If you've made it this far, you actually have a fully functional package that you can connect up to any schematic symbol, and place it on your board.

Go ahead, pat yourself on the back! You've done the bare minimum of sizing and placing a set of appropriately named pads, and organizing them in a single package, which is the main requirement to move on to the next stage, creating a symbol for your schematic.

That said ... you'll thank yourself later for putting a bit of extra effort into things now. Accurate footprints are about more than a few pads and proper names.

Now it's time to add in some basic mechanical details, and later to make sure we have a way of identifying our parts once they get place on our PCB!

Before we can do that, though ... we need to make an important detour into something fundamental to working in Eagle ...

Decidedly Not Your Eagle BFF: An Introduction to Layers

Layers are an essential part of Eagle. They're allow us to organize the many types of information that are required to make a PCB, and generate the documentation that we can share with other engineers or companies.

Layers are what allows us to generate the files that board houses can manufacture PCBs from.

That said, Layers is one of the more complicated things to wrap your head around if you're new to Eagle, so we'll try to explain the basics here.

Common Layers for Packages

Each 'layer' in Eagle has a dedicated number, and these layers are used to separate all the types of content that make up your PCB or your parts:

These layers contain documentation details (layer 51), actual manufacturing info such as the 'paste layer' (layer 31), the copper layers for you pads (layer 1), etc.

Since each layer has it's own dedicated functions, it's important that you use the right layer for the right type of information!

Many tools in Eagle use layers for many different things, and thankfully they generally select the most appropriate layer by default, but for reference sake we generally the following 'layers' when designing packages:
  • The Smd tool (to create pads) generally uses layer 1 to indicate which side of your PCB the pad should be placed on, though in very rare circumstances you may need to use layer 16 as well:
    • Layer 1 (Top) is used to draw pads on the top of the PCB
    • Layer 16 (Bottom) is used to draw pads on the bottom of the PCB
    • On multi-layer boards with the professional version of Eagle, you also have access to layers 2-15, but we won't worry about these for now
  • The Line Tool can draw lines on any layer, but we'll see shortly there are two layers that are particularly important with this tool:
    • Layer 21 (tPlace), which is used to draw lines that will be rendered as the silk screen on your PCBs (the printed text/lines/shapes we see)
    • Layer t51 (tDocu) is used for documentation purposes, such as drawing the mechanical dimensions of your part (more on that shortly!). Normally this layer isn't printed on the PCBs, but it's very important for documentation and for PCB design.

  • When assigning Names and Values to packages (more on that shortly as well!), the following layers are used:
    • Layer 25 (tNames) is used to hold the unique 'names' for each part on your PCB (ex. C1, R5, X12, etc.)
    • Layer 27 (tValues) is used to hold the value for each part (such as 10K, 0.1µF, AT86RF212, etc.)
We'll cover these and other layers on an as-needed basis, and this will start to make sense once you work with them, but for now these are the main ones to familiarize yourself with.

Navigating Through Layers

The only important thing to know now, aside from having a general idea of what layers are, is how to switch between layers when you need to.

Any tool that works with different layers will expose the same 'Layer Selection' drop-down box in the tool's command bar up in the top right-hand corner. You can see the drop-down box after selecting the line tool, for example, which will default to layer 21, which is the silk-screen for the top of your PCB.

We've extended the drop-down list out just for reference sake so that you can see some of the other layers you can select with this tool:
The best way to understand layers, though, is to start using them, so lets backtrack from this little side-route, and finish up the last little details of our new package!
Eagle is full of little shortcuts, and we can't cover them all here without overwhelming people, but one useful shortcut with the layer selection drop down is that you can select your tool (the line tool, for example), move your mouse over the layer selection box, and use the scroll wheel on your mouse to select layers. If you're switching between later 1 (top copper) and later 16 (bottom copper) this can save a lot of time.

This guide was first published on Apr 22, 2013. It was last updated on Mar 08, 2024.

This page (An Introduction to Layers in Eagle) was last updated on Apr 16, 2013.

Text editor powered by tinymce.