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 ...
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.
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.)
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: