【2025】Autodesk Fusion tutorial for beginners: explained in simple terms

There are several reasons behind the immense popularity of Fusion 360 in a short period. For example, this cloud-based software allows you to save and store your designs online for team collaboration. Moreover, it offers free, limited licenses for non-commercial use.

Most importantly, this software is packed with advanced features, such as CAD and CAM modules, a built-in 3D slicer, rendering, generative design, and topology optimization.

In this article, we will provide you with a comprehensive Fusion 360 tutorial on how to get started. Stay with us and start learning and practicing the Fusion 360.

Different Versions of Autodesk Fusion

Before starting the tutorial, you should be familiar with the different versions of Autodesk Fusion. Fusion is offered in two variations: Autodesk Fusion for personal use and Autodesk Fusion. In the free version, you can access all necessary 3D modeling tools. But if you want access to advanced features like simulation and 3D rendering, please buy the license from the Autodesk website.

We have created a small comparison table between these two versions. Please read it carefully before making up your mind to buy the desired version.

Autodesk Fusion Tutorial: Download and Setup

We have discussed the differences between the free and paid versions in the above section. Now, the question is how to get Fusion 360. Fortunately, Fusion 360 is a software that is compatible with both Windows and Mac. Before moving on, please check the hardware and system requirements. The application is currently unavailable for Linux; however, there are a few workarounds for Unix users.

Fusion 360 offers free educational licenses for students and instructors. You can also acquire a personal license by signing up on Autodesk’s official site and activating it to download the program.

The installation process is simple and easy. After installation, open the program and sign in to your Autodesk account to use Fusion 360. Below is a simple guide on how to download the software.

【2025】How to download Fusion for Free | Creating an Account

Understanding the Autodesk Fusion User-Interface

Let us have some discussion on the user interface of Autodesk Fusion 360. It might seem complex and intimidating at the beginning, but once you dive into it, you will quickly see that things become simple and easy. The main UI looks like the image shown above.

Let’s explore a few of the UI’s primary sections:

1. Data Panel: In this section, users can manage and access their designs and projects and upload local models to the cloud for team collaboration.
2. Toolbar: The toolbar is located at the top of the interface, where you can view and access the essential tools to create 2D and 3D models. If you click on the drop-down arrows, you’ll see a list of all the commands available in each tab and category. The shortcuts shown on the toolbar can all be customized.
3. Browser: In the top-left corner of the viewport, you’ll find a list of all your components, bodies, and construction planes organized in a file tree structure. You can select items by clicking on their names and rename them by double-clicking. Use the triangles on the left to expand or collapse folders, and the lightbulb icon to show or hide bodies and planes.
4. Navigation bar: These tools allow you to adjust the display and move the view manually. There are also handy shortcuts using a mouse, which we suggest trying to move around in 3D space: Zoom, Pan, and Orbit.
5. Timeline bar: This bar is located at the bottom of the interface and is an important part of the software. This section keeps a track record of all the steps taken to create or modify the model. So, you can go back to any step to make changes to your models.

Autodesk Fusion Tutorial: Creating a Model

In order to show you how to use Fusion 360, we will create a simplified model of the Geneva Wheel Mechanism. In most cases, you have to create one or more sketches to start the 3D modeling process. These sketches are then extruded into a solid shape for further necessary editing or modification.

Fusion 360 has a large library of features, but we will cover only a few of those basic features. These features allow you to create many types of models and are more than enough to help you get started with Fusion 360.

Before officially starting the tutorial, keep one thing in mind in this tutorial, we will be using the metric system for dimensions, but you are not restricted to using metric; you can use any unit system. To change default dimension units, go to the document settings and change the units.

【2025】How to Use Fusion 360: A Beginner’s Guide to Getting Started

Sketching

The Sketch entity is a 2D drawing that acts as a base to be transformed into a three-dimensional drawing. Almost every 3D model starts by drawing a 2D sketch, so we can say that this entity is one of the most important features in any CAD software.

With that in mind, it’s only fair that we start by exploring Sketch and some of its tools. Let’s begin by drawing a 2D profile of the main body, or chassis. To do that, we’ll first need to select a surface or one of the starting planes to draw a simple rectangle.

With that in mind, it is essential to start exploring Sketch and some of its tools. We will begin by drawing a 2D profile of the main body/parts. For this, we will select a starting plane to start the process.

Drawing the Follower Sketch

Start by creating a new component, “Follower”. Keep the component active and click OK. Select the top plane to start designing.

Line and Circle Command

The following are a few more steps on how to complete the sketch.

• Draw a 10-cm-diameter circle and select the line command. Keep the line command in construction mode. Now, draw two lines of 5 cm at angles of 54 degrees and 126 degrees.
• Now, draw a construction circle vertically aligned with the origin.
• Select the two construction lines and hit the “Lock” icon to fix them at their places.
• Now, go to tangent constraint and select the construction circle and a construction line. So they will be in tangent. Repeat this process with the other line.
• After doing the above step, select the sketch dimension command and place the dimensions as shown in the image.
• Now, turn off the construction mode and draw another circle of 6 cm diameter at the center of the construction circle drawn earlier.
• Now, go to “Create,” find the “slot” command, select “center-to-center slot,” and select the line (at a 54-degree angle). Select any point on the line and move it to the intersection to draw the slot. The slot diameter is 0.75 cm. Also, the inclined distance between the slot and the origin should be 2 cm.
• Now mirror the slot on the other construction line by selecting the “Circular Pattern” tool. Double-click on the slot and select origin as center. Change the quantity to 5 and press Enter.
• Now draw a circle of 1.5 cm diameter at the origin.
• The sketch is drawn completely. Lastly, we need to trim the unnecessary lines and geometries. For this, we use the “Trim” command. Click the trim command icon and remove the unnecessary details.
• Select the “circular pattern” command. Select the arc and set the origin as the center point for the object. Also, change the quantity to 5 and press OK. Go to the trim command again and remove the unnecessary portions

After doing the above steps, finish the sketch.

