Introduction to Inventor

An Interactive Workshop

22 min readSep 14, 2020

Preface

This workshop aims to serve as an introduction to basic Computer-Aided Design (CAD) concepts for people unfamiliar with virtual modelling. The software we introduce is Autodesk’s Inventor, available for free to students under an educational license here.

Each section of this workshop is accompanied by an instructional video. There are five sections, with each followed around one of the following topics:

About Inventor
Working in 2D Space
Working in 3D Space
Assembling Objects
Useful Features

If you have any questions — with the content covered in the videos or using Inventor in general — feel free to message the UQ MARS Discord Server. We’re happy to help you out.

Part 1 — About Inventor

We’re going to start out by learning a little bit about how we can use CAD modelling, and walking through how to set up our first file.

Why Learn CAD Modelling?

The models you create in Inventor can have a wide range of uses, for engineers and hobbyists alike. They may be used to create technical drawings for manufacturing physical components, 3D printed directly from a file, or used in other digital projects, such as PCB design or other simulations.

In this tutorial, we are going to be working on creating the part shown below, which would work as part of a robotic arm.

The goal — our finished robotic arm component

Before we can get started on that, however, we need to learn what tools to use.

Getting Started

You can create your first file by following these steps:

Open Autodesk Inventor
Once you get to the home screen, click on ‘File’ in the top-left corner, then ‘New’
A pop-up window, ‘Create New File’, will appear. Expand the ‘Templates’ folder to see a list of available templates to choose from. In this tutorial, we’ll be working in metric units, so expand ‘en-US’ and select the ‘Metric’ folder
Select ‘Standard (mm).ipt’ from the list of templates, then hit ‘Create’ in the bottom-right corner of the ‘Create New File’ pop-up window

Congratulations on making your first file! You’ll find yourself on a window that looks something like this:

It’s important to know what the following key parts of this screen are:

Workspace: Center of the screen. Where your part will be displayed. It’s blank for now, but we haven’t started yet
Toolbar: Top of the screen. You can select tools to use from up here. It won’t always look the same, depending on if you’re in 2D or 3D mode, but more on this later.
Hierarchy Browser: Left of the screen. Shows you the current part, the history of actions applied to it, as well as any work planes and axes created. The origin is there by default.
View Options: Right of the screen. Includes the clickable View Cube for predefined views, as well as tools for panning, zooming and rotating.

Part 2 — Working in 2D Space

Inventor works by turning the 2D profile sketches we create into 3D objects. To start making our first part, we’re going to explore the tools available in the 2D workspace.

Sketches and Work Planes

We’re going to create our 2D Sketch by clicking on the ‘Start 2D Sketch’ tool. This is available on the far left of the toolbar under the 3D Model Toolbar, as shown below:

‘Start 2D Sketch’ tool selected from the Toolbar

You’ll see now that three squares appear in the Workspace. These are the origin planes. When you start a part, what you’re doing is essentially making a 2D cross-section, which we are then able to turn into a 3D object later. So have a think about which way of looking at your part, or plane, will make it easiest to draw a cross-section.

Click on one of the three planes to get started. When drawing a part from scratch, which one you pick doesn’t matter too much, so we’re just going to pick the XZ Plane.

The 2D Sketch Environment

You’ll notice that once you’ve selected a Work Plane, the Toolbar will display different options from those we saw earlier. This is because we have now entered Sketch mode.

Let’s take a bit of a tour through the Create, Constrain and Format tabs to learn the basics of drawing lines.

The Create Tab — Part I

Let’s take a look at what some of these tools do, starting with those found in the ‘Create’ tab:

Line Tool: Used for creating straight lines. You start a line by clicking at one of the desired end points. You can then either click at the second end point, and a line will be created between the two, or you can enter a length and an angle into the boxes which appear. You can use the ‘Tab’ key to switch between the two. Once you’re happy with the length and angle in the boxes, left-click again to place the second end point.

After drawing your line, hit the ‘Escape’ or ‘Enter’ keys to exit the Line Tool, or right-click and select ‘Cancel’ from the wheel menu that appears. This also applies for all Tools.

Circle Tool: Used for creating circles. Start by clicking where you would like the center point of your circle. You can now drag the mouse in and out to choose a diameter, or enter one into the textbox if you know what size you’re after.

Rectangle Tool: Used for creating rectangles. The default ‘Two Point Rectangle’ option has you select one corner, then either enter a length and width in the textboxes, or place a second corner. The rectangle will then be drawn between the two corners, creating all four sides at once. This saves a bit of time to drawing four separate lines, and automatically constrains each side to be square.

