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, Personal Libraries are required to store, save and use:
created, modified Kicad, or imported 3rd party symbols and footprints.
Personal libraries are also a convenient way of storing frequently used Kicad library symbols.
The KiCAD library structure is “flat”. Kicad will only create Libraries. Kicad will not create a filing system into which created Personal Libraries can be placed.
It’s highly recommended to create Personal Folders into which Kicad created Personal Libraries are placed.
Creation of Personal Folders
First, personal folders must be created to contain personal libraries. Two are required to start: one for Symbols and one for Footprints and should be named as such.
These folders are created with your Operating System, not Kicad.
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.
Note:
- 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.
Note:
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”.
Note:
- 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.
Note:
The new library has no gray triangle beside its name and does not open. This is because it is empty.
Library management.
- 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.
Note:
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 and available in both the Schematic Editor library browser and the Symbol Editor library browser. Un-ticking a library will remove a library from view in both the Browsers. This may be of benefit to abbreviate the list of viewed libraries.
Visible column: The Visible column excludes any un-ticked libraries from the Schematic Editor library browser only. This does not alter the access and use of any active libraries in the Symbol Editor.
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, however, for temporary use, changing nicknames can save huge amounts of time scrolling.
eg. copying frequently used symbols from the Kicad “Device” Library to Personal Libraries.
Pin Library: This function allows any number of libraries, Personal or Kicad, to be pinned to the top of the library list in all the Editors. This function is accessed by Right Mouse Button click, on the required library, from the left hand displayed list, in either the Symbol or Footprint Editors.
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.
Footprint Libraries:
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.