requirements

Handling undercuts and accessibility

Changing part orientation relative to the tool

Using a multi-axis machine

Creating custom tools

Backside milling

Learning how to manage mill radius

Reducing the mill radius

Tweaking our part geometry

Changing the cutting direction

Solving a very bad design

Undercut face

Missing tool radii

Counterbore holes

All around radii

Summary

8

Part Handling and Part Setup for Milling

Technical requirements

Understanding the part

Choosing part placements

Choosing a part fixture

Choosing WCS offsets

Defining the first setup

Setup tab

Stock tab

Post Process tab

Defining the second setup

Setup tab

Stock tab

Post Process

Summary

9

Implementing Our First Milling Operations

Technical requirements

Face milling

Using CoroPlus to find the best tool for face milling and shoulder milling

Implementing face milling with Fusion 360

Shoulder milling

Calculating the cutting parameters by hand

Shoulder milling inside Fusion 360

Drilling

The Tool tab

The Geometry tab

The Heights tab

The Cycle tab

Tapping

Summary

10

Machining the Second Placement

Technical requirements

Face milling

Implementing a roughing operation using adaptive clearing

The Tool tab

The Geometry tab

The Heights tab

The Passes tab

The Linking tab

Milling a hole

The Tool tab

The Geometry tab

The Heights panel

The Passes tab

Finishing the part using a morphed spiral

The Tool tab

The Geometry tab

The Heights panel

The Passes tab

Thread milling

Thread geometry

Picking the proper threading tool

Implementing thread milling in Fusion 360

Summary

Part 3 – Laser Cutting Using Fusion 360

11

Getting Started with Laser Cutting

Technical requirements

Introducing lasers

How does a laser cut?

Reviewing the pros and cons of laser cutting

Advantages of laser cutting

Drawbacks of laser cutting

Summary

12

Nesting Parts for Laser Cutting

Technical requirements

Presenting the example model

Understanding nesting optimization

Sheet format

Batch volume

Creating a nesting with Fusion 360

Manual placement

The Arrange command

The Nesting and Fabrication extension

Summary

13

Creating Our First Laser Cutting Operation

Technical requirements

Using Fusion 360 for laser cutting

Creating a new setup for laser cutting

The Setup tab

The Stock tab

The Post Process tab

Creating a new cutting tool

The Cutter tab

The Cutting data tab

Implementing our first cutting operation

The Tool tab

The Geometry tab

The Heights tab

Simulation results

Summary

Part 4 – Using Fusion 360 for Additive Manufacturing

14

Getting Started with Additive Manufacturing

Technical requirements

Introducing additive manufacturing

Exploring the pros and cons of 3D printing over conventional manufacturing processes

The pros of 3D printing

The cons of 3D printing

Comparing different 3D-printing technologies

Fused deposition modeling

Introducing stereolithography

Introducing selective laser sintering

Summary

15

Managing the Limitations of FDM Printers

Technical requirements

Printing overhang geometries

Facing overhangs (undercuts) in 3D printing

Improving our prints using support structures

Understanding bed adhesion

Understanding anisotropies of the printed part

Choosing the first layer placement and part orientation

Summary

16

Printing Our First Part

Technical requirements

Presenting the model

Creating a new printing setup

Orienting the model onto the build platform

Place parts on platform

Minimize Build Height

Automatic Orientation

Generating the support structures

Simulating the toolpath

Using the post-processor

Summary

17

Understanding Advanced Printing Settings

Technical requirements

Creating a new printing preset

Understanding general parameters

Understanding extruder parameters

Extrusion options

Extruder 1 options

Understanding shell parameters

Understanding infill parameters

Understanding print bed adhesion

Thermal expansion and shrinkage

Print bed adhesion

Understanding support material parameters

Understanding speed parameters

Speed

Acceleration

Jerk

Understanding tessellation parameters

Summary

Part 5 – Testing Our Knowledge

18

Quiz

Technical requirements

Questions

Turning (from Chapters 1 to 5)

Milling (from Chapters 6 to 10)

Laser cutting (from Chapters 11 to 13)

Additive manufacturing (from Chapters 14 to 17)

Answers

Turning

Milling

Laser cutting

Additive manufacturing

Summary

Index

Other Books You May Enjoy

Preface

This book is not simply an introduction to the CAM module of Fusion 360. Of course, we will analyze in detail all the options of the program, and by the end, we will be able to create toolpaths to use with a CNC machine, that’s for sure. However, the real value of this book is the advice and best practices that come from years of experience in the industrial design and production sectors.

If they want to, anyone can download a piece of CAD software and learn it for themselves (this is how I, and many others, learned it); however, issues such as the choice of construction technology (and the relative tools to be used), the feasibility of manufacturing a component, or the optimization of a production lot are much more difficult things to learn independently. That’s why I believe that this book is valuable for any novice designer – it will save you from all the mistakes I learned the hard way!

Who this book is for

This book is for 3D enthusiasts or mechanical designers looking to turn their design ideas into 3D models, and their 3D models into final products. Familiarity with any CAD software or Fusion 360 design module is recommended; the book will then teach you the rest.

What this book covers

In Chapter 1, Getting Started with Turning and Its Tools, we will approach turning, its machining strategies, and the complex geometry of machining tools.

In Chapter 2, Handling Part Setup for Turning, we will find out how to create a new turning setup using Fusion 360 CAM.

