Autodesk Inventor 2023 Cookbook E-Book

Alexander Bordino

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

Seitenzahl: 459

Veröffentlichungsjahr: 2022

Beschreibung

Autodesk Inventor is an industry-leading, computer-aided design application for 3D mechanical design, simulation, visualization, and documentation. This book will help to bridge the gap between the fundamentals of this software and the more advanced features, workflows, and environments it has to offer.
Using cookbook-style recipes, you’ll gain a comprehensive understanding and practical experience in creating dynamic 3D parts, assemblies, and complete designs. You’ll also explore a variety of topics, including automation and parametric techniques, collaboration tools, creating sheet metal designs, and design accelerators such as frame generators. As you progress, the chapters will guide you through surface modeling tools, advanced assembly, and simplification tools, along with covering iLogic, Finite Element Analysis, and more.
By the end of this book, you’ll not only be able to use the advanced functionality within Autodesk Inventor but also have the practical experience you need to deploy specific techniques in your own projects and workflows.

Leseprobe

Autodesk Inventor 2023 Cookbook

A guide to gaining advanced modeling and automation skills for design engineers through actionable recipes

Alexander Bordino

BIRMINGHAM—MUMBAI

Autodesk Inventor 2023 Cookbook

Copyright © 2022 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.

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First published: November 2022

Production reference: 1211122

Published by Packt Publishing Ltd.

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ISBN 978-1-80181-050-0

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To my wonderful wife, Nav, for her love, support, and patience, without which writing this book would not be possible.

For Nonno B.

– Alexander Bordino

Contributors

About the author

Alexander Bordino is an award-winning product design engineer and Autodesk manufacturing technical specialist who specializes in consulting and training across the breadth of the Autodesk design and manufacturing portfolio. He has experience as an Autodesk Inventor Certified Professional, Autodesk Accredited Trainer, Accredited Stratasys FDM, and Polyjet Additive Manufacturing Trainer, and he attained a BSc (Hons) in product design at Nottingham Trent University. He currently works for a leading Autodesk reseller in the UK, specializing in Autodesk design and manufacturing products, empowering design and engineering companies in the UK to design products better, faster, and more efficiently. He has extensive experience of developing innovative product designs for a wide variety of organizations, obtaining industry awards, and patenting technology in his career. In 2017, Alexander was admitted as an Associate of the Worshipful Company of Horners, an ancient guild and livery company in the City of London, representing and supporting the UK plastics industry.

This book would not have been completed were it not for the support and love of my wife, family, and friends. I thank you all for your encouragement throughout. Thank you also to the Packt team, who have made the process of writing a book seamless and efficient. I thank you for your professionalism and valued suggestions throughout this journey. My thanks also go to the fantastic GrabCAD community, where many of the practice files in this book originated or have been inspired by.

About the reviewers

Didi Widya Utama has extensive expertise teaching CAD/CAM/CAE in the mechanical design and robotics fields and is an assistant professor of mechanical engineering at Universitas Tarumanagara, Indonesia. Additionally, he has years of expertise in the industrial sector, including manufacturing, CNC, mold and die making, and more. He is a gold-level Autodesk® Certified Instructor, an Autodesk® Certified Professional for Inventor, Autodesk Certified Professional in Design for Manufacturing, and a Certified Fusion 360® User. He has more than 10 years of experience teaching at the Autodesk® Authorized Training Center on the Autodesk software, including Autocad®, Inventor®, and Fusion 360®, for both the manufacturing industry and educational institutions. He has been involved in several engineering projects for years, including university research, government funding, and projects involving national and international engineering collaboration.

This book, titled Inventor Cookbook 2023, covers all aspects of the Autodesk® Inventor software, from the fundamentals to in-depth expertise. Additionally, the examples in the book are relevant and valuable, and they include additional tips for using the program. This book is excellent for beginners who want to learn about the Inventor software from scratch and more experienced readers who want to refresh their knowledge on the subject. This book can serve as a guide cookbook for those looking to develop and expand their software expertise.

Olanrewaju Sulaimon was born and raised in Lagos, Nigeria. He attended Yaba College of Technology, where he studied mechanical engineering for 2 years. It was during his internship he became interested in CAD in 2017. He is currently studying the same course at the University of Lagos, Nigeria. During a semester break, he started learning how to use Autodesk Inventor as it was one of the courses in the next semester. He found Inventor very interesting and fascinating due to its instant ability to convert from 2D sketches to 3D parts, then to assemblies. He has used Inventor to design several realistic projects that were later manufactured. He is very conversant with other CAD applications, such as Autodesk AutoCAD and SolidWorks.

Table of Contents

Preface

1

Inventor Part Modeling – Sketch, Work Features, and Best Practices

Technical requirements

Downloading your practice files

2D sketch design – Best practices

Start at the origin

Use sketch constraints often

Keep sketches simple

Use keyboard shortcut commands

Always fully constrain sketches

Create manageable steps

Never draw the same thing twice

2D sketch constraints – Best practices

Use the Status bar

Automatic geometric constraints

Degrees of freedom

Types of sketch constraint

Work planes – Best practices

Work axes – Best practices

Work points – Best practices

Applying best sketch and work plane practices to model a part

Getting ready

How to do it…

2

Advanced Design Methodologies and Strategies

Technical requirements

Understanding the different design processes

Bottom-up design

Multi-body design

Layout design

Adaptive modeling design

Creating a multi-body part design

Getting ready

How to do it…

Creating a layout design from imported .dwg CAD data

Getting ready

How to do it…

Applying and using adaptive modeling

Getting ready

How to do it…

Model credits

3

Driving Automation and Parametric Modeling in Inventor

Technical requirements

Reviewing equations and parameters in Inventor

Creating equations and driving a model

Getting ready

How to do it…

Creating parameters and driving a model

Getting ready

How to do it…

Reusing design feature data with iFeatures

Getting ready

How to do it…

Creating automatic mates using iMates

Getting ready

How to do it…

Creating table-driven master parts to configure sizes and states with iParts

Getting ready

How to do it…

Building an assembly of iParts with variations such as different sizes, shapes, and content using iAssemblies

