Correctly sizing and placing your pads is the most critical part of the footprint design process, so you'll want to be sure you understand this section very well!
Now that you know how to create a pad, it's time to learn how to properly size them and position them.

Before we can go any further, you'll need to pull out the GA1A1S202WP datasheet (or whatever other datasheet), and find the package outline. It's usually on the last couple pages of any datasheet, but in the case of this part it's on page 6 of the PDF.

For convenience sake, we've included a screenshot of the package outline below:
Everything that we need to know to create our package is on this page, and it's important to become familiar with how these package drawings work.

There are two important elements that we need to take into account create a package:

  1. The package 'dimensions', which is the physical outline of the package. We'll come back to this one later.
  2. The pad locations and sizes, which are the metal pads we will creates where to 'leads' or 'contacts' on your part will get soldered to your PCB.

Sizing Your Pad(s)

The first step we'll do to actually start creating a package for our sensor, is to start laying down the pads in the right size and location.

There are four pads on this part, represented by the four dark, hatched squares in the diagram.
Most manufacturers include a 'recommended footprint pattern', showing the suggested size for your pads. Be sure to follow these suggestions as closesly as possible when they are present.
Looking at the recommended footprint, we can see that this part has four identical pads, and the manufacturer suggests a pad size of 0.6 x 0.6mm.

To create a 0.6 x 0.6mm pad, we need to click the 'pad placement' tool we discovered in the previous page (the 'Smd' tool in the left-hand toolbar), and then adjust the size of the pad.

Once you've select the Smd tool, a new toolbar will appear at the top of your display with the settings for the new pad(s):
Adjusting the size is easy.

The toolbar contains four items, but we only need to worry about two of them here:
  • Layer Selection: The first drop-down box (shown with '1 Top' here) indicates on which 'layer' our pad should be placed. We'll explain layers later, but for now leave this at '1', which is the top copper layer, and where we want to place our pads 99% of the time.
  • Smd Size: The second box (labelled 'Smd:') is the most important one here. This is where we indicate the size of our new pad. It's currently 1.27 x 0.635.
To change our pad size to 0.6mm wide by 0.6mm high, we just type '0.6 x 0.6' in the 'Smd:' textbox.

Essential Eagle Skills

Side Note on Units and Sizes in Eagle

Do you remember your Eagle BFF from a previous page, the Grid Dialogue? You'll see one reason why this little icon is so important here.

Our pad size in the screenshot above is set to 1.27 wide by 0.635 high, but there are no units specified!

This is because the 'units' in Eagle are controlled via the grid settings, and we are free to switch back and forth between mm, mil, or any other supported unit, and the numbers will be adjusted accordingly.
We see 1.27 x 0.635 now because we are on a '0.1 mm grid'. If you click the grid icon again (dialogue box shown above), you can change the grid units to 'inch', which would cause the default Smd size to be displayed as 0.05 x 0.025, and all of the other numbers in Eagle to be adjust to inches (or mils, etc.).

For now, keep these in mm, though, since 99% of parts today are specified in mm.
This is true of any tool in Eagle, and it's very important to understand this or you can end up with a part in inches when you needed a part in mm!

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

This page (Setting Your Pad Size) was last updated on Apr 16, 2013.

Text editor powered by tinymce.