The Constrain Tab

The following tools may be found in the ‘Constraint’ tab. Constraints help to define rules for the way our lines connect together. If a constraint has been created, it cannot be indirectly broken, but can be deleted. Existing constraints may cause new constraints to show error messages if they cannot be created due to a conflict.

Dimension Tool: Similar to the box that appears after creating a line or circle, the ‘Dimension’ tool may be used to apply a length to a line, diameter to a circle, or define an angle between two lines.

Coincident Constraint Tool: Use this tool to make sure two lines or objects intersect one another. You can select an entire line, the center of a circle, or pick the endpoints or midpoints of a line for a more specific definition.

Perpendicular Constraint Tool: This tool may be used to enforce that two lines remain perpendicular, or at a right angle of 90°, to each other. It is also possible to chose a plane or axis for a line to be perpendicular to.

Tangent Constraint Tool: Can be used to make a line or curve tangential to curve. Tangential means that the intersection is forced to occur with the incident line perpendicular to the radius of the circle at the point of intersection.

The Format Tab

We’re also going to hop over to the ‘Format’ tab and take a look at the different types of lines we are able to create. You click on each icon to switch to drawing lines in that mode.

Construction Lines: These are a type of line which we can use while drawing, but won’t show up in the final profile. Consider them a sort of guideline which we can use to place our real lines on. They show up as dashed so you can easily tell them apart.

Center Lines: A type of line which we can use to mirror parts. They show up with a different dash type to Construction Lines. Any dimensions created on a Center Line will be mirrored equally on the opposite side.

Our First Sketch

Now that you’re familiar with some of the tools in Inventor, have a go at drawing the following sketch. If you get stuck, the video at the top of the section has a more detailed walk-through of each step. We will mainly be using the ‘Line’ and ‘Circle’ tools, as well making use of Construction and Center line types.

The combined power of the ‘Line’ and ‘Circle’ tools

Our part is starting to look good, but it’s not exactly perfect. See how there are lines inside our profile, connecting the straight sections to the center hole? We don’t want those in the final part, so we’re going to tidy it up so our sketch is just an outline of what we want to make.

The Modify Tab

To tidy up our sketch a little, we’re going to want to modify our existing lines, rather than drawing any new ones. The tools in the ‘Modify’ tab are going to help us do that:

Trim Tool: This tool can used to remove a section of a line or curve. You’ll need an intersecting line to mark how much you want to cut away, but the preview will highlight the section you are about to cut.

Extend Tool: The opposite of the ‘Trim’ tool. Select a line or curve to extend it to the next intersecting point. Again, a preview of the action will be shown when you hover over the line, helping you figure out where to click.

Cleaning up Our Sketch

Let’s go back to our sketch and use the ‘Trim’ tool to get rid of the extra lines we talked about earlier.

One trick used to make parts last longer is to replace corners with curves, to help spread out mechanical stress. It’s why airplanes have round windows rather than square or rectangular ones. We’re going to go back to the ‘Create’ tab to learn how to put some rounded corners on our part.

The Create Tab — Part II

The ‘Fillet’ and ‘Chamfer’ tools are useful to dull the corners on your parts. To use these tools, you’ll need two lines or curves which meet together at a point.

Fillet Tool: Use this tool to put rounded corners on your part. This works by selecting any two lines which meet in a corner, then inputting the radius of the curve you wish to use in place of the corner. It’s possible to select multiple corners at once, too.

Chamfer Tool: Use this tool to put a cut-off corner on your part. Works similar to the ‘Fillet’ tool, by selecting two lines that meet in a corner. It’s possible to make non-right angle chamfers using the menu that appears when using this tool.

Rounding Corners

Let’s have a go at rounding those corners. We used a radius of 3mm, but what you choose doesn’t matter too much for what we’re doing.

Our sketch is starting to look good now, but there’s still one problem — we’ve only drawn half our part. Let’s take a look at how we can mirror our part to make it symmetrical.

The Pattern Tab

The tools in this tab are focused on duplicating shapes you have already drawn. We’re only going to look at the ‘Mirror’ tool right now, though.

Mirror Tool: Used to mirror lines and curves. First, select the lines you with to mirror with the ‘Select’ option. Multiple may be selected . Then, pick the axes you wish to mirror about with the ‘Mirror Line’ option, then hit the ‘Apply’ button.