In Chapter 3, Discovering the Tool Library and Custom Tools, we will discuss several ways of importing new tools into the built-in tool library.Chapter 1

In Chapter 4, Implementing Our First Turning Operation, we will create a facing operation to remove a layer of material on the stock front.

In Chapter 5, Discovering More Turning Strategies, we will implement a wide variety of turning operations to machine a given component.

In Chapter 6, Getting Started with Milling and Its Tools, we will introduce milling, its underlying theory, its main cutting operations, and the tools typically used.

In Chapter 7, Optimizing the Shape of Milled Parts to Avoid Design Flaws, we will review the most typical design issues encountered on milled parts and the countermeasures to fix these problems.

In Chapter 8, Part Handling and Part Setup for Milling, we will analyze a complex part and choose its placements and machining.

In Chapter 9, Implementing Our First Milling Operations, we will create all the toolpaths to entirely machine our first stock placement.

In Chapter 10, Machining the Second Placement, we will complete our milling example by implementing advanced operations such as thread milling and 3D profiling.

In Chapter 11, Getting Started with Laser Cutting, we will approach laser cutting, reviewing how it works and its hidden complexities.

In Chapter 12, Nesting Parts for Laser Cutting, we will discuss several ways to optimize parts on metal sheets using multiple nesting tools.

In Chapter 13, Creating Our First Laser Cutting Operation, we will create a new setup and a new tool to generate a cutting toolpath to be exported to a laser machine.

In Chapter 14, Getting Started with Additive Manufacturing, we will approach 3D printing, its pros and cons, and the different technologies it’s made up of.

In Chapter 15, Managing the Limitations of FDM Printers, we will find out how to solve typical issues encountered when using an FDM printer.

In Chapter 16, Printing Our First Part, we will analyze the basic settings needed to orient our part onto a build platform and to generate a G-code program.

In Chapter 17, Understanding Advanced Printing Settings, we will analyze all the advanced settings used to fine-tune an FDM printing process and their effects on the generated toolpath.

In Chapter 18, Quiz, you will face a simple quiz to test your level of knowledge after reading the book.

To get the most out of this book

Since everything will be explained in the simplest possible way, no particular prior understanding of the manufacturing world is required. However, a bare minimum knowledge of common technical terms related to mechanical engineering, as well as some knowledge of the Fusion 360 design environment or similar CAD software, is required.

Please note that this book assumes you are reading it chronologically – for example, basic topics explained at the beginning will not be explained again later. To get the most out of this book, it is highly suggested not to jump through it.

Software covered in the book

Operating system requirements

Fusion 360 (a trial or paid subscription)

Windows or macOS

CoroPlus (a trial or paid subscription)

Windows, macOS, or a web browser

The Nesting and Fabrication extension (a trial or paid subscription)

Windows or macOS

Download the example code files

You can download the example code files for this book from GitHub at https://github.com/PacktPublishing/Making-Your-CAM-Journey-Easier-With-Fusion-360.

Download the color images

We also provide a PDF file that has color images of the screenshots and diagrams used in this book. You can download it here: https://packt.link/lh01Z.

Conventions used

There are a number of text conventions used throughout this book.

Bold: Indicates a new term, an important word, or words that you see on screen. For instance, words in menus or dialog boxes appear in bold. Here is an example: “Select Custom tools from the Tool library panel.”

Tips or important notes

Appear like this.

Get in touch

Feedback from our readers is always welcome.

General feedback: If you have questions about any aspect of this book, email us at [email protected] and mention the book title in the subject of your message.

Errata: Although we have taken every care to ensure the accuracy of our content, mistakes do happen. If you have found a mistake in this book, we would be grateful if you would report this to us. Please visit www.packtpub.com/support/errata and fill in the form.

Piracy: If you come across any illegal copies of our works in any form on the internet, we would be grateful if you would provide us with the location address or website name. Please contact us at [email protected] with a link to the material.

If you are interested in becoming an author: If there is a topic that you have expertise in and you are interested in either writing or contributing to a book, please visit authors.packtpub.com.

Share Your Thoughts

Once you’ve read Making Your CAM Journey Easier with Fusion 360, we’d love to hear your thoughts! Please click here to go straight to the Amazon review page for this book and share your feedback.

Your review is important to us and the tech community and will help us make sure we’re delivering excellent quality content.

Download a free PDF copy of this book

Thanks for purchasing this book!

Do you like to read on the go but are unable to carry your print books everywhere?

Is your eBook purchase not compatible with the device of your choice?

Don’t worry, now with every Packt book you get a DRM-free PDF version of that book at no cost.

Read anywhere, any place, on any device. Search, copy, and paste code from your favorite technical books directly into your application.

The perks don’t stop there, you can get exclusive access to discounts, newsletters, and great free content in your inbox daily

Follow these simple steps to get the benefits:

Scan the QR code or visit the link below

https://packt.link/free-ebook/9781804612576

Submit your proof of purchaseThat’s it! We’ll send your free PDF and other benefits to your email directly

Part 1 – Implementing Turning Operations in Fusion 360

In this first part, we will approach a lathe and its most common turning operations, trying to fully understand the potential and main limitations of this particular type of manufacturing process. After diving straight into turning equations and the underlying theory, we will implement a set of turning strategies to fully machine a simple part. In addition, we will cover important topics such as the tool library and custom tools.