Getting ready

How to do it…

Model credits

4

Freeform, Surface Modeling, and Analysis

Technical requirements

Creating area lofts

Getting ready

How to do it…

Creating path and guide rail sweeps

Getting ready

How to do it…

Creating solid geometry from basic extruded and lofted surfaces

Getting ready

How to do it…

Creating 3D Sketches for Surfacing and applying the Trim, Combine, Thicken, and Ruled Surface commands

Getting ready

How to do it

Learning how to trim, patch, and convert surfaces to solids with Sculpt

Getting ready

How to do it…

Replacing a solid face with a surface

Getting ready

How to do it…

Using the Copy Object command to create a matching contoured part to another part

Getting ready

How to do it…

Importing surfaces into Inventor

Getting ready

How to do it…

There’s more

Validating surface designs with Zebra Analysis, Surface Analysis, and Curvature Analysis

Getting ready

How to do it…

Understanding the basic features and techniques of freeform modeling

Getting ready

How to do it…

Freeform modeling within the context of existing geometry

Getting ready

How to do it…

Model credits

5

Advanced CAD Management and Collaboration – Project Files, Templates, and Custom Properties

Technical requirements

Creating and managing an Inventor .ipj project file

Getting ready

How to do it…

Managing the Content Center

Getting ready

How to do it…

Style and Standard Editor – creating and editing templates

Getting ready

How to do it…

Collaborating with shared views

Getting ready

How to do it…

Collaborating and sharing designs with Pack and Go

Getting ready

How to do it…

Model credits

6

Inventor Assembly Fundamentals – Constraints, Joints, and BOMS

Technical requirements

Constraining components in assemblies – the best practices

Getting ready

How to do it…

Applying Joints in assemblies

Getting ready

How to do it…

Applying and driving Motion constraints

Getting ready

How to do it…

Duplicating and replacing components in an assembly

Getting ready

How to do it…

Creating and configuring a BOM

Getting ready

How to do it…

Detailing and customizing a BOM in a drawing file

Getting ready

How to do it…

Model credits

7

Model and Assembly Simplification with Simplify, Derive, and Model States

Technical requirements

Simplifying assemblies

Getting ready

How to do it…

Deriving components

Getting ready

How to do it…

Creating model states in parts

Getting ready

How to do it…

Creating model states in assemblies

Getting ready

How to do it…

Using model states in drawings

Getting ready

How to do it…

Model credits

8

Design Accelerators – Specialized Inventor Tool Sets for Frames, Shafts, and Bolted Connections

Technical requirements

Creating frames using the Frame Generator environment

Getting ready

How to do it…

Detailing the BOM for frames in the drawing environment and producing cut lists

Getting ready

How to do it…

Structural Shape Author – creating your own custom frame members and publishing these to the Content Center

Getting ready

How to do it…

Creating gears in Inventor with the Spur Gear Design Accelerator

Getting ready

How to do it…

Creating shafts in Inventor with the Shaft Component Generator tool

Getting ready

How to do it…

Applying automatic bolted connections

Getting ready

How to do it…

Model credits

9

Design Communication – Inventor Studio, Animation, Rendering, and Presentation Files

Technical requirements

Creating an image render with Inventor Studio

Getting ready

How to do it…

Animating components of an assembly in Inventor

Getting ready

How to do it…

Presentation files – creating exploded views and animations of assemblies

Getting ready

How to do it…

Creating and adding decals and custom materials

Getting ready

How to do it…

Model credits

10

Inventor iLogic Fundamentals — Creating Process Automation and Configurations

Technical requirements

Understanding the fundamentals and usage of iLogic

Getting ready

How to do it…

Creating a configurable part with iLogic rules

Getting ready

How to do it…

Creating a configurable assembly with iLogic

Getting ready

How to do it…

Creating an iLogic form and Event Triggers

Getting ready

How to do it…

Model credits

11

Inventor Stress and Simulation – Workflow and Techniques

Technical requirements

Introduction to the Stress Analysis Environment – how to conduct a simple analysis study, workflow, and interface

Getting ready

How to do it...

Performing stress analysis on bolted connections

Getting ready

How to do it...

Calculating wind loads and using midsurfaces

Getting ready

How to do it...

Calculating weld sizes using stress analysis and the Weld Calculator

Getting ready

How to do it...

Model credits

12

Sheet Metal Design – Comprehensive Methodologies to Create Sheet Metal Products

Technical requirements

Setting up and configuring your sheet metal template

Getting ready

How to do it…

Creating a sheet metal part with faces, flanges, bends, hems, and cuts

Getting ready

How to do it…

Applying advanced sheet metal base features – Contour Flange, Lofted Flange, and Contour Roll

Getting ready

How to do it…

Converting a solid into a sheet metal part and performing a rip

Getting ready

How to do it…

Creating and applying a custom sheet metal punch

Getting ready

How to do it…

Designing sheet metal parts in assemblies and .dxf output

Getting ready

How to do it…

Detailing sheet metal parts in the drawing environment

Getting ready

How to do it…

Model credits

13

Inventor Professional 2023 – What’s New?

