This is my first post in what will probably be 4 parts on Eagle CAD’s libraries. I’m not going to give a step by step beginner’s tutorial on using Eagle CAD libraries. That is covered elsewhere. Just Google “eagle cad tutorial”, or go straight to the Eagle CAD tutorials on Sparkfun.
I’m planing to cover libraries at a level slightly above beginner that should help you build your own personal parts library that will be easy to use and save you time in the long run.
Eagle CAD 6 was recently released. I haven’t used version 6 yet, but I believe most if not all of this information will remain useful.
Note that I may use the word “footprint” where Eagle CAD uses the word “package”. Either way, this is the physical representation of the PCB layers used for layout.
Also, I use “PTH” for through hole, and “SMT” for surface mount (but you knew that already, right?)
Use existing parts from other libraries with caution
My first recommendation is to not blindly trust library parts created by others. The problem is that I have found way too many errors in libraries created by others. You might think that since someone else has a working design using a part from the library, that the part must be right. While it is a good sign, the reality is they may have corrected an issue in their copy of the library, or worked around it somehow.
So I check any part I use for the first time from another source very carefully. It takes some time to do a thorough check, but it is far less time than you will loose if you have PCB’s built with errors.
Finding the right part
There are a lot of libraries supplied with Eagle CAD and available for download from Cadsoft. Sparkfun and Adafruit also make their libraries available for free. It can take a lot of time to manually look for a part that may already be in one of those many libraries.
ESawdust created an online search tool that can help you find parts in those three sets libraries. It is a huge time saver and I use it often. I don’t know if he is keeping it up to date with new parts and libraries.
Get the datasheet
I start a design by downloading the datasheets for parts I am going to use in my project. Usually near the top of the datasheet you will find pinout information, and near the bottom you will find the package dimensions and sometimes a recommended footprint.
The manufacturer’s recommended footprint is meant for volume production on automated machinery. I will take it as a starting point, but I usually increase the pad sizes for hand assembly, to give me more pad to touch with the soldering iron. This is especially true for SMT parts.
Here are the steps I go through to check a part from someone else’s library before I use the part:
Library part reuse checklist
Open the library and find the Device.
Check that the schematic symbol looks OK.
Look at the packages that have been defined. If they have the right one for your project, open it in the library editor.
Check the >NAME and >VALUE text. When placed on the schematic, Name is replaced with the reference designator (“U1”). Value is replaced with a value you enter (“1 uf”) or the name (“2N2222”) of the part.
Size of text should be at least 0.032 inches – typical for SMT parts. I prefer 0.05 inches for PTH. You can shrink it in your layout later if it is too big.
For small text, proportional or vector font doesn’t matter. During layout, if you change the text size to above 0.05 inches, you should also change the font to vector. Vector font is more accurate in size when translated to Gerber format.
- Check the pad sizes against the datasheet.
- For SMT parts, the pad needs to be longer than the pin if you are going to do hand soldering. A bare minimum for me is 0.5 mm, 1 mm is better.
- For PTH parts, the hole size is usually 0.031 (DIP, low watt resistors and capacitors) or 0.043 inches (high watt resistor or transistor, headers), depending on the size of the lead. It should not be a tight fit unless it is a mechanical guide pin, for example on on a connector.
- Pad Thermals and Stop boxes should be checked. For SMT parts, Cream should also be checked.
- Check the XY locations of the pads carefully for the correct spacing. Through hole (PTH) parts are usually easy as they are on 0.1” centers. SMT parts usually require switching View > Grid to mm with size 0.1. Use the “Mark” tool to check relative spacing.
- Check that the number order (or name) of each pad matches the datasheet.
- Check the silkscreen, layer 21, tPlace. The silkscreen needs to help you correctly locate each part and find pin 1 during assembly and debug.
- I like to have a nice outline of the part in layer 51, tDocu. I print this layer out as a guide while I’m assembling boards. It can also help guide you during layout parts placement, especially big parts such as connectors that have bodies much larger than the pads indicate.
- Layer 39, tKeepout, is used by the DRC function to check that parts are not too close. Many parts don’t have it. Normally, I lay out through hole parts with plenty of spacing. If I am doing an SMT board that is tight on space, I use tKeepout to make sure I have left enough room for my tweezers. So my SMT parts (usually) have tKeepout.
Yes, that’s a long list, but I’ve found every one of the problems listed above on more than one part. Most parts I check have some issue from that list that I fix before it goes into my projects.
Pad size, location, and pin order are of course the most critical. Do not assume they are right!
The rest of the list are issues that will be like a pebble in your shoe as you try to create your PCB designs.