Mirroring Our Sketch

Let’s try mirroring our sketch now. Select all the lines we’ve draw on the left-hand side using the ‘Select’ option in the ‘Mirror’ tool, then pick our Center Line as the ‘Mirror Line’. Our sketch should now look something like this:

That’s looking pretty good! You can go ahead and hit the ‘Finish Sketch’ button, the big green tick at the end of the Toolbar, to return to the 3D environment.

Part 3 — Working in 3D Space

So we’ve got ourselves a 2D sketch, which serves as an outline of our part. How do we go about making it into a 3D object?

Types of Extrusions

Depending on the type of shape we want to make, there are two main tools we will want to use to do this — ‘Extrude’ and ‘Revolve’. Let’s take a look at these now:

Extrude Tool: This tool takes the cross-section we created earlier, and projects it by a specified length to turn it into an object. Start by clicking on the outline of a sketch, then entering a distance to project by. You can chose which direction you project in, as well perform a symmetrical or asymmetrical projection, too, with the options in the Extrusion pop-up menu. If you can’t select your sketch, it most likely means your shape is not ‘closed’ and that there is a break in the outline somewhere.

Revolve Tool: Works similar to the ‘Extrude’ tool, but produces a circular projection. Select your outline, then select an axis to revolve around. Instead of a distance, you input an angle to revolve by.

Extruding Our Part

We can extrude our part with the following steps:

Select the ‘Extrude’ tool
Select the profile of our 2D Sketch. Use the preview to make sure you’re picking the right area.
Set a distance of 2mm and select the Symmetrical option.
Once you’re happy with the settings, hit ‘OK’

Navigating in 3D Space

Now that we have a 3D part, let’s run through a few of the view options we have. These can be found on the right-hand side of the screen.

The first of these are the View Cube and Home button. Clicking on a face, edge or corner of the View Cube will rotate you to a pre-defined view of the object., putting you nice and square with the origin axes. You can also click the Home button to take you to the default camera position.

Clicking either of these will also zoom you out enough such that the whole part is viewable on screen. You can also zoom in and out by using the scroll wheel on your mouse.

The first option in the sidebar is the Full Navigation Wheel, but we’re going to be skipping over that as it’s not very beginner-friendly. Instead, we’re going to go through the next four icons one-by-one:

Pan Tool: Signified by the hand icon. This lets you move across the screen without zooming or rotating. You can pan by either selecting this tool and left-clicking, or by holding the the middle-click button and moving the mouse.

View All Tool: Signified by the magnifying glass and page icon. This will automatically zoom you out so that the whole part is visible and centered on the screen. Click the icon once to use.

Free Orbit Tool: Signified by the orbital icon. This allows you to view your part from any angle you wish, going beyond the pre-defined views given by the View Cube. Left-click and drag the mouse with this tool selected to use.

Look At Tool: Signified by the flip book icon. With this selected, you can click on a face of your part to have the camera automatically line up with it, useful for when you have more complex objects with unusual faces.

Changing Materials

The next thing we’re going to do to our part is add some colour. At the top of the screen, above the Toolbar, you will see there are two drop-down menus — one that reads ‘Generic’, the other ‘Default’.

The left-hand one can be used to change the part’s material. This will affect things like calculated mass and tensile properties in simulation. Inventor has a large selection of materials, with everything from gold to carbon fiber and wood included. There’s also material options for several types of 3D printing plastic, not to mention that you can define your own. The right-hand box will only apply cosmetic changes, leaving the technical properties untouched.

We went ahead and set the material to ‘Silver’ and the colour to ‘Smooth — Red’, but go ahead and pick your favourites.

Making Modifications

Next up, we need to make a few modifications to our part we’re happy with it. We want to put some rounded edges on corners to make it smooth to handle. We also want to put a screw through the hole at each end, so we want to cut some material away such that the screw head sits flush with the part.

Recall the ‘Fillet’ and ‘Chamfer’ tools from Part 2? We’re able to use 3D versions of these to make changes our part without editing the original sketch. Go ahead and select these from the ‘Modify’ tab of the 3D Model Toolbar. To apply a fillet:

Select the ‘Fillet’ tool
Select the top and bottom perimeters of the part
Use the pop-up menu to set the radius to about 0.5mm
Hit ‘Apply’ when you’re happy with the preview

You can do the same again for the ‘Chamfer’ tool, this time selecting the top and bottom edges of the screw holes at each end. Again, we went with a 0.5mm distance on this one.

Your part should now look something like this:

Adding Text

Want to write your name on the part? Add a version number? Or a label? We’re going to add ‘UQ MARS’ to our part, but feel free to use your own name here.