This part includes the following chapters:

Chapter 1, Getting Started with Turning and Its ToolsChapter 2, Handling Part Setup for TurningChapter 3, Discovering the Tool Library and Custom ToolsChapter 4, Implementing Our First Turning OperationChapter 5, Discovering More Turning Strategies

1

Getting Started with Turning and Its Tools

Moving from 3D computer-aided design (CAD) models to manufactured parts may look like a giant leap difficult to overcome. In reality, it is not something to be scared of, and in the following pages of this book, we will try to explain step by step all the major challenges to overcome. In the end, you should have gained more confidence with machining and the manufacturing world in general.

In this chapter, we will approach a lathe for the first time, exploring components, terminology, and best practices without relying on prior knowledge.

The goal of this chapter is to let you familiarize yourself with the theory before approaching real case scenarios. Although you may want to start spinning your chuck immediately, a dive into basic concepts is very important; after all, behind every successfully machined part, however complex it may be, there is always the fundamental underlying theory.

We will also discuss turning, reaching a general understanding of what is possible and what is not possible with this method. This type of knowledge is fundamental to unleash turning's potential, instead of trying to copy and paste provided examples into your machining scenario.

In this chapter, we will cover the following topics:

Approaching a lathe and its componentsUnderstanding the main parametersExploring main machining strategiesUnderstanding tool geometry

Technical requirements

There are no technical requirements for this chapter; however, just in case you have tools and inserts floating around the room, you may want to collect them in order to observe them as you read.

Approaching a lathe and its components

Turning, long story short, it is a very old machining technique discovered thousands of years ago. While understanding Egyptian pottery may sound interesting to some, it is definitely out of the scope of this book, so we are going to jump right into the action!

Turning is a mechanical process where a cylindrical part is put on fast rotation, and then approached by a cutting tool that progressively removes material from it. The machine that lets us shape our part with this technique is called a lathe.

If you ask a professional CNC user, they will tell you that a lathe is a rather complex machine that consists of many components such as the saddle, the tailstock, the headstock, and so on. Don’t worry about all these intimidating words—we will approach turning in the simplest way possible. In the following screenshot, we can find a lathe stripped up to the bones:

Figure 1.1: Lathe main actors

Ultimately, there are only four actors involved in turning:

Chuck: A fast-spinning clamping device; it holds the stock to be machinedCutting tool: A special hard-metal blade that removes material from the stockMachined stock: Our part before machining is completedChip: The removed particles and filament (waste material)

If you have ever approached a working lathe, I’m sure you noticed that the material shape about to be machined—the stock—spins very fast, while the cutting tool moves quite slowly, with a lot of chips being generated and projected all over the surrounding environment.

Even if the chip is valueless, it doesn’t mean that we can pretend it doesn’t exist; if we did, it would very easily render our part and our tool valueless. Controlling chip formation is very important (not only for turning) because it has the bad habit of becoming an entangled mess (a little bit like pasta) and damages everything it comes into contact with.

There are several types of lathes on the market; some are really big and some are very complex, but at the end of the day, all of them are pretty similar to one another.

Now that we understand the main components of the lathe, we can dive just a little bit into the theory behind such an incredible machine!

Cylindrical coordinate system

In order to understand coordinates, we need to remember that we live in a 3D world. In our world, in order to specify the location of an object with exact precision, we must provide a set of three numbers (coordinates) that measure the distance from a point in space—the origin—in a given direction.

In our daily lives, we often use Cartesian coordinates; here, we have a few examples:

When working in an Excel file or when playing Battleship, in order to locate a cell, we need to know the row number and column number (2D Cartesian coordinates)If we want to give the dimensions of an object, we must provide the length, the width, and the height (3D Cartesian coordinates)

However, as mentioned, all the examples previously listed are Cartesian coordinates, where coordinates are expressed as a length along axes oriented at 90° from each other.

Orienting all the axes at 90° is generally the best approach for parts with a cubic shape, however, when it comes to lathes, a different coordinate system may be better. This is because all parts machined with a lathe have an axial symmetry, meaning that basically every part looks more or less like a cylinder. Therefore, we can use cylindrical coordinates instead.

With cylindrical coordinates, we do not express a point position with three distances; we express a position with an angle and two distances. We can see this in the following screenshot:

Figure 1.2: Cylindrical coordinates’ components

Let’s specify what the labels mean:

The red arrow is the axial direction (longitudinal), which is the rotation axis.The yellow arrow is the rotation angle ().The green arrow is the radial direction. Note that the arrow is not static; you can pretend it is a hand of a clock, where all the ticks on the dial would be a possible radial direction. There are infinite green arrows around the rotation axis, each rotated by an angle () from 0° to 360°!

With these three numbers, we already can specify with extreme precision every single point inside and outside our stock. However, it will be useful to introduce another direction.

The blue arrow is the tangential direction. It may not be so simple to understand the tangential direction, but we can just say that it is a vector that starts from the tip of a radial vector with a direction perpendicular both to the radial vector and to the axial vector.

Now that we know a bit more about cylindrical coordinates, we can start using this knowledge to differentiate between turning operations!

Different types of turning operations

To discuss the different types of turning operations, we will look at the two main families of machining:

External machiningInternal machining

Let’s take a look at these in more detail.

External machining

These operations are the most common operations performed while turning. In this type of process, the material is removed from “outside-in” along the radial direction. This basically means that the average radial coordinate of our tool will keep reducing during the operation.

