Eagle library for Arduino Pro Mini

Background

While building a portable FM receiver I have just noticed that there are no Eagle library for the Arduino Pro Mini devices. Or at least I wasn't able to find one when I searched for. Since creating a new Eagle library is not a big deal I decided to give it a try, so here we go.

@Edit: later I found that there are some Arduino Eagle libraries available at Autodesk website -> Support -> Libraries. However, it was fun to reinvent the wheel 🙂

The Basics

Whenever you want to create a new reusable Eagle part you must enclose it within an Eagle library. An Eagle library (*.lbr) encapsulates three components:

• the symbol - is what you see on your Eagle schematics
• the package - is what you see on your Eagle board (the PCB footprint)
• the device - is a mapping between of pins-pads of the two above

Creating an Eagle library for Arduino Pro Mini

The following is a log of the steps I've done for creating the Eagle library for Arduino Pro Mini:

1. open Eagle Control Panel, go to Projects->eagle and then create New Folder with the name Arduino
2. from the Eagle Control Panel open the menu File->New->Library; a new Library document is opened; Save As : arduino-pro-mini.lbr
3. open the menu Library->Manage symbols and create new symbol with the name ARDUINOMINI
4. open the menu Library->Manage packages and create new package with the name ARDUINOMINI
5. open the menu Library->Manage devices and create new device with the name ARDUINOMINI
6. at this the library editor is ready waiting for us creating/drawing the new device
   • 
7. now we want to open the newly created ARDUINOMINI symbol; click the symbol on the Symbol list then right-click and choose Edit option; the Symbol Editor will open and there we will be able to design the schematic symbol for the new device
8. select the Draw->Line option for drawing the frame of the device; draw a rectangle with the height=13 sqares and the width=6 squares
9. select the Draw->Pin option for drawing the pins of the device (Visible=pin); draw 12 pins along the height-side and 6 pins along the width-side (on the top)
10. select the Edit->Name option for renaming the pin's names; rename the pins according to the Arduino Pro Mini pinout layout
11. add a text ">NAME" with Layer attribute="Name"; optionally add another text "Arduino Pro - Mini" rotated 90CCW
    • 
12. now we want to open the corresponding ARDUINOMINI package. This will be the part footprint as printed on a PCB board. Select Library->Manage packages then select the ARDUINOMINI package; the Package Editor will open and there we will be able to design the board layout for the new device
13. make sure you set the grid unit to 1.27 mm
14. for each pin add a Draw->Pad element (round)
15. for each pin add a text label with size=0.508 then place the text like in the image below:
    • 
16. now we want to open the corresponding ARDUINOMINI device; select Library->Manage devices then select the ARDUINOMINI device; the Device Editor will open and there we will be able to configure the new device
17. select the Edit->Add menu then choose the ARDUINOMINI symbol; drop the symbol centered on the screen
18. click the New button shown on the panel near the device editor then select the ARDUINOMINI package
19. click the Connect button shown on the panel near the device editor then, for each pin-pad tuple create a connection by selecting the pin and respectively the pad then clicking the Connect button
20. click the Prefix button shown on the panel near the device editor then specify a prefix (eg. "AR") for the device; make sure you check the "On" value too
21. save all changes when done; make sure you use the new library in your schematic otherwise you won't be able to find the new package (under the name arduino-pro-mini)
22. now we can use the new device in an Eagle schematic!

Here is an Eagle schematic using the newly created Arduino Pro Mini device:

Source code

The Eagle library source code (*.lbr) was released to public domain under the GNU GPL v3 license.

The Arduino Pro Mini Eagle library source code is available at Github. However, you may find useful some other libraries created by different people (check the Autodesk Eagle support libraries).

Now, if you think that this article was interesting don't forget to rate it. It shows me that you care and thus I will continue write about these things.

The following two tabs change content below.

• Bio
• Latest Posts

Eugen Mihailescu

Founder/programmer/one-man-show at Cubique Software

Always looking to learn more about *nix world, about the fundamental concepts of math, physics, electronics. I am also passionate about programming, database and systems administration. 16+ yrs experience in software development, designing enterprise systems, IT support and troubleshooting.

Latest posts by Eugen Mihailescu (see all)

• Dual monitor setup in Xfce - January 9, 2019
• Gentoo AMD Ryzen stabilizator - April 29, 2018
• Symfony Compile Error Failed opening required Proxies - January 22, 2018