Technical requirements

General enhancements to Inventor 2023

New Home screen: Home replaces My Home

GPU Ray Tracing display

iLogic

Improved Free Orbit

[Primary] replaces Master in model states

The Alt + Q new keyboard shortcut for Annotate

Performance enhancements and Express Mode

Interoperability between Fusion 360, Revit, and more

Fusion 360 tools

Data exchange and interoperability enhancements for Revit and Inventor

Sketch enhancements

Fixing broken projected geometry

Model sketching and the annotating text enhancement

The new link sketch format for sketch blocks

Part enhancements

Sheet metal extended browser information

The Sheet Metal Template option

New Sheet Metal Mark command for engraving/etching features

3D annotation Datum Target command added

Tolerance feature enhancements

Data reference frame label selection

Multiple selections for 3D annotation leaders

Tolerance and parameter updates to model states

Tolerance type options in Parameters

Multi-Value sort order in Parameters

Fillet tolerance

The Relationships command for suppressed features

Assembly and presentation enhancements

BOM setting updates

Changes to substitute model states

New options for Simplify

Constraint workflow command change

Drawing enhancements

Detail View drawing enhancement

Model state name within drawing labels

Remove existing sheets from new drawings

Model credits

Index

Other Books You May Enjoy

Preface

Autodesk Inventor is an industry-leading, computer-aided design (CAD) application for 3D mechanical design, simulation, visualization, and documentation. In this book, we aim to bridge the gap between the fundamentals of this software and the more advanced features, workflows, and environments this powerful design solution has to offer.

Using cookbook-style recipes, you will gain a comprehensive understanding and practical experience in creating dynamic 3D parts, assemblies, and complete designs. We will also explore a variety of topics, including automation and parametric techniques, collaboration tools, creating sheet metal designs, design accelerators such as frame generators, surface modeling tools, advanced assembly, and simplification tools, iLogic, and finite element analysis.

By the end of this book, you will not only be able to use the advanced functionality within Autodesk Inventor, but you will also have the practical experience to deploy these techniques in your own projects and workflows.

Who this book is for

This book is aimed at CAD engineers, mechanical/design engineers, and product designers who have a basic understanding and experience of Inventor fundamentals. It aims to guide and coach you beyond the basics and into the advanced functionality of the software and environments within it.

What this book covers

Chapter 1, Inventor Part Modeling – Sketch, Work Features, and Best Practices, explains the best practices involved in part modeling with the uses of sketches and all the work features covered. Then combine your knowledge of these best practices to complete a modeling challenge of a complex part.

Chapter 2, Advanced Design Methodologies and Strategies, discusses how and when to apply different design methodologies and strategies in Inventor, and the merits of each. You will learn and gain experience with practical examples of how each can be used. This chapter will also cover how to utilize external and non-native CAD data in Inventor.

Chapter 3, Driving Automation and Parametric Modeling in Inventor, discusses how to implement levels of automation into both parts and assemblies, by understanding the importance and use of equations and parameters to drive configurations. You can copy features across parts with iFeatures, automate the mating of parts with iMates, and create configurations using iParts and iAssemblies. Finally, you will learn how to link external spreadsheets and parameters to drive models in Inventor.

Chapter 4, Freeform, Surface Modeling, and Analysis, explains how to create surface geometry in various forms and how to use the freeform modeling tools within Inventor to create organic and complex forms. The chapter will break down the various ways surfaces can be created within Inventor. You will also learn about surface validation techniques and how to surface model in the context of an assembly.

Chapter 5, Advanced CAD Management and Collaboration – Project Files, Templates, and Custom Properties, focuses on some of the important admin that’s required to deliver successful projects with Inventor. It explains how to manage project files and best practices, how to set up templates and design standards for a company in both parts, assembly and the drawing environment, and how to manage content center libraries. In most cases, these areas are overlooked, but successful data management and organization are essential to delivering projects, on time and within budget. Engineering managers and CAD managers will find this topic of use most of all.

Chapter 6, Inventor Assembly Fundamentals – Constraints, Joints, and BOMS, discusses the fundamentals of successful assembly design and techniques. It will also cover how to effectively use constraints and joints in an assembly and the best practices, and how to use, edit, and customize BOMs in Inventor, including placement in the drawing environment and annotating a GA.

Chapter 7, Model and Assembly Simplification with Simplify, Derive, and Model States, covers techniques for simplifying geometry in a part and assembly to aid in the management of largeassemblies and assist in the collaboration of models with external suppliers, customers, and stakeholders. Particular focus will be spent on model states, which were released in 2022 and superseded the traditional level of detail and positional representations of older releases.

Chapter 8, Design Accelerators – Specialised Inventor Tool Sets for Frames, Shafts, and Bolted Connections, explains how to use design accelerators for a range of product types, and how to create frameworks, gears, shafts, and bolted connections within the assembly environment. This is a key skill set in Inventor that allows for automation and extreme efficiency with workflows. The conventional means of creating these types of products or adding them to existing assemblies is very time-consuming. Engineers and designers will greatly appreciate the value that using the design accelerators provides when the situation demands it.

