The first time the KiCad Schematic Editor is run and the global symbol table file sym-lib-table is not found in the KiCad configuration folder, KiCad will guide the user through setting up a new symbol library table. This process is described above.

Symbol libraries can only be used if they have been added to either the global or project-specific symbol library table.

Add a library either by clicking the button and selecting a library or clicking the button and typing the path to a library file. The selected library will be added to the currently opened library table (Global or Project Specific). Libraries can be removed by selecting desired library entries and clicking the button.

The and buttons move the selected library up and down in the library table. This does not affect the display order of libraries in the Symbol Library Browser, Symbol Editor, or Add Symbol tool.

Libraries can be made inactive by unchecking the Active checkbox in the first column. Inactive libraries are still in the library table but do not appear in any library browsers and are not loaded from disk, which can reduce loading times.

A range of libraries can be selected by clicking the first library in the range and then Shift-clicking the last library in the range.

Each library must have a unique nickname: duplicate library nicknames are not allowed in the same table. However, nicknames can be duplicated between the global and project library tables. Libraries in the project table take precedence over libraries with the same name in the global table.

Library nicknames do not have to be related to the library filename or path. The colon character (:) cannot be used in library nicknames or symbol names because it is used as a separator between nicknames and symbols.

Each library entry must have a valid path. Paths can be defined as absolute, relative, or by environment variable substitution.

The appropriate library format must be selected in order for the library to be properly read. "KiCad" format is used for KiCad version 6+ libraries (.kicad_sym files), while "Legacy" format is used for libraries from older versions of KiCad (.lib files). Legacy libraries are read-only, but can be migrated to KiCad format libraries using the Migrate Libraries button (see section Migrating Legacy Libraries).

There is an optional description field to add a description of the library entry. The option field is not used at this time so adding options will have no effect when loading libraries.

The symbol library tables support environment variable substitution, which allows you to define environment variables containing custom paths to where your libraries are stored. Environment variable substitution is supported by using the syntax ${ENV_VAR_NAME} in the symbol library path.

By default, KiCad defines several environment variables which are described in the project manager documentation. Environment variables can be configured in the Preferences → Configure Paths…​ dialog.

Using environment variables in the symbol library tables allows libraries to be relocated without breaking the symbol library tables, so long as the environment variables are updated when the library location changes.

${KIPRJMOD} is a special environment variable that always expands to the absolute path of the current project directory. ${KIPRJMOD} allows libraries to be stored in the project folder without having to use an absolute path in the project library table. This makes it possible to relocate projects without breaking their project library tables.

Symbol libraries can be defined either globally or specifically to the currently loaded project. Symbol libraries defined in the user’s global table are always available and are stored in the sym-lib-table file in the user’s KiCad configuration folder. The project-specific symbol library table is active only for the currently open project file.

There are advantages and disadvantages to each method. Defining all libraries in the global table means they will always be available when needed. The disadvantage of this is that load time will increase.

Defining all symbol libraries on a project specific basis means that you only have the libraries required for the project which decreases symbol library load times. The disadvantage is that you always have to remember to add each symbol library that you need for every project.

One usage pattern would be to define commonly used libraries globally and the libraries only required for the project in the project specific library table. There is no restriction on how to define libraries.

Legacy libraries (.lib files) are read-only, but they can be migrated to KiCad version 6 libraries (.kicad_sym). KiCad version 6 libraries cannot be viewed or edited by KiCad versions older than 6.0.0.

Legacy libraries can be converted to KiCad 6 libraries by selecting them in the symbol library table and clicking the Migrate Libraries button. Multiple libraries can be selected and migrated at once by Ctrl-clicking or shift-clicking.

Libraries can also be converted one at a time by opening them in the Symbol Editor and saving them as a new library.

When loading a schematic created prior to the symbol library table implementation, KiCad will attempt to remap the symbol library links in the schematic to the appropriate library table symbols. The success of this process is dependent on several factors:

A symbol is a schematic representation of a component. A symbol is composed of:

A symbol library is composed of one or more symbols. Generally the symbols are logically grouped by function, type, and/or manufacturer.

Symbols can be derived from another symbol in the same library. Derived symbols share the base symbol’s graphical shape and pin definitions, but can override the base symbol’s property fields (value, footprint, footprint filters, datasheet, description, etc.). Derived symbols can be used to define symbols that are similar to a base part. For example, 74LS00, 74HC00, and 7437 symbols could all be derived from a 7400 symbol. In previous versions of KiCad, derived symbols were referred to as aliases.

