The final step in making a relatively complete symbol is adding a little bit of information about the pins themselves.
This step isn't strictly necessary, but it can be useful in certain situations, and it's worth spending a minute or two adding this one last touch before moving on to the final step in the device design process.

Setting Pin Directions

It can be useful to say what direction or function a pin serves, particularly if you make use of some of the rules checking functionality in Eagle to validate your schematic and board files.

Eagle defines a number of possible pin directions, which we can see by right-clicking on any pin and selecting the properties window, and then expanding the 'Direction' drop down list, as shown below:
Not all of these direction are commonly used, but the important ones that you should be concerned with are:

  • nc - For 'Not Connected', which is used to indicate that this pin should not be connected to anything on your schematic. Assigning a pin as 'NC' will allow Eagle to warn us if you mistakenly connect something this this pin.
  • in - For input pins
  • out - For output pins
  • io - Pin is bi-directional (input and output) * This is the default pin direction!
  • pwr - For VCC, VDD, VSS, GND, VBUS, VIN, VBAT, and similar 'power' pins
  • pas - For pins on passive parts like resistors and capacitors (no often used creating custom parts)
To set the pin direction, just right-click on every pin and select the 'Properties' option, then set the direction in the properties dialogue box. In the case of the GA1A1S202WP, we would set the direction as follows:
  • Set VSS, GND@1 and GND@2 to 'pwr'
  • Set IO to 'out', since this is actually the analog output on our device
This will give you something resembling the following on our updated symbol:

Adjusting Pin Length (Optional)

This is purely a cosmetic step, but if you wish you can also make the pins larger or smaller. My own preference is to set the pins to 'short' (the default, shown in the image above, is 'middle').

If you want to, you can change the length in the properties window. Whatever size you decide to work with, though, you should try to be consistent about keeping the same length throughout your library.

You can see the results of setting the pin length to short in the image below:
That's it! We've made a complete schematic symbol representing our part, and we're ready to move on to the final step in the part design process, connecting out symbol and our package in the device editor!

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

This page (Final Pin Adjustments) was last updated on Apr 22, 2013.

Text editor powered by tinymce.