Chapter 9, Design Communication – Inventor Studio, Animation, Rendering, and Presentation Files, explains that successful design is usually measured on how well the benefits and the solution are understood by stakeholders; therefore, being able to demonstrate these in 3D within Inventor is highly important. Designers need to be able to render, animate, and sometimes quickly annotate parts and assemblies to communicate key design changes, updates, and showcase product features. This chapter focuses on how a designer can implement renderings, explode views with presentation files, and create animations. This chapter also focuses on some of the more basic skills of model manipulation.

Chapter 10, Inventor iLogic Fundamentals – Creating Process Automation and Configurations, gives a basic introduction to automation with iLogic and what can be achieved with this. It provides an overview of the environment and practical examples of iLogic in use. You will then progress and create several iLogic rules and use these, before finally creating an iLogic form, controlling the configuration of an assembly. This is a key chapter for enabling you to automate functions, model updates, and changes within the software.

Chapter 11, Inventor Stress and Simulation – Workflow and Techniques, gives an introduction to the stress analysis environment in Inventor, how this works, what is achievable with the standard stress analysis, and workflows to adopt and various types of analysis. It also discusses design and how important it is that designers are able to test and validate their designs, prior to manufacture. Having a basic understanding of the essentials of FEA within Inventor gives the designer the key advantage of being able to iterate and test designers quicker and more efficiently, instead of having to rely on external stress analysis engineers all of the time.

Chapter 12, Sheet Metal Design – Comprehensive Methodologies to Create Sheet Metal Products, provides an introduction to the sheet metal environment within Inventor and a detailed walk-through of the functionality and methods you can use to create sheet metal features. This chapter will also show how you can bring final sheet metal parts into the drawing environment to add detail with bend tables, hole tables, and folded and unfolded flat patterns for export.

Chapter 13, Inventor Professional 2023 – What’s New?, talks about what’s new in Inventor 2023. You will learn all of the new features and additions to Inventor Professional 2023 in both the part, assembly, and drawing environments.

To get the most out of this book

This book is aimed at advanced users of Autodesk Inventor Professional. It is recommended that you have taken part in an essentials training course at an Autodesk Authorised Training Center or a similar course before proceeding, or that you have sufficient experience with the basic fundamentals of Autodesk Inventor.

You will need a working and licensed copy of Autodesk Inventor Professional 2023 to complete the recipes in this book, and a Windows 10 operating system. Post-2023 versions of Inventor will work with the recipe practice files. Internet access will be required for the initial download of recipe files for this book.

Autodesk Inventor 2023 System Requirements: https://knowledge.autodesk.com/support/inventor/learn-explore/caas/sfdcarticles/sfdcarticles/System-requirements-for-Autodesk-Inventor-2023.html

Download the example code files

You can download the Inventor lesson files for this book from https://packt.link/w6Kik

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/tnAxK.

Conventions used

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

Code in text: Indicates code words in text, database table names, folder names, filenames, file extensions, pathnames, dummy URLs, user input, and Twitter handles. Here is an example: “To begin this recipe, you will need to create a New Standard (mm) Assembly .iam file and have it open.”

A block of code is set as follows:

Parameter("CATL-SIDE PLATE #1:1", "CATH")=CATLL Parameter("CATL-SIDE PLATE #1:1", "AMOUNTR")=Ceil((Parameter("CATL-SIDE PLATE #1:1", "CATH")+32.5)/275) Parameter("CATL-SIDE PLATE #1:1", "SPACINGR")=Parameter("CATL-SIDE PLATE #1:1", "CATH")/Parameter("CATL-SIDE PLATE #1:1", "AMOUNTR")

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 Finish Sketch and then repeat this operation on the other side.”

Tips or Important Notes

Appear like this.

Sections

In this book, you will find several headings that appear frequently (Getting ready, How to do it..., How it works..., There’s more..., and See also).

To give clear instructions on how to complete a recipe, use these sections as follows:

Getting ready

This section tells you what to expect in the recipe and describes how to set up any software or preliminary settings required for the recipe.

How to do it…

This section contains the steps required to follow the recipe.

How it works…

This section usually consists of a detailed explanation of what happened in the previous section.

There’s more…

This section consists of additional information about the recipe in order to make you more knowledgeable about the recipe.

See also

This section provides helpful links to other useful information for the recipe.

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.

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1

Inventor Part Modeling – Sketch, Work Features, and Best Practices

Sketches and constraints are one of the most important aspects of your Inventor model. A good and well-defined sketch is of paramount importance in ensuring that your model is stable and can be easily edited with design updates or changes with equations and parameters.

A sketch, or your model in this instance, is very much like the skeleton of an organism; if the sketch is not strong, lacks clear definitions, or is overly complex, the rest of the body has issues and problems. You should already have a reasonably good understanding of the basics of sketch geometry in Inventor and already know the fundamentals, but as they are so critical to successful CAD design, it is always worth revisiting and refining these core skills.

In this chapter, before expanding into the practical recipes, you will learn the best practices for applying successful sketches to your models, and additional tips that will complement your existing fundamental knowledge and application of these tools. This chapter then explores the roles of planes, axes, and points (collectively known as work features) in the sketch environment, and the best practices for these. Finally, we will explore essential feature modeling tools, and combine this knowledge in a part modeling recipe.

Here are the learning objectives for this chapter:

2D sketch design – Best practices2D sketch constraints – Best practicesWork planes – Best practicesWork axes – Best practicesWork points – Best practicesApplying best sketch and work plane practices to model a part

Technical requirements

To complete the recipes, you will require Autodesk Inventor 2023, or a newer version installed on your machine. The recipe files are not backward compatible and will not work with software versions older than the 2023 version. To download and use the practice files that are required to complete the learning objective, type the following address into your internet browser: https://packt.link/w6Kik

Downloading your practice files

To make the most of the downloaded practice files’ .zip folder, you will have to set the Inventor project file up correctly for the practice files. This enables Inventor to quickly access the location of your practice files from your C drive.

