Explore 3D

Part 1: Beginners Guide to Fusion 360

Johann Wyss

Issue 24, July 2019

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Tinkercad is great when you first start out in 3D printing but is limited in what it can do. We show you how to get started with Fusion 360 instead, and it’s also free to use!

3D printing can be an extremely fun and rewarding hobby. It can teach you a huge amount about manufacturing processes, CNC robotics, material sciences, and general engineering. For the most part, we all start out just exclusively trawling Thingiverse for something cool and unique to print. Shortly after, we learn to make small modifications to the things we find on Thingiverse and then start to make our own small designs using Tinkercad as a starting point.

Soon, we quickly learn the limitations of Tinkercad. Whilst incredible things can be made with this free online tool, it’s a lot more clunky than a specially designed piece of CAD software.

Over the next few issues, we are going to show you how you can easily make some of your own designs using Fusion 360.

There are many 3D CAD programs available, however, we picked Fusion 360 because it is powerful parametric modelling software, which students and hobbyists can get free of charge. This is a very important point because most parametric modelling software are prohibitively expensive, costing several thousands of dollars for a yearly license.


The first thing we need to do is download the software. Go to https://www.autodesk.com/campaigns/fusion-360-for-hobbyists which will bring you to the following welcome screen.

Select the ‘Get started now’ button. This will scroll the page down showing the following options.

Follow the steps shown ensuring you take your time and read through the page titled “check your eligibility”. If you’re eligible to use the software, which we imagine you will be, go on to step 2 and choose the “create account” link.

Fill in the details using a correct email address and you will be bought to the next screen. Alternatively, if you already have an Autodesk account from TinkerCad or Eagle, you can use that account to log in. Just use the sign in button at the bottom of the page.

Now it’s just a matter of installing the software onto your computer, which is done by pressing the get started button.

After installing and running for the first time, you will be prompted to verify your email address. Go to your email client and find the verification email sent from Autodesk. Simply press the “Verify Email” link in that email and follow the prompts to login to your new Autodesk account.

You then want to open the Fusion 360 software on your computer and sign in using the same details.

After a small wait to finalise the install, you will be greeted with the following screen showing you how to access you preferences, including privacy settings, etc.

That’s it, you now have a Fusion 360 account and the software installed on your system.


If you look to the right of the main work area, you will see a small dialog box. This box allows you to select navigation and view settings based on what you’re used to. For example, if you are familiar with Tinkercad, you can select it from the navigate and view dropdown menu. This will change all of your mouse controls to match the controls in Tinkercad. This makes it much easier to navigate. Take note of the settings and familiarise yourself by navigating around the empty work plane in front of you.

Now that you have grasped the work plane manipulation, let's move on and start learning how to draw in Fusion 360.

Press the ‘Start here' button if you want to follow some tutorials provided by Fusion 360, or select the close button to get drawing.

Note: We highly recommend you go through the provided tutorials as they will undoubtedly teach you some tips and tricks specific to Fusion 360 that we may not cover over the next few issues.


For our very first project, we are going to start with something nice and simple, just to get ourselves comfortable with the Fusion 360 interface.

A useful tool for newcomers to 3D CAD design is a round gauge (also known as a Radius Gauge). This is a basic tool a 3D modeller can use to easily measure the curvature of an item you are modelling. Let’s say, for example, you want to make a cover for your mobile phone.

There are a number of rounded corners and rounded edges on modern phones. It would be very time consuming and difficult to physically calculate the geometry for each of these rounded edges, so for quick jobs, it's often much more convenient to have a round gauge. You simply put the gauge against a rounded object to determine the radius.

You will certainly find this gauge useful as you start to model real-world objects. It's simple yet detailed design makes it the perfect candidate for our first ever Fusion 360 project.

To get started, take a look at the drawing on the opposite page to give you the basic idea of what we are going to draw in Fusion 360.

The first thing we need to do in Fusion 360 is set the perspective. Since we will start by drawing a simple 2D shape and extruding it from a single plane, we find it best to work from the top-down perspective.

To change to this top-down perspective, mouse over to the perspective box in the top right corner of the work plane. Left click the word 'top' on this cube and your perspective will change to this plane.

From here, we want to start drawing the features of the round gauge.

Select the 'Sketch' button in the top left menu and then select the blue square that appears on the work plane. This square sets the origin to the plane, which means in what space we are drawing X, Y or Z.

To start drawing, press the 'C' key on your keyboard. This will select the circle drawing tool. Left-click once anywhere in the work plane and you will begin to draw a circle. From this point, you can simply enter the required diameter of the circle.