Start off by creating a new 2D Sketch. You’ll notice that this time, the origin planes won’t appear. Instead, we’re able to click on the faces of our part. Selecting the top face should give us plenty of space to write our text.

Now you’re in Sketch mode, go up to the ‘Create’ tab and select the Text tool. A pop-up menu will appear which lets you choose text size, font, colour, alignment, etc. We went with a text size of 1.0mm

When you’re happy with your text, hit ‘Okay’. If your textbox is situated vertically instead of horizontally, you can use the ‘Rotate’ tool in the ‘Modify’ tab to put it the right way up. Select the text, then pick any point with the Center Point option to rotate about.

We’re going to use the following process to make sure our text is centered:

Draw one Construction Line that runs horizontally along the member, between the center points of the two screw holes
Draw another Construction Line that runs vertically along the member, between the top and bottom edge, at the center of the part
Constrain the text to each of the Construction Lines. You can do this either with the ‘Dimension’ tool, as shown in this section’s video, or by using the ‘Coincident Constraint’ tool and binding the green half-way point of the top and left sides of the textbox to the vertical and horizontal lines, respectively
Hit the green ‘Finish Sketch’ button to exit Sketch mode and return to the 3D workspace

Our text currently exists as a flat 2D Sketch. To turn it into something that will show up in manufacture or 3D printing, we need to use the ‘Emboss’ tool to add some definition.

Click on the ‘Emboss’ tool and select our text sketch. You’ll see now that this pop-up looks a little bit like the ‘Extrude’ menu. Select the text profile, then choose whether you want to emboss or engrave from the face. Embossing will add material, making the text ‘stick out’, while engraving will remove material, insetting the text. We’re going to go with the ‘Engrave’ option, as this usually reads easier when 3D printing, and produces a smoother finish. Choose a depth of about 1mm then hit ‘Okay’ to apply.

Your component should now be looking something like this:

Finished linking member with engraved text

Don’t forget to save your part one you’ve finished.

Part 4 — Assembling Objects

We’ve got ourselves a part, but what if our project is made of multiple components? You can use an Assembly to place multiple parts into the same workspace, allowing you to see the finished product.

Making an Assembly

We make an Assembly as a new type of file. To get started, follow these steps:

Similar to making our part, click on ‘File’ in the top-left corner, then ‘New’
Expand the ‘Templates’ folder in the pop-up window. In the file hierarchy on the left-hand side, expand ‘en-US’ and select the ‘Metric’ folder
Select ‘Standard (mm).iam’ from the second row of templates, then hit ‘Create’ in the bottom-right corner of the ‘Create New File’ pop-up window

When you enter the Assembly environment, you’ll be met by blank Workspace and a new Toolbar.

Placing a Component

Select the ‘Place’ tool from the Toolbar. Navigate to the location where you saved the part, then select it and hit ‘Open’. You can now place the part into the Assembly environment by left-clicking. We’re going to go ahead and put two copies of it down.

Two copies of our part in the Assembly Workspace

Joining Two Components

We’ve placed our parts, but how do we get them to interface with each other? Let’s take a look at the ‘Constraint’ tool in the ‘Relationships’ tab to learn how to do this.

Constraint Tool: Similar to the constraint options in 2D Sketch, Assembly Constraints can be used to bind faces or edges together. Types of constraints include Mate, where two faces are orientated to be connected, Flush, where two faces are orientated to face in the same direction, Axial, where two axes are situated to be aligned, and Tangential, which allows for curved faces to be joined.

First off, we’re going to right-click on one of our parts and make sure the ‘Grounded’ option is ticked, about two-thirds of the way down the pop-up menu. This will lock the part in place, meaning only one of our parts will be able to be moved.

Next up, we’re going to create a Mate constraint between the large flat sides of our two parts. Then, create an Axial constraint between one of the screw holes of each component, and that of the other. If you’re not sure where to click on the parts to do this, check this section’s video. When you’re done, your assembly should be positioned something like this:

Creating Parts and Work Features

While our two parts are lined up, it might be a good idea to show how a screw would fit in the holes. To make sure our screw fits, we’re going to create a new part right from our Assembly. First, we’re going to take a look at the ‘Work Features’ tab, and how we can create more planes and axes for us to draw on.

Plane Tool: Similar to the three origin planes we see at the start of every part, we can use the Plane tool to create more planes for us to draw on. We can create planes offset from existing surfaces, axes or the origin planes.

Axis Tool: Lets us create additional axes on our components. Creating more axes is especially useful when you want to mirror, pattern or revolve a part. Offset from an existing feature, plane or axis.