To set up the project, follow these steps:

Go to your PC Downloads folder, and copy the zipped folder titled Inventor Cookbook 2023 Practice Files. This is the data you have just downloaded.Paste the zipped folder into Windows (C:). Then, right-click on the folder, select Unzip, and the files will unzip into a folder of the same name.Now, start Inventor. From the Home screen, in the top right, select Settings, as shown in Figure 1.1:

Figure 1.1: Browsing the project file

Then, in the Projects dialog box, select Browse from the bottom of the menu:

Figure 1.2: Browse selected in the Projects dialog box

From here, navigate to the unzipped Inventor Cookbook 2023 Practice Files folder and select it. Within the folder, select the Inventor Cookbook 2023.ipj file.Select Open, followed by Done. This will now ensure that Inventor is using the correct project file for the Inventor Cookbook 2023 practice files.You can check this by navigating back to Home and hovering the cursor over the active project. The full name of the project will display underneath this, as shown in Figure 1.3:

Figure 1.3: Inventor Cookbook 2023.ipj project file successfully loaded

More information regarding managing project files will be provided in Chapter 5, Advanced CAD Management and Collaboration – Project Files, Templates, and Custom Properties.

For now, you are all set to begin!

2D sketch design – Best practices

Successful sketch design underpins the entire design. It is the foundation of nearly everything you do in CAD, so reviewing best practices and techniques, even at an advanced level, is worthwhile. We will now begin to focus on some of the important theory behind this before embarking on the recipes.

Here are the best practices you should follow when creating sketches in Inventor.

Start at the origin

Start your initial sketch from the origin or, if not possible, create a dimension from one sketch entity to the origin. In any new Inventor file, the only point of reference that is known to Inventor is the origin. By creating your sketch using the origin, you will need to give Inventor less information about your sketch, as it is already working from a known point in time and space.

In Figure 1.4, two identical sketches are shown. The right sketch was defined from the origin, while the left was dimensioned to the origin:

Figure 1.4: Two identical sketches – the right was created using the origin, while the left was dimensioned to the origin

You can see from here that more dimensions have been added to the left sketch than the right. Both are correct, but the right rectangle has been created in a much more efficient manner with fewer variables. This may seem simple, but with more complex sketches, utilizing the origin becomes of greater significance.

Use sketch constraints often

Effective use of sketch constraint tools allows you to build logic and information about the sketch that dimensions alone cannot provide. If you can fix lines as being horizontal, parallel, or coincident, you will define your sketches much quicker and more efficiently than with just the use of dimension. It also makes editing sketches easier, as there are usually fewer variables to change.

Keep sketches simple

The simpler the sketch, the better. A sketch should be minimal and only contain what is necessary for your next feature command to use. Too often, CAD users will overcomplicate sketches by trying to create complex end features with sketch lines, arcs, and circles. This is not necessary, as it is the feature commands that will do the work and translate the design into something meaningful in 3D.

Before a sketch is created, you should break down what features you will use, two or three steps ahead in your design process, to create the desired outcome. There is no need to put all the information for your complex part in one sketch; be sure to break it down into manageable segments. This makes the modeling process more organized and efficient.

Use keyboard shortcut commands

Much like in Autodesk AutoCAD, the same quick keyboard shortcuts can be used in Autodesk Inventor, such as L for line, C for circle, and so on. The spacebar will repeat your last used command, and the Esc key will exit it.

As shown in the following figure, the Tab key allows you to flip between what type of dimension to enter when using a sketch command:

Figure 1.5: Graphics window when creating a sketch line; pressing the Tab key allows the user to navigate between length and angle

In this instance, a Line command is demonstrated. Pressing the Tab key at this stage allows the user to quickly flip between entering a length or angle. The Tab key will also lock the dimension value after the value has been added, and then you can switch to another dimension and repeat the process.

All of these shortcuts will save valuable time and clicks. The full list of Autodesk Inventor keyboard shortcuts can be found here: https://damassets.autodesk.net/content/dam/autodesk/www/campaigns/inventor-resource/Inventor-Keyboard-Shortcuts-Guide.pdf.

Always fully constrain sketches

Leaving unconstrained geometry in an Inventor sketch is not a good idea. Later in the design process when you have edits to make to a model or feature, you will find your model will update and change shape in a completely random fashion. This is because elements of the sketch at the model’s foundation are undefined, unfixed, and unknown. As you add dimensions and constraints to a sketch, the sketch entities will become defined.

You can tell whether a sketch is fully defined by the color of the sketch lines. By default, in Inventor, unconstrained geometry is black, green, or purple, and constrained geometry is dark blue. In a sketch itself, if you grab an entity and try and move it, a fully constrained sketch will remain in position. Spend time defining sketches, as it pays dividends later in the design process. Always apply geometric constraints before dimensional, as this will prevent your initial sketch from distorting.

You can also use the Auto Dimension tool. This will calculate the dimensions required to fully constrain your sketch and will add its own if you select this. Be warned, however, as this will apply dimensions in a random way; if you need a couple of dimensions to fully constrain a sketch, it’s worth using Auto Dimension, seeing what dimensions are placed, and then deleting these and adding your own in place. It is not advisable to draw out a whole sketch without dimensions and then default to hitting Auto Dimension.