Our drawing shows the curved edge on the right side of the gauge has a radius of 8. We need to multiply that value by 2 to get the diameter. Enter 16 on your keyboard and press Enter.

You should now have a perfect 2D circle, which you can place on the work plane. You can click and hold the centre point of this circle and drag it around the work plane to position it where you want.

Looking at the drawing above, we know that the opposite side is also constructed with a circle with a radius of 22.1, giving it a diameter of 44.2.

Repeat the previous steps and create a second circle with this diameter and place it to the left of the first circle.

Your drawing should look something like this. Note that at this point, we can move both circles around as there is no relationship between the two objects. To fix this, we want to create a straight line between the top of the two circles 126.35mm long. To do that, use the line tool by pressing 'L' on your keyboard, and draw a straight tangental line across the top with a distance of 126.35mm.

In the sketch palette on the right of the work plane, you will see some constraint options. These options allow you to define the relationship between features in your drawing. In this case, we want the line we just drew to be a tangent to the two circles. Select 'Tangent' and then select each of the circles. This will force the circles to align tangental to the 126.35mm line joining them.

Select the 'Coincident' button, select the circles, which will make them both tangent and coincident to the 126.35mm line, firmly locking them all together.

Note: After doing this, the objects will turn black signifying they are fully constrained, and you will be unable to move them. This is ideal as these can not be changed by later actions.

The final step to finishing the outline is to draw a line connecting the bottom of each circle. Simply press the 'L' key on your keyboard and draw a line between the two circles. Use the tangent and coincident constraints to lock this line to the existing features. When you’re done, the sketch should become shaded and the lines should all be black indicating they are fully constrained.

Now we want to add the 11mm radius on the left of the shape. To do this, do the same as previous and press 'C' on your keyboard, then enter the dimensions. We want the diameter now, so its diameter = 2 (radius) or 2 x 11 = 22mm diameter.

Once the circle has been placed, press 'D' on your keyboard to bring up the dimension tool. Select the centre point of the circle we just added, and then the connecting point between the top line and left circle as shown below.

We want this distance to be 13mm, as the diagram shows that the start of the R11 is 2mm from the tangent junction. We also want this to only protrude ½ (radius) into the existing shape. Therefore, use the 'D' key on your keyboard to select the dimensioning tool. Set the distance from centre point of the circle to the top line to one half of the radius as shown.

The drawing should now look like this.

You want to repeat the same process for the remaining 8 radius features on the top line. Keeping in mind, the radius is ½ diameter and the depth is ½ radius. Also, note that each feature is separated by 2mm.

TIP: In Fusion 360, while entering the dimensions you can enter mathematical operations.

To get the distance between the two circles we used the line tool 'L' on the keyboard to measure the distance between the two features. You then simply adjust the distance between the two centres until the distance = 2.

For example, if the distance between the centres of the two features is 23, and the measured gap between them using the line tool was 4.5, you would simply make the distance between them (23 -2.5). This would adjust the gap to 2mm.

When you’re done adding all of the top radii, it should look like this.

We have added the dimensions here to make the distance between circle centres easier. In particular, note that the results are an estimate and more than good enough for the purpose of this exercise.

We now want to add the final radius to the bottom side. Follow the same steps as the previous, noting that the radius starts at the tangent point of the 44.2mm outer circle and the bottom line.

Once you have drawn this, you want to also add a 4mm circle in the 44.2mm end. This will form a hole to allow us to hang the gauge off or connect a key ring. It isn’t important where we place this, just make sure it's close to the edge if you want to attach a ring to it.

When you’re happy with all of the dimensions, choose the 'Select' button from the menu. While holding down the CTRL key on your keyboard select the sections you want to extrude. When done, it should look like this.

Press 'Q ' on your keyboard to enter the press pull tool, which will bring up the following options.

We want to extrude this to 4mm to match the provided drawing. This will force all of the shaded blue areas to become a solid object with a thickness of 4mm. In the distance section, enter 4mm and select OK.

With the 2D model now a 3D model, we are able to start adding some of the details such as the chamfers and number indicators.

Let's start by first placing the numbers. We didn’t add their positions to the drawing as it isn’t overly important where they are placed, provided of course, it easily shows which radius it is referring to.

To get started, select the top face of the 3D model. In the menu, select the dropdown arrow on the sketch button. Move your mouse over the Text selection and left click. Move your mouse to where you want to place your text and left click. This will bring up the text placement menu. Here you can enter the text you want to display, set the size of the text and its angle.