In the following screenshot, we have a typical external machining operation depicted:

Figure 1.3: External machining example

Just by glancing at the figure, we should understand that the tool starts on the outside of our part where the radial coordinate is at the maximum, while machining it will progressively reduce it when moving toward the center (where the radial coordinate is 0).

Since, as we will discover, there are many different types of machining strategies, it is a bit difficult to find a strict definition for external machining; however, everything will be clearer when compared to the next machining approach.

Internal machining

These operations are different from the previous case since the material is removed “inside-out.” So, the average radial coordinate for our tool is growing during the operation:

Figure 1.4: Internal machining example

As you can see from the previous screenshot, the tool is moving inside our stock, and the cut chip may find itself stuck in the cavity since there is material all around the tool. As you can also see, the tool is still quite visible, but there are cases where we may completely lose the line of sight after a certain depth, and this is not good for beginners.

As a matter of fact, when we first approach turning, it is always a good idea to look constantly at our part while being machined since we can check the surface finish, prevent unforeseen collisions with parts of the stock or parts of the lathe, and monitor chip evacuation. For all these reasons, internal machining may be a bit trickier than external machining.

Note

As a rule of thumb, if the forming chip is somehow free to flow and falls on the ground, we are in external machining; if it can be stuck inside, we are in internal machining.

It is now time to explore something a bit more technical but really important to understand: working parameters!

Understanding the main parameters

It is now time to talk about the parameters involved in our turning operations. First of all, what is a parameter? In short, a parameter is a value or a setting that we can change.

Of course, some parameters are easier to change than others. For example, changing the axial movement speed for our tool is very simple, while on the other hand, changing the maximum cutting power may require a bigger and more powerful lathe.

Also, as we will shortly discover, some values are somehow connected to others; changing one parameter may change one or more others, so we have to optimize parameters according to our lathe specs and to the part we want to machine.

Let’s find out what the main parameters are that we have to work with.

Turning speed

The turning speed is a measure of how fast the chuck is spinning; it may be measured in radians per time unit () or in revolutions per time unit ().

As shown in the screenshot, the bent vector represents the part spinning along the longitudinal axis:

Figure 1.5: Turning-speed visualization

One revolution of our chuck corresponds to an angle () of 360° or (depending on whether it’s measured in degrees or radians). But, since is measured in revolution per time unit, we need to divide the angle by the same time unit, so that from the angle, we get angular speed ().

In short, we just need to remember this formula:

Old lathes had turning speeds that were only adjustable by manually changing the belt and pulleys, or changing the gears. Today, there are lathes that can control the rotation speed with inverters and encoders. So, depending on your lathe, the turning speed may or may not be a parameter that's easy to change.

Note

Please be careful when dealing with time units: sometimes the time unit may be seconds and sometimes minutes. As you can imagine, one revolution per minute is very different from one revolution per second, so when using any formula, please always be sure of its units!

Cutting speed

The cutting speed () is the relative speed between our cutting tool and the surface it is cutting. There is only one important thing to notice, which is that the cutting speed is highly dependent on the radial position of our tool: the bigger the diameter means the higher the cutting speed (at a constant rotation speed).

As you can see in the screenshot, we have a common rotation speed for the two tools (since the chuck rotation is always the same); however, as you may have noticed from the different arrow lengths, the tool that is machining a bigger diameter has a much higher cutting speed (vertical vector) than the tool machining a smaller diameter:

Figure 1.6: Cutting-speed visualization

Note

A vector can be defined by a magnitude and a direction. Magnitude is represented by the arrow length, while the direction is represented by the direction of the pointed tip.

Cutting speed is typically measured in meters per minute (m/min), and there is a very simple formula for calculating it:

Here, is the diameter in millimeters (mm) and is revolutions per minute (RPM).

For example, let’s imagine we have a chuck rotating at 500 RPM, and we are performing a longitudinal operation at a constant radial distance of 50 mm (basically, we are machining a stock with a diameter of 100 mm). What is the cutting speed seen by our tool? It's very simple:

Now that we have seen the cutting-speed formula, it should be now clear that when machining a shape with different radial coordinates assumed by our tool, the cutting speed will be subject to changes. Since the working diameter is not a parameter we can change (it is related to the part shape we want to machine), in order to change the cutting speed, we can only adjust the chuck RPM. That’s why most of the time, you will see bigger parts spinning slower and smaller parts spinning faster! Once the tool is almost at the rotation axis, the cutting speed will always drop to zero, independently of how fast the chuck is rotating.

Cutting depth

The cutting depth () is a parameter that gives us a measure of how much we impose an interpenetration between our tool and our part; it is measured in mm. Basically, it is related to how much of our cutting edge is engaged with the stock:

Figure 1.7: Cutting-depth visualization

As we can see, there are two tools machining the same diameter. The one on the left, however, is engaging the stock at a very small cutting depth, and therefore it removes only a thin layer of material. The tool on the right is cutting at a much bigger cutting depth and therefore it is removing a much thicker layer, and most of the cutting edge is engaged.

Please note that cutting depth is not always measured in the radial direction; sometimes, it can be measured in the axial direction. It mainly depends on the type of machining process we use (we will explain this in the Exploring main machining strategies section later in the chapter).