Extrude Command

Before proceeding, let’s discuss the extrude feature. Extrude is one of the most used tools in 3D modeling, and it is available in all CAD software. This command pulls a 2D design along a predetermined path to turn it into a 3D shape. Its primary features include:

• Adding depth to sketches.
• Removing material from objects.
• Creating surfaces easily.
• Building basic part shapes.
• Versatile design tool.

Extruding the sketch

Now, it’s time to go 3D! In this section, we will learn to use and practice this command. So stay with us and follow the simple and easy steps.

• Simply go to the Extrude command and select the 2D sketch. Extrude the sketch to 0.50 cm.
• Go to modify and select the chamfer command and apply chamfer at the edges (keep chamfer distance = 2 cm).

Our follower is ready.

Creating Other Parts

Now, we will create a CAM for the Geneva wheel mechanism. Below is the step-by-step process to follow:

• After creating the follower, go to the main assembly and create a new component. Give it any name you want. We will name this tutorial “CAM.” Remember to check the “activate” box and click OK.
• Select the top plane and create a new sketch. On the left side, click on Follower and turn on the previous sketch.
• Now, go to the “project” and select the construction circle. Turn on the projection link and hit the OK button.
• Select the Circle command and draw three circles of diameters of 6.5 cm, 6 cm, and 1.5 cm, respectively.
• After that, draw a circle vertically aligned with the origin of the construction circle. Keep the diameter of the circle 0.75 cm.
• Draw two lines tangent to the 6.5 cm diameter circle from both sides, vertically aligned from the origin. Go to the tangent command, select the 6.5 cm circle, and then select a line to make them tangent. Do the same process for the second line as well.
• Select the “Horizontal/Vertical” icon, then choose the origin and other points to align them vertically.
• Now, go to sketch dimensions and place the accurate dimensions.
• Select the corner and place the fillet of 0.5 cm radius.
• Select the 3-point arc command and draw it anywhere at a 6 cm circle (already drawn.)
• After that, assign a vertical dimension between the center of the construction circle and the edge of the arc. Keep the distance of 2 cm and finish sketching.

Extrusion

We will extrude the selected profiles downward and upward to make new and joined bodies with accuracy.

• Extrude the sketch by selecting the Extrude command and selecting the profiles as shown in the figure above. Extrude these profiles downward up to -0.5 cm. Select New Body in the operation box.
• Now, turn on the visibility of the “CAM” sketch and use the extrude command to extrude the remaining profiles up to 0.5 cm, upward. Select “Join” in the operation.

Assembly

We have created all the parts of our tutorial design. The last step is to assemble our design. Before starting this procedure, let’s have a short and brief introduction to assembly. Assembly is a 3D model that is made by combining different parts together to achieve a desired output. A machine is made by assembling multiple parts together. Assemblies are used to design complex systems and products like vehicles, machinery, and aerospace structures.

Now, we are going to assemble all the parts of the Geneva Wheel mechanism to complete our tutorial. So, follow these steps and enjoy your first 3D model.

Assembling the parts

Everything from creating the follower to creating the CAM part of the mechanism is done, and now it’s time to assemble them. Let’s follow the necessary steps and get the work done.

• Before assigning any joints between them, we need to provide support. For this, go to “Create” and select the “Cylinder” option. Select the surface of the follower and draw a circle with a diameter of 1.5 cm. Then, extrude this circle downwards to 2 cm in length. The operation should be “New Component.” Click OK. Also, right-click on the cylindrical component and make a new copy.
• Click on any component, say the cylindrical component, and make it ground. So, this will not move from its original position while other components are free to move.
• Go to “Joint.” For component 1, select the circular face of the follower, and for component 2, select the face of the axis. The motion type is revolute.
• Again, go to “Joint,” and for Component 1, select the circular face of the CAM, and for Component 2, select the face of the remaining cylinder. Right-click on the second cylinder and make it ground.
• Go to the move command and change the “move object” to components. Select the follower and move it at an angle of 36 degrees.
  Now, here is an issue: if we move our components, they overlap each other. To fix this, go to assemble and enable all contacts.

FAQ

Here are some common questions about getting started with Fusion 360, answered in simple terms:

Conclusion

By completing this tutorial, congratulations on your first CAD model in Fusion 360. We made a fun model using simple tools. Think of all the other models you can create with just these basic tools; we’ve only just started! If you encounter any difficulties while following this tutorial, you can refer to the video provided above in the article.

You must now realize how easy it is to use Autodesk Fusion. It just needs practice and dedication to improve your skills in 3D modeling and rendering. We suggest you check out other articles, watch tutorial videos on YouTube, and stay consistent in your practice. If you want to excel in Fusion, you can also take online courses on platforms like Coursera and Udemy.

Although we haven’t covered all the tools in this tutorial, we hope you’ve learned something from it. We also hope that after this tutorial, your interest in learning Fusion 360 has grown!