To create our screw in the Assembly environment:

Click on the ‘Create’ button at the start of the Toolbar. Put in a filename and location, then hit ‘Okay’
You will need to select a face to work off. Select one of the large flat faces of our linking members
Select the ‘Axis’ tool, then select one of the curved surfaces that surrounds our two overlapping screw holes. Clicking will create a new axis that runs right up the middle of our joint
Select the ‘Plane’ tool, then select the XZ plane. You can find this by clicking on your new component’s filename in the File Hierarchy, then expanding the Origin folder, then left-clicking on the XZ plane.
Select our newly-created axis. Hit ‘Okay’ when asked to put in an angle. Exit the ‘Plane’ tool.
Drag the newly created axis so that it sits near our screw holes.

Your work plane should now look something like this:

Projecting Geometry

Now, create a 2D Sketch on our new work plane. We’re going to use the Project Geometry tool in the ‘Create’ tab, so let’s read up on what that does.

Project Geometry: This tool allows us to create an ‘image’ or projection of a feature on another plane. Think of this like a shadow — the shadow changes depending on the angle between the two objects, but serves as an outline of the shape.

Try having a go at using the ‘Project Geometry’ tool to project the walls of our screw hole onto our plane. We’re going to fill in the rest of our sketch too, so that we have half of our screw’s profile. See if you can make the sketch shown below. If you need help with the specific steps, check this section’s video.

Once you’ve got that, hit ‘Finish Sketch’, then use the ‘Revolve’ tool to turn our profile into a round 3D object. Select the axis we created earlier as the revolution axis and perform a full revolve (360°).

Hit ‘Return’ in the top-right end of our Toolbar to finish your component and return to the Assembly. You can now turn the visibility of the Work Plane and Axis off. That’s it! You’ve finished your Assembly!

Our completed Assembly — complete with linking members and screw

Part 5 — Useful Features

Our Assembly is looking good, so we’re going to cover a few more useful features of Inventor before we wrap up.

The following tools are especially useful to keep in mind when working on your own Inventor projects:

Measure Tool: Useful for measuring the distance between two features. Click on any two faces, edges, vertices, planes or axes to check the distance between them. Found in the Tools Toolbar.

Center of Gravity Tool: Shows the location of the center of gravity of a part or assembly, in the form of a set of axes and planes. This will update as you make changes to your parts, and can be found in the ‘Visibility’ tab of the View Toolbar.

Half-Section View Tool: Allows you to see a cross-section at any point along your part. Click on a plane or face and enter an offset to view the cross-section from. Found in the ‘Visibility’ tab of the View Toolbar.

Exporting Files for 3D Printing

CAD is great for making virtual models, but can we make anything physical with it? We sure can! If you want to 3D print a file you’ve made, open the part, then go to the ‘File’ menu, hover over ‘Print’, then select ‘Send to 3D Print Service’. Make sure the length, width and height displayed in the menu match your part’s expected dimensions. In most cases, you’ll want your scale to be 1:1 as well. Set the Export File Type to STL and hit ‘Okay’ to create the file.

You should then be able to load this file onto your 3D printer and create a physical version of your component.

Conclusion

Covered Content

If you made it this far, you should now have an understanding of how to do the following things:

Use the 2D Sketch environment to create a part from scratch
Use the 3D environment and tools to view and modify a model
Change the material your part is made of
Create an Assembly using multiple files to show how your project fits together
Use some of Inventor’s most useful tools to measure and understand your part better
Export a finished file for 3D printing

Where Next?

This tutorial only scratches the surface of what is possible with Inventor and CAD software. Things we didn’t cover include:

Creating technical drawings which describe your part’s dimensions and how it can be manufactured
Using the Sheet Metal environment to design components made from folded material
A variety of tools for creating more complicated shapes, such as the Spline Tool, Lofted Extrusions, Thread and Shell
Simulation tools to help you perform stress analysis and predict when your part will fail
Importing pre-made parts from open-source file repositories

If you’re keen to learn about any of these specifically, have a Google or check out Autodesk’s online Design Academy for more tutorials.

If you decide to start a project of our own and get stuck, we’re always happy to help out on the UQ MARS Discord Server, too.

Thank You

Congratulations! You’ve officially finished the UQ MARS Introduction to Inventor workshop, and made producing this content worthwhile. We’re keen to see what you make with the knowledge you’ve gained in this tutorial, so feel free to show off your projects or hit us with any lingering questions.

If you’d like to give feedback on this workshop, use this form to share your thoughts or give suggestions.

Thank you for reading!

Created and presented by Keith Cunningham
Article and editing by Matthew Cook