Create manageable steps

It is tempting to try and get all the model information in one sketch, but this can often cause unnecessary complications and take more time. It is far better to break down the geometry and sketches into manageable sections and let your feature commands do the work. Keep your sketches basic and simple. This also makes future edits much easier to complete, as your Model browser and feature history will become more organized.

Never draw the same thing twice

Always look for lines of symmetry in your design; it is more economical and efficient to draw half of something and then use a Mirror or Pattern command to duplicate it. If you have already drawn a feature that is to be repeated in the design, use Copy or a Pattern/Array tool. This again helps build adaptivity in your sketches. If an element of a repeating pattern must be changed, the other elements will also change and update. Your aim should be to maximize efficiency and productivity at every opportunity!

Those are the best overall practices for a successful sketch design; applying these techniques correctly will have you creating sketches quickly and efficiently as part of your workflow. Sketch constraints are an important aspect of this, and we will now cover the best practices of these.

2D sketch constraints – Best practices

Mastering constraints within a sketch is a common area in which new and experienced users can struggle. Just knowing what each constraint function does and how they can be applied can be challenging enough, and there is also confusion in that constraints can be found in both the 2D sketch and 3D model environments within Inventor. In this section, we will primarily be focusing on 2D sketch constraints in relation to the best practices to follow:

A 2D sketch constraint constrains sketch geometry in one single sketch plane and, along with applied dimensions, allows you to quantify and fully define the geometryA 3D assembly constraint does much the same, only this is used to constrain a 3D part within the context of an assembly

Here are the best practices for working with constraints in Inventor.

Use the Status bar

The Status bar at the bottom right of the graphics window indicates the number of dimensions required to fully constrain a sketch. This will only start to show data once a sketch is created and you are in the sketch environment. In the following example, a simple rectangle was drawn in the sketch environment:

Figure 1.6: Status bar communicating how many dimensions are required for an unconstrained rectangle

Your goal should be that once you create a sketch, you want to get the dimensions needed down to 0 to ensure that the sketch is fully defined and constrained. As you apply constraints and dimensions, you should see this number reduce. If you are struggling to define a specific sketch, it can be a good indicator as to what you need to achieve a full sketch definition.

Automatic geometric constraints

Geometric constraints are created automatically, through the creation of lines, arcs, and other geometry, as you sketch in the sketch environment. These geometric constraints allow the sketch to be edited with predictable results, and they can also act as guides for aligning geometry and further defining your sketch. As automatic geometric constraints are applied, you will notice that, in the graphics window, alongside your sketch, graphical representations of the sketch will appear, giving you notice of what constraints Inventor has applied for you.

These can of course be manually deleted, and the automatic constraints can be turned off if required, but in most cases, they are useful, as they will limit the required dimensions the user has to input.

In the following figure, you can see that Inventor automatically inferred a tangential constraint between the line and arc as it was drawn, and applied a parallel constraint to the horizontal line. The visual sketch relationships can also be dragged and moved through the workspace if required:

Figure 1.7: Automatically inferred sketch constraint between a line and arc

To access the Constraint settings (including turning off this feature), turn off Constraint Inference; within a 2D sketch, navigate to the Sketch tab, and along the right-hand side of the ribbon, look in the Constrain tools, where you will find the Constraint settings, shown in Figure 1.8.

Figure 1.8: Location of the Constraint settings in the ribbon

Tip – Keyboard shortcut

Within a sketch, you can quickly cycle between showing or hiding the graphical representation of the sketch constraints with the F8 and F9 keys.

Degrees of freedom

When sketch geometry can change size and shape, this is known as degrees of freedom. An example would be that a circle has two degrees of freedom: its center and its radius. Clearly defining both will result in a fully constrained circle sketch.

To display degrees of freedom, with no command active, highlight your sketch geometry, right-click, and select Display Degrees of Freedom:

Figure 1.9: Display Degrees of Freedom in a sketch

Make sure to use Display Degrees of Freedom in your sketch, as this will notify you, as the user, where you may need to apply additional geometric or dimensional sketches to achieve a fully defined sketch. Your goal with constraints in sketches should be to eliminate the degrees of freedom.

Types of sketch constraint

Having knowledge of what each constraint does and how they can be applied is crucial to successful and efficient sketch design. Quite often, users can get confused about what each constraint means, particularly because some of the graphical representations look quite similar. This summary provides a list of each constraint and what they do, with the corresponding sketch constraint image for ease of reference.

You can locate the sketch constraints in the Sketch tab, then Constrain:

Figure 1.10: Location and graphical representation of all Inventor sketch constraints in the ribbon

Figure 1.11 gives a breakdown of all the sketch constraints in Inventor and how they are used:

Figure 1.11: Sketch constraints and examples in Inventor

A clear understanding of the constraint options will enable you to create stronger sketches that are more easily defined and can be updated quicker and more efficiently, without causing your sketch to distort when dimensions are changed.

Sketch constraints are important, but a key understanding of planes and their best practices is also necessary to create models effectively in Inventor. The next section covers planes in Inventor, how they work, and the best ways of using them.

Work planes – Best practices

When modeling in Inventor, the correct application of work planes and features is of great importance. When creating features within Inventor, the existing geometry may not possess the required reference to place a new feature or sketch. In this scenario, the creation of a plane is used to create the feature references required.

Several different types of work planes can be applied and having a fundamental knowledge of them is essential to master more advanced functionality.

