KiCAD is supplied with extensive Symbol and Footprint (and 3D, not addressed here) libraries.
These are fine for simple, initial use, but inflexible due to their being “read-only”.
KiCAD also, on installation, creates the default libraries and their paths in the “system/program” area of your system,
This means those Kicad default libraries will be overwritten whenever an update or re-installation is made.
Because of the above limitations, almost all users create their own libraries.
Creating personal libraries might seem a daunting task, but really isn’t.
Personal libraries allow you to create, modify, import and use symbols as you like.
Notice the KiCAD library structure: it’s “flat”, no sub-libraries or hierarchies at all, neither in the program itself, nor in the file structure.
It’s highly recommended to stay with this method when organizing personal library file systems.
It’s also essential that your own libraries are in a “user/document” area of your system which can be backed up (like all your other valuable documents).
The first thing to do is to create the folders for your user libraries. Fortunately, you only need two to start with: one for Symbols and one for Footprints.
KiCAD does not care where these folders are created and placed, provided they have both read and write access.
Creation of Personal Libraries.
Take a little time to plan the naming of Personal Libraries. Reorganizing and recreating libraries sometime in the future because of poor original planning is an irksome task.
The Official Kicad Libraries may give some inspiration, however, don’t just name a library “Device” and throw everything into that one library.
When naming libraries, always allow for additional similar libraries to be added.
Eg. Capacitors: There are hundreds of capacitor footprints; much too unwieldy for a single library. Maybe name capacitor footprint libraries: Capacitors_SMD, Capacitors_THT, Capacitors_Electrolytic, etc.
- Many smaller libraries are generally easier to navigate than a few large libraries.
- Many smaller libraries will load quicker than a few large libraries. Refer: KLC
There is no need to create all the libraries thought to be ever needed at once. Create as needed.
To create a Symbol Library:
- Open “Symbol Editor”
- Left click “File”
- Left click “New Library”
- Choose “Global”
- Left click “OK”
A window will open.
The appearance of this window may alter slightly according to your Operating System.
- Name the library (red arrow).
- Do not remove the attachment ( .kicad_sym ) or, if altered, re-type exactly.
- Use the Left hand list (blue rectangle) to navigate to the Personal Kicad Symbol Folder.
- In the example shown, “D” drive holds the Kicad Personal Libraries. “D” drive is accessed through “Other Locations”.
- The path to the new library will show above the Library list (green rectangle).
- All other previously created Personal Symbol Libraries will appear in the box under the title “Name”
A new Symbol Library has been created.
- Left click Save.
The window will disappear and the new Symbol Library will appear in the list of libraries in the Symbol Editor.
The new library has no gray triangle beside its name and does not open. This is because it is empty.
- Left click Preferences > Manage Symbol Libraries.
A window titled Symbol Libraries will open.
- Select Global Libraries.
Scroll to the bottom of the list of libraries to find the newly created personal library.
All personal libraries will show below Kicad official libraries in this window.
Global and Project Libraries.
Libraries stored in Global Libraries are at all times accessible by all projects.
Libraries stored in Project Libraries are only accessible through the project to which they are attached. This means to use a symbol in a future project, that project with its project library (in which the symbol was stored) must be opened and the symbol in question copied to a Global Library to be re-used.
It is more efficient and easier to originally place all created symbols and footprints in Global Libraries and then copy those Symbols to created Project Libraries if and when required.
Project Libraries are created exactly the same way as Global Libraries. Project Libraries will automatically be placed with the project unless steered by the New Library Manager to a place previously created by the Operating System.
Explanation of the Symbol Editor window
Active column: The Active column decides which libraries will be shown in the Symbol Library Browser in the Schematic Editor. Un-ticking a library will remove a library from view in the Browser. This may be of benefit to abbreviate the list of viewed libraries.
Nickname: This governs the position of a library in the Symbol Library Browser list.
The libraries in the Browser are listed in Numeric followed by Alphabetic order. Changing Nicknames can be useful for conveniently relocating personal libraries.
Nicknames can be changed at any time without interfering with Library Paths.
Compare the Nicknames and the Personal Library Names (Cyan Arrows) in the above illustration.
By placing a number preceding the Library Name in the Nickname, the order of the libraries in the Symbol Library Browser change. See below.
- Changing nicknames for Official Kicad Libraries will not work on a permanent basis because each library update will re-install the original Nickname.
Library Path: This shows the complete path Kicad uses to find a library. If a library is moved, the path needs to be changed for Kicad to be able to find that library.
To change the path, either type the new path into this box, or,
Left Click in the box, Left Click on the newly appearing Folder Icon at the Right in this box, then navigate, using the further newly opened “Select a File” window, to your location changed library, then Left Click “Open” followed by Left Click “OK”.
Your new path is now entered.
Library Format: If an imported library is not in the Kicad format it cannot be used by Kicad.
Description: Personal notes on what is in the library.
The Icons below the main table:
"+ Icon" adds a row to type the entry of a new or previously removed Kicad library.
"Folder Icon" opens the same window as “Library Path” to enter a new or previously removed Kicad library.
"Up & Down Arrows" change the location of a library only in this library list.
"Bin" deletes a highlighted library from this library list and, consequently, also from the Browser List.
This Delete Icon will not delete a library from the library folder in the Operating System.
To completely remove a Library from a computer, first, delete it from this Symbols Library list, then, using the Operating System, delete that same library from the Folder in which it is contained.
Migrate Libraries: This button is for automatically translating early format Kicad Symbol Libraries to current format Kicad libraries.
Path Substitutions: will be explained in a later Wiki.
Creating and managing Personal Footprint Libraries is identical to the method for creating and managing Personal Symbol Libraries except:
The Footprint Editor is used (in the PCB Editor).
“Manage Footprint Libraries” in Preferences is used.
New Footprint libraries should be placed in the previously created Footprint Folder.