Higher cutting depth means more material removed and therefore faster machining, but requires more cutting power and leads to higher stress on our tool and our part. For this reason, please consider that higher cutting depths may partially bend our stock (especially if it is long and supported on one side only). Bending may lead to weird shapes with a rough finish.

Cutting feed

The cutting feed () is a parameter that measures how much our tool is advancing along the cutting direction at every revolution of our chuck, and therefore it is measured in mm per revolution (mm/rev)

Similar to cutting depth, higher feeds lead to higher machining speed at the cost of higher tool wear and higher power being required. The part finish is highly connected with feed values; as a rule of thumb, a lower feed value means higher surface quality.

In the following screenshot, we have two tools machining the same stock at the same cutting depth:

Figure 1.8: Feed visualization

However, in the first example, there is a much smaller feed step than in the second, so though they have the same turning speed, the tool on the bottom will reach the end of the stock much quicker, at the cost of higher surface roughness.

Be careful, as certain operations must be performed at a constant feed, such as threading. Threads have a constant pitch per rotation; therefore, we must set the feed to be equal to the thread pitch in such a scenario.

Note

Threading is the process of making a thread. It may be related to a male thread (such as a screw) or a female thread (such as a nut).

Adjusting the feed will also affect the chip. We can assume that a lower feed will produce a very long and entangled chip, while a higher feed will produce small particles. This is illustrated in the following screenshot:

Figure 1.9: Chip formation related to feed

We should always try to hit a sweet spot in chip thickness, width, and length. The ideal chip shape is the one in the middle of the screenshot.

Note

Chip formation is a very interesting world of its own. I don’t really want to distract you from the main topic; however, if you want to learn more about chip formation and different chip types, I suggest you take a look at this interesting link: https://www.bdeinc.com/blog/types-of-chips-formed-during-cnc-milling/.

Cutting power

The cutting power is the mechanical power required to machine our part at a given set of parameters. It is measured in kilowatts (kW).

Before setting all our parameters, we must always check whether our lathe is powerful enough to handle the machining we want to perform. This is the simple formula to remember:

Here, is the cutting power measured in kW; is the cutting speed measured in m/min; is the cutting depth measured in mm; is the feed step measured in mm/rev; and, finally, is the specific cutting force measured in MegaPascal (MPa).

As you may have noticed, there is a new value called that we haven’t seen yet. is a parameter related to material strength, tool shape, feed ratio, and cutting depth. This is a difficult parameter to evaluate, and I don’t want to bother you with complex calculations… but luckily, I don’t have to. We can simply refer to tables where equations are already sorted out by experts. Please note that this is a rough approximation of the real value, so you may want to take it with a grain of salt and have a bit of a safety margin on cutting power!

Here, we can find an example of the most common iron alloys:

Material/Feed

0.1 mm/rev

0.2 mm/rev

0.3 mm/rev

0.4 mm/rev

0.6 mm/rev

Cast iron

3200 MPa

2800 MPa

2600 MPa

2500 MPa

2300 MPa

Mild steel

3600 MPa

3100 MPa

2700 MPa

2500 MPa

2300 MPa

Medium steel

3100 MPa

2700 MPa

2600 MPa

2500 MPa

2300 MPa

Hard steel

4050 MPa

3600 MPa

3300 MPa

3000 MPa

2600 MPa

Tool steel

3200 MPa

2900 MPa

2600 MPa

2500 MPa

2400 MPa

Figure 1.10: Kc approximation for steel and iron

Using such a table is quite simple: we simply select the row according to the material we are about to machine, then we select the column with a feed similar to the one we plan to use, and the result approximates the real value.

Note

If you are intrigued by this parameter, you can find all the formulas for a precise evaluation of here: http://www.mitsubishicarbide.net/contents/mhg/enuk/html/product/technical_information/information/formula4.html.

As you can see, there is a very useful formula where we can insert our cutting parameters to get our value. If you are hungry for more formulas, there is a very good explanation about here: https://www.machiningdoctor.com/glossary/specific-cutting-force-kc-kc1/#k1c-and-mc-chart-for-material-group.

With that last equation, it is now easy to understand that all parameters are connected and that we must change them accordingly to meet the maximum cutting power available for our lathe.

You may be wondering whether it is a must to target maximum power. No, it is not, but from the production point of view, not using our machine at its full potential will cost us more money per hour. However, a typical scenario where we will not use maximum cutting power is when we are machining a fragile material that we may damage with our chuck closed at maximum force to sustain chuck torque.

Now that we have covered the main parameters, we should better understand our lathe. Next, let’s jump into something juicier: turning operations and strategies!

Exploring main machining strategies

When we plan how to machine our part out of the stock, we have to think like a chess master. What I mean by this is that we have several pieces we can play with, but in order to win the game, we have to use every component in the best possible way it can be used. Therefore, we need to plan which piece to play first and with which type of move: do we move the bishop or the queen? Do we move by one square at a time or full speed ahead?

In the following sections, we are going to discover the main moves we can play with when it comes to turning.

Longitudinal operations

Longitudinal machining is a simple and common operation strategy, suitable for rough machining with high power and strong tools. Let’s check a basic example in the following screenshot:

Figure 1.11: Longitudinal machining approach

The typical approach for longitudinal operations is to move the tool on the front of our stock (at a safe distance), set the cutting depth in the radial direction, and then move the tool forward. As we can see in the screenshot, while cutting, our tool is moving along the axial direction only, so we have a constant cutting speed per cutting pass. Once at the desired distance, the tool will disengage our stock radially and then repeat the process until the right diameter is machined.