The full list and an explanation of each one can be found in Inventor. Navigate to the 3D Model tab, and along the ribbon, you will find the Work Features area. Clicking on Plane will reveal the drop-down list of all work planes that can be created within Inventor. Hovering the cursor over each Plane option shows an explanation of how each one can be used:

Figure 1.12: List of planes from the Plane command

Work planes are non-solids and do not have any mass; they are simply used as a reference from which to create new geometry or features where there normally would not be any. By default, at the origin of a new part, you will have three origin work planes.

Figure 1.13 provides a summary of all work planes in Inventor, and examples of how they are used:

Figure 1.13: Work planes and examples in Inventor

Now that we have covered all types of work planes, here are some best practices to keep in mind:

In some instances, you will need to create multiple planes to create and place a plane where it is desired; these can be known as sacrificial planes.You can rename planes and axes in the Model browser. This helps bring organization to your model and allows for faster edits.Redefining planes is possible. Right-click on a plane and select Redefine Feature. You will then be asked to select a new reference for that plane.Work planes are infinite in size although, in the graphics window, they will only display as a small segment. This is so as not to confuse the user or obstruct the view. You can resize and stretch the visible area of any plane.Combining axes, points, and planes is encouraged to create the correct references for geometry.

Work planes in Inventor are complementary to the use of work axes; in the next section, we will examine the types of work axes you can apply and how these are used.

Work axes – Best practices

A work axis is a construction line of infinite length that is parametrically attached to a part. A work axis compliments the use of work planes and can be used as a reference in the creation of new axes/planes, or other part modeling features such as a Revolve operation.

A summary of all work axes in Inventor (with examples of how they are used) is shown in Figure 1.14:

Figure 1.14: Work axes and examples in Inventor

Now that we have covered all the work axes, here are some best practices to keep in mind:

Work planes and work points can be created when applying work axes and used as a reference.You can redefine references for axes by right-clicking on a work axis and selecting Redefine Feature.You can change the visibility of work axes in the same way as work planes. Right-click on an axis and select Visibility. The global control for this in Inventor can be found by clicking on the View tab, then the Visibility panel, and selecting Object Visibility.

With work axes, quite often, a point of reference needs to be made with a work point. This next section covers the types of work points, how they are used, and the best practices.

Work points – Best practices

Work points are used as references when creating planes and axes. They can also be used in the application of a 3D sketch.

A summary of all work points in Inventor (with examples of how they are used) is shown in Figure 1.15:

Figure 1.15: Work points and examples in Inventor

Now that we have covered all work points, here are some best practices to keep in mind:

You can apply work points to a vertex, sketch point, mid-point, and center point of loops and edges, and the intersection of a plane/surface and line pointOnce the work point option is selected, you must then select applicable references to create the pointCenter Point of Loops and Edges is useful to act as a reference for a Hole feature that is required to be centered on the referenced geometry, regardless of updates

Now that we have covered the basics of sketches and work features, in the first recipe of the book, you will apply the knowledge learned and create a complex part.

Applying best sketch and work plane practices to model a part

In this exercise, we will combine many of the best practices for sketches, constraints, and planes to model a part most efficiently.

There are numerous ways that this part could be created, and there is no absolute correct method, but this method is one of the most efficient and will make use of the skills and topics already covered in this chapter.

Getting ready

To begin, we need to analyze the finished part in Figure 1.16. The part is shown from above and underneath. The objective is to recreate this in the most efficient way. No dimensions are given at this stage, as we will go through each step, and the appropriate dimensions will be given at each step.

Figure 1.16: Final part – the end objective of this recipe

While this may look like a complex part with a myriad of geometry, using the best practices outlined previously, we can create this in a very efficient way that enables the user to also make quick edits to the part should this be required in the future. All dimensions will be given to you at each step.

There is no requirement to use a practice file with this recipe; you will simply need to create a new part file.

The first step is to look at the model and begin to understand the plan for the features and methodology that will be used to create it. You may just have a hand-drawn sketch or an idea in your head about what is to be created in Inventor, but the same rule applies.

Here are some things that we can decipher from the image of the part in Figure 1.16:

There are revolved profiles that make up the bulk of the modelIt has multiple lines of symmetry, which means that areas of the part can be copied or arrayedIt has repeating patterns; many of the features in this model are repeating and, therefore, need only to be created onceThe part is hollow, meaning a Shell operation could be usedThe fillets are uniform and can be created in one operation

How to do it…

So, let’s combine the best practices for sketches, constraints, and planes to model a part in the most efficient way:

Create a new part file. To do this, from File, select New, then New again. Select Metric, then Standard (mm).ipt.The first sketch can take several forms. To begin, start at the origin, as this will result in fewer dimensions and constraints being required to define the first sketch.

As the part is made up of revolved geometry, it is logical to proceed with a suitable sketch that can be revolved. The center construction line placed will act as the reference for a Revolve operation later. As the part is symmetrical, it also makes sense to only draw half the profile:

So, click on Start 2D Sketch and create the sketch shown in Figure 1.17 on the XY plane.

Figure 1.17: The first sketch to create on the XY plane

Now that a base sketch has been created and is fully constrained, use the Revolve command to revolve this sketch 360 degrees from the axis. This will create the base feature. To do this, select Finish Sketch, navigate to the 3D Model tab, and select Revolve (you can also press R to access Revolve too).Proceed to select the three sketch profiles created, then select Axis from the box and pick the construction line to act as an axis for Revolve. The preview should look Figure 1.18:

Figure 1.18: Revolve operation of the first sketch

Select OK to complete the revolved feature.

Now that the base feature is complete, we can move on to detailing the model further. In the previous step, using a simple sketch and the appropriate feature, we created the base feature of the model efficiently, in a way that is easy to edit and update.

Navigate to the top view and select Start 2D Sketch on the face highlighted in Figure 1.19:

Figure 1.19: Face to create the second sketch

In this next operation, we will now create the arrayed lugs that protrude from the mid-section of the shape. As they are repeated and identical, it is logical to only draw this once and then copy/pattern the feature afterward. The holes will also be applied at this stage.

Create the sketch shown in Figure 1.20. Remember to select F7 while in the sketch to temporarily cut the model, so that you have better visibility of the sketch plane you are working from:

Figure 1.20: Sketch plane with model cut using the F7 command

To create this sketch from the sketch tools, select Project Geometry and select the two faces of the model. This will trace the geometry and project a copy of this to your sketch. This allows you to utilize the existing geometry present in other features (see Figure 1.20). This results in fewer dimensions and constraints being required to build the sketch.

Then, using the Line command, create a line that is joined from the outer profile and inner profile, as shown in Figure 1.21:

Figure 1.21: The next sketch lines to apply

Then, using Construction Line, create a construction line through the center of the part. This is shown by the dotted line in Figure 1.21. After that, using Line, apply a line from the outer profile to the inner profile. Select Dimension and apply a 5 mm dimension between the line that you created previously and the central construction line. Repeat the process for the other side.

Select Finish Sketch and press F7 to resume the default view.Select Extrude and pick the sketch profile created in step 8. Extend this to another face, and select the face, as shown in Figure 1.22:

Figure 1.22: Extrusion of newly created lug profile

Select OK to complete the feature creation.The next step is to create the various hole placements on the model. So, select the top face of the model and select Start 2D Sketch.Then, use the Project Geometry command to create a center point circle from the sketch origin that is 35 mm in diameter, as shown in Figure 1.23:

Figure 1.23: The sketch required to create the center bore

Select Extrude and pick the inner profile of the 35 mm circle. Then, select Cut, followed by Through All, which creates the central bore of the model:

Figure 1.24: Cut operation of the circular sketch to create the bore

Create a new sketch on the top face of the lug previously created. Here, we will define the hole placement.Use the Project Geometry command to project the geometry of the face and apply construction lines as shown in Figure 1.25 The construction lines snapped to mid-points will create an intersection where a sketch point can be placed to locate a hole using the Hole feature.Add the sketch point to the intersection of the construction lines:

Figure 1.25: Sketch point at the intersection of a sketch curve

Create a sketch on the XY work plane. If the work plane was not in the correct location, one could be created using an axis through the revolved feature, and then creating a plane referencing this axis and a vertex on the model. Fortunately, in this case, the XY plane is in the location required, as we have consistently modeled from the origin throughout.Press F7 to cut the model to improve visibility and create the following sketch. Use Project Geometry, and select the geometry shown in Figure 1.26:

Figure 1.26: Geometry to project

Proceed to create two construction lines that snap to the mid-points of the previously projected geometry. At the intersection of the two construction lines, apply a sketch point to locate the hole, as shown in Figure 1.27:

Figure 1.27: F7 cut away in sketch mode required to locate and place the second sketch point

Select Finish Sketch.Now, we will generate the desired holes. From the 3D Model tab, in the Modify panel, select Hole from the ribbon, and select the two sketch points as the center point/locating reference. Only one hole can be created at a time this way, so the same will have to be repeated for the second hole.Apply the settings shown in Figure 1.28 to detail the hole:

Figure 1.28: Hole command in use, using the sketch point as a reference

You should set the diameter as 5 mm, the Hole type as Simple Hole, Seat as None, and the Termination type as Through All. Also, ensure the Direction setting of the hole is as per Figure 1.28.

Repeat steps 22 and 23 for the second hole, but set Direction as Symmetric instead. Then, select OK to complete. The result is shown in Figure 1.29:

Figure 1.29: Second hole using a second sketch point created as a reference

This allows us to apply two holes in one operation. Exit the Hole command.

The base features are now created, and we can now focus on creating the circular array of repeating features. Because this has been drawn once, we need to reuse the geometry to be efficient.Begin by selecting the 3D Model tab, then select Circular Pattern.Ensure that the lug extrusion and both holes are selected as features to pattern. For the axis, select the internal cylinder; this will create a work axis within the feature command, from which to revolve Circular Pattern. You can also pick the features from the Model browser while in the command.

Figure 1.30: Circular Pattern creating the rest of the required geometry

Set Placement to 6 and ensure the features are patterned 360 degrees. Select OK.Now, the fillets on the model must be applied. This could have been done before Circular Pattern, but it is best practice to apply fillets after, as this is often quicker and requires less processing time. All the fillets can still be added in one operation.Select Fillet from the 3D model tab, and select the edges shown in Figure 1.31. In the Fillet command, set the radius of the fillet to 2.5 mm, and for the edges, select 12 Edges, as shown in Figure 1.31:

.

Figure 1.31: First fillet operation and required filleted edges

Deselecting a fillet

If you accidentally select the wrong edge and apply a fillet in the Fillet command, hold Shift and select the incorrect edge to remove the fillet. This keeps you in the command and prevents a restart of the operation.

Do not select OK to complete. Instead, hit the green plus icon on the menu to detail another type of fillet on the model. This process can be repeated and enables you to generate many types of fillets in one operation, keeping the Model browser and history of features clean.Select the edges shown in Figure 1.32, and set the fillet radius to 3 mm:

Figure 1.32: Second fillet operation

Finally, apply a 1