KiCad provides a symbol editing tool that allows you to create libraries, add, delete or transfer symbols between libraries, export symbols to files, and import symbols from files.

In general, the flow for designing a symbol involves:

The Symbol Editor main window is shown below. It consists of three toolbars for quick access to common features and a symbol viewing/editing area. Not all commands are available on the toolbars, but all commands are available in the menus.

The button displays or hides the list of available libraries, which allows you to select an active library. When a symbol is saved, it will be placed in this library.

Clicking the icon on the left toolbar toggles the treeview of libraries and symbols. Clicking on a symbol opens that symbol.

After modification, a symbol can be saved in the current library or a different library.

To save the modified symbol in the current library, click the icon. The modifications will be written to the existing symbol.

To save the symbol changes to a new symbol, click File → Save As…​. The symbol can be saved in the current library or a different library. A new name can be set for the symbol.

To create a new file containing only the current symbol, click File → Export → Symbol…​. This file will be a standard library file which will contain only one symbol.

Graphical elements create the visual representation of a symbol and contain no electrical connection information. Graphical elements are created with the following tools:

The vertical toolbar on the right hand side of the main window allows you to place all of the graphical elements required to design the representation of a symbol.

Symbols can have up to two body styles (a standard symbol and an alternate symbol often referred to as a "De Morgan equivalent") and/or have more than one unit per package (logic gates for example). Some symbols can have more than one unit per package each with different symbols and pin configurations.

For example, consider a relay with two switches, which can be designed as a symbol with three different units: a coil, switch 1, and switch 2. Designing a symbol with multiple units per package and/or alternate body styles is very flexible. A pin or a body symbol item can be common to all units or specific to a given unit or they can be common to both symbolic representation so are specific to a given symbol representation.

By default, pins are specific to a unit and body style. When a pin is common to all units or all body styles, it only needs to be created once. This is also the case for the body style graphic shapes and text, which may be common to each unit, but typically are specific to each body style.

To add additional units to a symbol, set the Number of Units property to the appropriate number in the Symbol Properties dialog. By default, symbol units are named Unit A, Unit B, etc., but you can set an arbitrary name for the current unit using Edit → Set Unit Display Name…​.

To add an alternate body style, set the Has alternate body style (De Morgan) property in the Symbol Properties dialog.

You can create and insert a pin by clicking on the button. Pin properties can be edited by double clicking on the pin. You can also delete or move pins that you have already added. Pins must be created carefully, because any error will have consequences on the PCB design.

All library symbols are defined with four default fields. The reference designator, value, footprint assignment, and datasheet link fields are created whenever a symbol is created or copied. Only the reference designator is required.

The Footprint field, if used, contains a reference to a footprint for the symbol. The format is LIBNAME:FOOTPRINTNAME, where LIBNAME is the name of the footprint library in the footprint library table (see the Footprint Library Table section in the PCB Editor manual) and FOOTPRINTNAME is the name of the footprint in the library LIBNAME.

Symbols defined in libraries are typically defined with only these four default fields. Additional fields such as vendor, part number, unit cost, etc. can be added to library symbols but generally this is done in the schematic editor so the additional fields can be applied to all of the symbols in the schematic.

Power symbols are symbols that are used to label a wire as part of a global power net, like VCC or GND. The behavior of power symbols is described in the electrical connections section. Power symbols are handled and created the same way as normal symbols, but there are several additional considerations described below.

It may be useful to place power symbols in a dedicated library. KiCad’s symbol library places power symbols in the power library, and users may create libraries to store their own power symbols. If the Define as power symbol box is checked in a symbol’s properties, that symbol will appear in the Schematic Editor’s Add Power Symbol dialog for convenient access.

Below is an example of a GND power symbol.

Power symbols consist of a pin of type "Power input" that is marked invisible. They must also have the Define as power symbol property checked. Invisible power input pins have a special property of making implicit global connections based on the pin name.

Um ein Spannungsversorgungssymbol zu erstellen führen Sie folgende Schritte aus:

An easier method to create a new power symbol is to use another symbol as a starting point, as described earlier.

The Symbol Editor can check for common issues in your symbols. Run the symbol checker using the button in the top toolbar.

The symbol checker checks for: