Using Fusion 360 to Design Complex PCB Shapes in Eagle CAD
When designing PCBs in Autodesk Eagle, it is relatively easy to create board designs with simple geometric shapes: rectangles, circles, polygons, and other simple shapes are easy to create using the line tool in Eagle. Creating simple variations on these shapes is also quite simple: squares with rounded corners, pill shapes, rectangles with cutouts, and many other designs are not too difficult to create.
However, what if you need to design a highly complex PCB shape in Eagle?
Here’s an example of one such PCB design. A couple months ago, I built a hexapod robot named Capers II. I am very proud of that project and I’ve received quite a bit of positive feedback about the robot. However, building a full-scale hexapod robot like Capers II is quite expensive – just the servos alone cost about $600 before adding the frame and electronics. So, for that reason and several others, I decided to embark on a new robotics project, building another hexapod robot that is much smaller, and much cheaper to build, than Capers II.
One issue with miniaturizing the robot is that the electronics stack used on Capers II is quite big all on its own. Therefore, for the miniature version, I decided to build a new controller board that would pull double-duty as the actual structure of the robot. In other words, the robot will basically be a walking PCB. So here we come to the subject of this post. The outline dimension of the robot’s controller PCB will look like the image below.
So, while it would certainly be possible to plot out the Cartesian coordinates for each of the vertices and circle centers in this design, and then input those one by one into the command interface in Eagle, this would be an extremely tedious process. Plus, it would be difficult to make any changes to iterate on the design.
Fortunately, you can use Autodesk Fusion 360 to design the board outline and then, with a simple procedure, move that design into Eagle. This way, your mechanical design work can take place in a software designed for that purpose, and your electronics design work can be done in Eagle, without having to mess around with its slightly clunky dimensional design tools.
Let’s get started.
- 1) Design your Board in Fusion 360
- 2) Create a Complete Outline Sketch
- 3) Export the Sketch as DXF
- 4) Import the DXF into Eagle
- 5) Replace Circles with Holes
1) Design your Board in Fusion 360
Of course, the first step in the process of using Fusion 360 to create complex PCB outlines in Eagle is to create your design in Fusion 360. For the most part, you can use the sketching tools in Fusion 360 to create whatever shape you need for your project. Creating your board outline using Fusion 360 is much, much easier than creating complex shapes in Eagle because the tools in Fusion 360 are so much easier to use.
For the example in this post, the miniature version of the Capers II robot, the PCB outline designed in Fusion 360 looks like the image below.
This is a design, made in Fusion 360, for the PCB for a robot project. The complex shape means this design would be extremely difficult to create using Eagle.
One of the other benefits of using Fusion 360 to design your PCB board outline is that you can extrude that outline in order to virtually build your project and verify that all the parts of your design fit together the way you want before ordering your PCBs.
Constraints
Fusion 360 gives you the ability to create an near-infinite range of different designs. However, you should always be aware of constraints imposed on your project by the PCB fab house you wish to use. Every PCB fabricator will publish a list of design requirements, as well as a list of features their processes will be unable to create. Some of the items to consider are maximum and minimum board sizes, maximum and minimum hole sizes, internal cutout capabilities, plated slot capabilities, board thicknesses available, drill size delineations, milling capabilities, and more.
Be sure to check out the design rules for your PCB fabricator of choice before completing your design work in Fusion 360. Below are a few examples:
2) Create a Complete Outline Sketch
Before we will be able to convert the PCB design in Fusion 360 to the dimension layer in Eagle, we will need a single sketch in Fusion 360 that contains the entire perimeter of the PCB design plus any internal features, like holes, cutouts, or slots. Assuming that you’ve used several different sketches in Fusion 360 to create your PCB design, the easiest way to get the sketch needed for this guide is to start a new sketch and re-draw all the features in the design.
Let’s start with the perimeter of the PCB design. There is a useful tool in Fusion 360 that will allow us to trace the outline of the PCB with only a few clicks. First, start a new sketch on the top of the PCB design. Then, open the Offset tool, located in Sketch > Offset, or by pressing O.
The offset tool allows you to replicate sections of your design and expand or contract the new sketch profile from the original outline. In this case, however, we do not want any offset, so simply set the offset perimeter in the Offset tool to zero.
You can use the offset tool with an offset value of 0 to quickly create a sketch of the outer perimeter of your design.
As for any other internal features, you can use the Offset tool set to a zero offset again for any complex features. Otherwise, for simple features like holes or slots, it is easiest just to use the corresponding sketch tool to trace those features.
By the time you are done, you should have a sketch with the outline of your PCB design along with any internal features.
3) Export the Sketch as DXF
Now that we’ve created a complete outline sketch of the PCB design in Fusion 360, we will need to convert that sketch into a format Eagle can understand. So, in the file browser in Fusion 360, locate the sketch you just made of the entire PCB outline and all its internal features. Right click on the sketch and select Save as DXF. A DXF file is a CAD file format developed by Autodesk that is designed for compatibility among different programs.
Then, simply choose a location to save the DXF file.
4) Import the DXF into Eagle
Our work in Fusion 360 is done. Now, open up Eagle. You will also want to either open up a pre-existing design or create a new BRD file.
Importing the DXF generated from Fusion 360 into Eagle will be done with a User Language Program (ULP). ULPs are one of the features that make Eagle such a powerful PCB design tool. ULPs are scripts created by the community that give Eagle much, much more functionality. ULPs can do all kinds of things, but for this tutorial, we will be using a ULP design to import DXF files. So first, click the ULP button in the Eagle toolbar.
You will be presented with all the available ULPs, and there are many. The one we need today is import-dxf. So, find that ULP in the list or search for it, and press OK.
Next, click the browse button and find the DXF file you created earlier.
Make sure the ULP is targeting the dimension layer. In the Target Layer dropdown, select 20 Dimension if it is not selected automatically. Finally, click OK and then, in the next window, press Run.
5) Replace Circles with Holes
By this point, you should have a dimension layer in Eagle matching your PCB design from Fusion 360.
It looks great. However, even though the dimension layer is totally accurate to the original design, there is still an issue. If you have any internal features, like the holes in the design above, you will need to replace this with the correct feature in Eagle. For example, the circles on the dimension layer need to be replaced by using the holes feature in Eagle.
So, start by selecting the Hole tool in Eagle.
Next, we will need to set the diameter of the tool to match the diameter of the holes in your design. If you don’t know the diameter of your holes, you can always hop back into Fusion 360 and use the Measure tool to find out. Anyway, to set the dimension of your Hole tool, type in the diameter of the hole, with units as well, into the Drill field.
Next, place the hole near the circle it will replace. Don’t worry about positioning the hole in exactly the correct position. We will re-position the hole in a moment. In order to place the hole directly on top of the circle, we will first need to determine the coordinates of the circle. Select the Info tool in Eagle.
With the Info tool, click on one of the circles you are trying to replace with a hole. The Info tool will show you the coordinates of this circle. You might want to write down the values because you will need them again in a moment.
With the circle’s dimensions recorded, use the Info tool on the hole you are moving. Again the Info tool will give you the coordinates of the hole. Replace these coordinates with the coordinates of the circle you recorded earlier.
When you press OK, the hole will move directly on top of the circle.
Conclusion
By using Fusion 360 and Eagle together, you can create highly complex PCB designs. Fusion 360 handles the dimension design using tools designed for creating mechanical designs. By importing the design into Eagle from Fusion 360, you don’t need to deal with the cumbersome drawing tools in Eagle. Instead, your efforts in Eagle can be focused on the electronics design.
0 Comments