Since this is longitudinal machining, the main cutting direction is on the longitudinal axis at a given radial distance; therefore, after a chuck rotation, our tool will be moved by one feed step along the longitudinal direction.

As a recap, in this type of machining, the cutting feed is along the axial direction, while the cutting depth is fixed and constant and is measured along the radial direction. As we are about to discover, there are other machining strategies where what we just said doesn’t apply.

Facing operations

Facing is used when we need to clean the front face of our stock:

Figure 1.12: Facing machining approach

As shown here, while cutting, our tool is moving in the radial direction only; therefore, the cutting power will keep changing unless we adjust the feed or rotation speed accordingly.

The standard approach for facing operations is to move the tool at a safe distance in the radial direction, set the cutting depth in the axial direction, and then approach the stock radially. Once at the desired position, the tool will disengage our stock axially and then repeat the process until the right length is machined.

Since in facing, we are basically cleaning a slice of our stock, we are operating at a fixed axial coordinate and our tool is moving radially. So, after a chuck rotation, our tool will be moved forward by one feed step along the radial direction.

As a recap, when facing, the cutting feed is along the radial direction while the cutting depth is along the axial direction (this is different than longitudinal operations!).

Plunging operations

Plunging is similar to facing since the tool is moving in the radial direction only; however, because plunging is used for grooving or cutting, the tool is much slimmer. That’s because circlips grooves can be very thin, and our tool needs to fit inside them. Another reason is that when cutting our part, it is not a good idea to perform a large cut because that would require a lot of material removed without a real need.

As already mentioned for facing, since radial coordinates are always changing, so does the cutting power, unless controlled by feed changes or RPM.

As shown in the following screenshot, the typical approach for plunging is to position our tool at a safe radial position, set the desired axial coordinate, and then approach the part radially:

Figure 1.13: Plunging machining approach

So, to recap this strategy, plunging is similar to facing since it has feed along the radial direction too, but the main difference is that we cannot set the cutting depth since the tool cutting edge is always engaged entirely; therefore, the cutting depth is always at the maximum possible value!

Profiling operations

Profiling is one of the most complex operations since the tool moves constantly radially and axially. Let’s check the following screenshot for an idea of how profiling works:

Figure 1.14: Profiling machining approach

As shown in the screenshot, the motion path of our tool can be very complex; therefore, this type of operation is the most flexible and is well suited for finishing our part. However, due to the fact that the cutting direction is not constant, there is always the risk of impact between the tool and our stock. As you may have noticed in the screenshot, after “climbing the first hill,” our tool will likely collide with the stock since the required path is too steep for the tool to pass.

To reduce the possibility of errors, an impact simulation is always a good idea in CAM, but for complex machining operations such as profiling, you must always check the results. Especially when a beginner is approaching turning for the first time, 99% of the time they will discover that the back of the tool or the shank will collide where the profile gets too steep or too narrow.

If we want to analyze what happens to our cutting parameters when profiling, we have to remember that the profile is not constant along the radial direction nor along the longitudinal direction; it keeps changing. So, unless our chuck is able to control rotation according to the tool’s radial position, the cutting speed will not be constant.

Having said that, we also need to remember that feed is measured along the cutting direction, so it will keep changing along the profile; the same can also be said for cutting depth.

Finally, we are at the end of yet another section. There is only one last major topic to cover: tool geometry.

Understanding tool geometry

As we discovered, there are many possible operations and geometries that we can machine on our lathe, but not every tool is suitable for every operation (always remember the chess analogy). We are now going to classify tool geometry in order to recognize, at first glance, which tool is more suitable for which machining strategy.

We can split the geometry of a cutting tool into three main categories:

Tool edgesTool surfacesTool angles

Let’s start with our deeper analysis of the geometry.

Tool edges

In the following screenshot, we can see a tool with a transparent shank where the edges are highlighted:

Figure 1.15: Main tool edges highlighted

You’ll notice that the tool shown is very crudely drawn and is simply a square. In reality, as we are going to discover, tool geometry is way more complex; however, at the moment, we will pretend it is a real tool since understanding surfaces and edges will be simpler this way.

Here are thethree edges:

The main cutting edgeThe auxiliary cutting edgeThe nose edge

Let’s take a look at them.

Cutting edge

As the name suggests, the cutting edge is a sharp edge that cuts our stock that is rotating against it. The cutting edge simply cuts along the feed direction and cuts the main portion of the chip.

Auxiliary cutting edge

In order to cut the stock, we need to cut in two directions. So, the auxiliary cutting edge cuts the side of the chip and removes the material from the stock.

Nose edge (radius)

The nose edge is not a real “edge.” It is never sharp because it wouldn’t last a single second while machining; instead, it is a “smooth edge” with a specific radius that can be bigger or smaller according to the tool we choose. A tool with a bigger nose radius will be less sharp and therefore will be able to sustain higher feed rates and higher cutting depths for a longer time.

Saying that, it is important to note that the nose radius is responsible for the surface’s finish. As you can see here, from a geometrical point of view, a higher nose radius will lead to less surface roughness when machining, and therefore to a better surface finish:

Figure 1.16: Changing the nose radius will change surface roughness

So, it looks like you may always want to use a large nose radius for roughing and for finishing… well, not so fast—there is a catch! When working at a low cutting depth (for example, when finishing a flexible part), a big nose radius will generate higher radial forces that are going to create strong vibrations (more details on that in the Entering angle (KAPR) section at the end of this chapter). Such vibrations will ruin the surface finish. A tool with a small nose radius will be super sharp and short-lasting, but also incredibly more effective at small cutting depths when finishing.