We went with 4mm text. Any smaller and it would be difficult to print clearly, and much higher will reduce our room to sketch in the logo or picture, etc. If you’re going to do the DIYODE logo we recommend you keep it at 4, however, if you’re putting anything else, it will depend on the room you have left.

You want to repeat the process for all 10 of the different radii.

With all ten numbers added and in place, press 'Q' on your keyboard to enter the 'Push Pull' function. Hold down Ctrl and manually select each of the numbers. This will bring up the following extrude menu.

Set the distance to -0.5 to extrude a void into the surface of the model half a millimetre and press OK.

If you change the perspective, you will see the now indented numbers on the surface of the model, as shown below.

Next, we want to add some chamfers to the edges. This will give the model a much more finished appearance.

We are going to give every bottom surface a 1mm chamfer and repeat on the top with the exception of the radii edges. We want them as sharp as possible to aid in gauging.

To add the chamfer select the modify dropdown arrow and select Chamfer. This will open the menu options shown above. Hold down Ctrl and select the edge of each surface, excluding the top side radii. When you release Ctrl, the program will automatically chamfer the edges as per the value in the distance dropdown. When you have chamfered the desired edges by 1mm select OK.

The final step is to add the DIYODE logo or your own. A suitable DIYODE logo is available in the Resources section below.

The easiest way to do this is to import an image and simply trace around it. Naturally, the better the quality of image the easier this will be. Of course, you need to physically trace every edge and then extrude it so this shouldn’t be done with high detail images. There are ways to import .SVG files, which are vector files. However, this requires other software and is outside the scope of a basic introduction to Fusion 360.

To bring an image into Fusion 360, simply select the Insert icon, which will open the attached canvas dialog box. Select the image you wish to import, then select the surface you want the image placed. We are going to make it on the top surface of the round gauge, so select that surface.

This will import the image in full size. To drop the size down, in the scale x and y boxes, we want to enter 0.4. Make sure you do the same value in both, otherwise the ratios will be changed. Also, make sure the Display Through box is left unchecked, otherwise you won’t be able to see the image when we start tracing.

Once you have scaled it to the size you want click-and-drag the image to place in where you want it. When you’re happy with its positioning just choose OK.

Select the top face of the model and press 'L' on your keyboard to select the line tool. The vast majority of our logo is straight lines so we can, for the most part, use the line tool. If your image is fully made of organic shapes, skip ahead to the spline tool section.

You want to trace around each of the straight lines of the letters in the logo using the line tool. Ignore the curved sections of the O and D’s for now, we will use the spline tool for them.

We find it’s a good idea to first do the top and bottom lines. These can be used to define the edges of each letter.

When all the straight lines are traced, select the sketch dropdown arrow in the menu and select the control point spline tool. This tool will smooth out the line your drawing and the more points of reference you give it the smoother the line. Select one of the line ends you made previously, and whilst zoomed in, carefully select the edge of the image following the curvature until you meet the next line end. You simply double-click the end of the meeting line and the spline tool will create a smooth curvature for you.

Precision is not overly important for this logo, the slicing and printing operation will usually remove any small inconsistencies, and as such, provided the spline tool follows the same general shape you will be fine. However, if you’re printing fully organic shapes you will want to take your time with the spline tool.

After you have traced around the logo it should look similar to this.

Just like with the text earlier, we want to extrude this logo as a hollow. Except, in this case, the logo is sitting flat on the work plane surface. As such, we want to include a 3.5mm offset to have it start at this point and extrude out 0.6mm so it clears the model surface.

To do this, press 'Q' on your keyboard to enter the Press-pull process. While holding Ctrl, select each letter of the logo you wish to extrude. Note you may need to change the view so you’re looking at the logo from below.

Once you have done that, your first ever Fusion 360 3D object is complete!

All we need to do now is export the file as an .stl so we can print it. Select the 'Make' button, which will bring up the 3D print menu.

You want to select the model and uncheck the “Send to 3D Print Utility” box. The model will turn blue and show the triangulation wireframe. You can change the refinement if you like, however, we find we just tend to set it to high for every print.

When you’re happy, press OK and choose where to save the file and what name to give it. You can now add this file into your Slicer and print it as normal.

The skills shown in this tutorial are just the basic drawing and extruding tools you will need to get started with Fusion 360. However, the only way to get confident with something is to keep at it.

You can keep the momentum going and modify the gauge, try making it in 0.5mm increments, for example, 3.5mm radius to 12.5mm. The more you use the software the more comfortable you will become with it.