Using Fusion 360 for PCB Design
Clarus Goldsmith, June 2024
Last updated
Clarus Goldsmith, June 2024
Last updated
Some PCB manufacturers will have board specifications that describe their manufacturing capability. Typically these specifications set minimum (or maximum) sizes for parameters, such as the minimum trace width, minimum trace spacing, or minimum drill size. These specifications will be available on the manufacturer's website, such as the ones for a 2-layer board from OSH Park given below. It's important to consider the specifications of the manufacturer you're going to send your PCB to while you're laying out the board.
In Fusion 360, these specifications are called Design Rules. They can be accessed from the 'Rules DRC/ERC' tab in the 'PCB document' window of your design (the one where you lay the components out on the board). Specifically, click on the green checkmark with 'DRC' above it to edit the design's design rules.
You will likely not need to mess with the design rules most of the time, and if you do, you'll only need to change a few of them. Here are a few of the common reasons you'd need to change a design rule.
You may need to adjust the copper weight of your board for higher load applications, such as if you're making a power distribution board for a robot. You can do so under the 'Layer Stack' tab of the DRC window. You will need to check the 'Edit material properties' box before you can edit the 'Weight' column. In this tab, you can also add layers to your board.
As you can see in OSH Park's design rules above, manufacturers will often specify a minimum amount of space components can have between them (e.g., trace width). This ensures that traces don't accidentally get connected together while the copper is being milled out. You can change spacing parameters like trace width in the 'Clearance' tab of the DRC window. It's generally a good idea to set Wire-Wire, Via-Wire, and Via-Pad clearances to at least 10 mil, particularly if you're prototyping through places like the Innovation Hub with more limited manufacturing capability.
The Innovation Hub uses rivets to create vias and plated through holes, and these are the only sizes they have.
Suggested minimum trace width
12 mil (~0.3 mm)
Plated through hole diameter
59 mil (1.5 mm)
Via diameter
27.56 mil (0.7 mm)
Some manufacturers, such as OSH Park, provide Design Rule files specifically for use in Fusion 360. This way you can just import the file instead of manually setting all of the design rules individually.
To import these .dru files into Fusion 360, open the DRC window. On the 'File' tab, click on the 'Load...' button in the bottom right corner. In this new window, click on 'Browse...' In this new file explorer window, change the type of file to 'Eagle Design Rules (*.dru)' in the dropdown next to the 'File Name:' bar, then navigate to where the .dru file is stored and select it.
Opening this file will import the Design Rules into your current PCB design. You can then click, 'Apply' to reformat your board with these new Design Rules.
If you're applying new Rules to a board that has already been laid out with other Rules, there may be errors (such as floating traces or extra trace lengths). You can see these in the 'Errors' tab and make any necessary changes as needed.
Fusion 360 has a large number of libraries available that allow you to include different components' schematic icon, board footprint, and 3D model into your design easily. However, they don't have every component out there. Sometimes you may have a specific component you want to use in your design that isn't in any of Fusion's libraries. When that happens, you can include these components by making your own custom library.
To do so, first find your desired component on a website such as Digikey or Mouser. On the product page, there will be a line item called, "EDA/CAD Models."
Clicking on this will take you to the website's selection of footprints and models for the component. You can download any of the options available. When choosing download format, select 'Fusion360 PCB' and 'STEP' as your options.
Once your download is complete, extract the ZIP file in your Downloads folder and open the .lbr file contained inside from within Fusion 360. This will allow you to edit the contents of a Library containing only this component. You can then save this Library anywhere in your Fusion Cloud and it'll be available to use in any of your electronic schematics.
Importing the .lbr as above adds a schematic symbol and a footprint for the component. However, there are a few extra steps required to also include a 3D CAD package such that it looks like the actual component on a 3D PCB rendering.
First, open the STEP File you downloaded with the .lbr file earlier in Fusion 360. Save it somewhere on your Fusion Cloud.
Next, in the Library you've created for your component, find the footprint you want to add the 3D package to and right click it. Select, 'Create New 3D Model.'
This will open a tab with the footprint of the component laid out with green-dashed lines. Save this new file in the same place as the STEP file. Click on the 3x3 grid icon in the top left corner to open the Data Panel, then navigate to where you saved the STEP file. Right click on the STEP file and select 'Insert into Current Design.'
This will add the 3D model into the file, typically right on top of the footprint. For some models you may need to orient the model to properly sit on the footprint. Once that's complete, like on the green and white 'Finish' checkmark. This will take you back to the Library window, with the 3D model tied to this footprint as a Package.
In some cases, components will have multiple footprint variations. However, the component's package will be the same across these variations. In this case, you can attach the 3D model from one variation to another by right clicking on that footprint and selecting, 'Attach Copy of Existing 3D Model,' then selecting the other footprint in the menu.
Once your 3D models have all been added, save the library to use it in your designs. If you updated an existing library that you were already using in a design, you will need to refresh the library in that design. To do so, go to the 'Library' tab in the Schematic Document and select, 'Update design from all libraries used in this design.'
To export the files necessary to actually make your PCB, go to the 'Manufacturing' tab in the PCB document. You can first double check that all of the files look like you would expect by clicking on the 'CAM Processor' icon.
In the CAM Processor window, the Gerber files are what we're interested in, as these are the types of files most manufacturers use to create a PCB. You can view each file to double check that all of the traces, through holes, and silkscreen drawings appear as they should. Then, close the window.
To actually export the necessary Gerber files, click on the 'Export Gerber, NC Drill, Assembly and Drawing Outputs' Icon.
Click 'OK' on the first window, then choose where you'd like to save the ZIP of CAM files. Then click 'Save.' You can then upload this ZIP file to your PCB manufacturer of choice's website to preview the finished board and pay for them to make it.