Now that we have learned something about the three main edges of every tool, let’s now start talking about the three main surfaces and their relative orientation.

Tool surfaces

All the edges listed up until now come into contact at the tip (or the nose) of the part. Three main surfaces are defined from this intersection. As always, it is way easier to understand the geometry by looking at asimple example:

Figure 1.17: The main surfaces of a tool

Here, we can see three highlighted surfaces to study:

Rake surfaceMain flankAuxiliary flank

Let’s take a look at them.

Rake surface

The rake surface is the surface generated between the main cutting edge and the auxiliary cutting edge. It is the surface our chip is rubbing against before being evacuated. As you can imagine, much of the cutting power is transmitted to the stock through the cutting edge and the rake surface. At the moment, there is not much more to say about it, but as we will shortly discover, the main point of interest is its rotation.

Tool flanks

In our tool, we have two flanks:

The main flank is generated between our cutting edge and our nose edgeThe auxiliary flank is generated between our auxiliary cutting edge and our nose edge

After that quick look at surfaces, let’s analyze angles.

Tool angles

When machining our part, we have many angles involved; some angles are related to the tool shape, while others are related to the way our tool is installed on the lathe.

Rake angle

The rake angle ( ) is the angle that describes how much our rake surface is rotated around the cutting edge. We can classify tools according to their rake angle, and we can distinguish three types of tool families: negative tools, neutral tools, and positive tools.

In the following screenshot, we can see those three tools, from left to right respectively:

Figure 1.18: Rake angle visualized

More positive values will result in a super sharp tool (with a lower life span) capable of an easy-flowing chip very suitable for a surface finish.

More negative values will result in a stronger tool with a higher life span. Since the cutting edge is not so sharp, the tool will be great for roughing passes with higher cutting depth. As you can see in the screenshot, negative rake angles impose a hard twist in the forming chip; therefore, it won’t flow so easily and will break into smaller particles that may rub against the machined surface.

There is not much to say about neutral tools—their properties are a mix between positive tools and negative tools.

Please note that there is also a less important rake angle measured from the auxiliary cutting edge:

Figure 1.19: Rake angles

In the screenshot, we can find the main rake angle on the left and the auxiliary rake angle on the right.

Relief angle

When introducing tool flanks, we missed one important thing—they should never rub or collide against our stock or our machined part.

As you can imagine, the only part of our tool that should ever rub against our stock is our cutting edge(s). In the tools seen up until now, there is actually a really large surface rubbing against the machined part. Let’s analyze the following screenshot for a better understanding of what is going on:

Figure 1.20: Friction area for a squared tool

As shown in the screenshot by the arrow, all that area is rubbing against the machined side! Not good at all! The same is true on the other flank.

To prevent this type of behavior, in real life, the two flanks are always rotated along the cutting edges by a relief angle in order to avoid friction. Every tool always has relief angles, and the angle value cannot be negative; otherwise, cutting edges would never engage the stock (because the bottom of the flank will hit the stock first):

Figure 1.21: Relief angles displayed

We can find in the previous screenshot the auxiliary relief angle (on the left) and the main relief angle (on the right). These angles avoid friction with the turning stock while machining.

Nose angle

While looking at all the tools displayed up until now, you may have noticed that the angle between our cutting edge and our auxiliary cutting edge—called the nose angle—is constantly 90°. Just in case you are wondering… more often than not, this is not true; there are many different shapes available on the market!

Let’s check the following screenshot to grasp what the nose angle is:

Figure 1.22: Nose angle visualized

Why don’t we try to analyze the tool shown in the screenshot? We should have lots of ways to analyze it. At the first glance, we should recognize that it is a positive tool (but almost neutral), that it has small relief angles on the two flanks, and as measured by the arrow, the nose angle is 60° with a small nose radius as well. Not bad!

This is a somewhat old type of tool; it has a large drawback: once the cutting edge or rake surface is really damaged, we have to throw it in the bin and buy a new tool. Today, the most typical approach is to have a tool composed of a shank and a swappable insert that can be replaced without changing the entire tool.

In the following screenshot, we can see on the left we have an “old-style” tool made in a single piece, while on the right side, we have a tool shank and a replaceable insert (both have the same cutting geometry):

Figure 1.23: Insert versus solid tool

Also, please note that most of these inserts are symmetrical, so they have multiple cutting edges; once one of them is spent, we simply rotate the same insert and keep spinning the chuck!

In the following table, you will find a few typical insert examples with different nose angles and their suggested use:

TOOL SHAPE

Name

R (Round)

S (Square)

C (Rhombic 80°)

W (Trigon)

T (Triangle)

D (Rhombic 55°)

V (Rhombic 35°)

Preview

Nose angle

0/90°

90°

80°

80°

60°

55°

35°

TOOL USAGE

Versatility

0

0

+++

++

++

+++

+

High-depth roughing

+++

+++

++

+

+

0

0

Low-depth roughing

0

+

++

+++

++

+

0

Finishing

0

0

+

++

+++

+++

+++

Profiling

0

0

0

+

++

+++

+++

Figure 1.24: Tool specifications and typical use

The table shown is divided into two sections. The first part is related to the tool shape, where we can find the seven different families, their naming convention, and their shape. The second part of the table rates tool usage from “+++” to “0” (with “++” and “+” values in the middle). Let’s reviewthe usages:

Versatility: If we were alone on a desert island with our lathe, which tool would we take with us? A higher ranking (“+++”) means that that tool is a good choice in many situations and can more or less do everything. It is a workhorse and not choosy!High-depth roughing: If we need to remove a lot of material with rough passes at high cutting depth and high power, we need a very strong tool. A higher ranking (“+++”) means that the tool is tough and long-lasting, while a lower ranking (“0”) means that the tool is super sharp and will likely break or wear immediately.Low-depth roughing: In this scenario, we still need to perform roughing passes but with a thinner cutting depth. This case is somewhere between a roughing pass (where we remove a lot of material and we don’t mind about tolerances and surface quality) and a finishing pass (where we try to get good surface quality and tight tolerances). I decided to include it just to let you note that at low cutting depth, the round shape is very bad because it causes vibrations (this will be described later in the Entering angle (KAPR) section).Finishing: If we need to finish our part, we probably need to remove a thin layer of material. A higher ranking (“+++”) means a super sharp tool suitable for a good surface result.Profiling: With this ranking, we are going to evaluate which tool is better for machining complex profiles. A higher ranking means that the tool is very good and that it is not limited by accessibility issues, while a lower ranking means that the tool may often collide with the stock. The main difference between profiling and finishing is that the profiling score also considers shape accessibility.

We just mentioned shape accessibility—what does that mean? The answer is simple: slim and sharp tools can reach areas beefier and stronger tools cannot. Let’s check the following screenshot:

Figure 1.25: Different accessibility displayed

As we notice at the first glance, the round tool (type R) cannot remove as much material as a rhombic tool (type D) because the area to be machined is too deep to reach for it.

We have just taken a look at all the angles that we can find when looking at a tool on the workshop shelf. Is this the end? Not really—despite the tool shape, we can always decide to mount it rotated! Let me introduce you to the entering angle.

Entering angle (KAPR)

The entering angle is the angle measured from the feed direction to the cutting edge.

Changing the entering angle can dramatically change tool performance and chip management. In normal circumstances, it is always a good idea to set the KAPR close to 90°. With flexible parts, we should never set an entering angle lower than 70° if possible. The reason is pretty simple: changing the angle is actually changing the way our cutting edge is transferring power to the stock material:

Figure 1.26: The same insert mounted at different KAPR angles

As shown on the left of the screenshot, when close to 90°, our tool is transferring power mainly in the longitudinal direction, and only a small percentage of the total is transferred as the radial component.

On the right, we can see that the tool is far from 90°, and therefore the radial component is much higher; this is bad, especially with flexible parts, because they will bend.

Why is bending a bad thing? Let’s review the following screenshot for a better understanding:

Figure 1.27: Bending

As you can see, the screenshot depicts a scenario where a slim part is machined with a longitudinal operation. Other than that, we can see that the tool has a 45° entering angle and a high cutting depth, which is the perfect recipe for high radial forces that will bend the part while machining.

As you can see at the top of the screenshot, the stock is heavily bent while machining, so we can imagine high vibrations due to the runout of the center rotation line and low surface quality.

As we can find at the bottom of the screenshot, after the machining is completed, what should have resulted in a nice cylindrical surface appears more like a cone with a higher diameter where the bending was more severe!

It may look like a small entering angle is forbidden, but not so fast. There are many different scenarios where we may have to use small angles; here are some examples:

When we want to improve tool life span: At the same cutting depth, with a smaller entering angle, a bigger part of our cutting edge is engaged, and therefore the cutting force will be distributed over a bigger area with smaller stress on the insert that will last longer.When we want to machine a thread: Let’s take a look at the following screenshot for a better understanding of this example:

Figure 1.28: Threading operation displayed

As shown in the previous screenshot, when threading we must use an entering angle and a nose angle strictly dictated from the thread specs: 60° as KAPR and 60° as the nose angle (for most metric threads); that’s why the triangle insert is very often used for threading.

As we already mentioned, remember that when threading, many parameters are locked to thread specs: from the thread pitch, we must impose a certain feed step, and from the thread angle, we must use a tool with a specific nose angle, entering angle, and maximum nose radius. Do not underestimate the nose radius when threading: if it’s too large (over thread specs), the nut will not be able to be screwed on.

So, when threading, if we need to reduce vibrations or bending, there is only one parameter left… we can change the cutting depth only.

As a bonus point, let’s explain why the round tool shape can be a good choice at high cutting depth but may generate high vibrations at low cutting depth. Let’s analyze the following screenshot:

Figure 1.29: Round-tool KAPR

As you can see, the tool on the left is cutting at a high cutting depth; therefore, it is exchanging all the cutting force on a wide range of angles, from almost 90° to 0°, so the radial force generated is not a main issue. On the other hand, the tool on the right is engaging a thin layer only, and the cutting force is shared from almost 0° to 0°. Such a small KAPR will create massive vibrations—that’s why round tools are good for high-depth machining but not so much for low depths (and the same can be said for the nose radius).

When facing, a round tool may become handy even at low cutting depth since we don’t care that much if the force is transferred to the chuck!