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 Editor or Symbol Chooser.

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 path variable substitution.

The appropriate library format must be selected in order for the library to be properly read. The supported formats are listed above. Only KiCad format libraries (.kicad_sym) can be saved. Other symbol library formats are read-only and must be converted to KiCad format before you can modify them.

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 path variable substitution, which allows you to define path variables containing custom paths to where your libraries are stored. Path variable substitution is supported by using the syntax ${PATH_VAR_NAME} in the symbol library path.

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

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

${KIPRJMOD} is a special path 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.

Non-KiCad format libraries, including legacy libraries (.lib files), are read-only. They need to be converted to KiCad format (.kicad_sym files) before you can save changes to them.

Libraries in other formats can be converted to KiCad 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:

KiCad provides a symbol editing tool that allows you to create libraries; add, edit, delete, or transfer symbols between libraries; export symbols to files; and import symbols from files. The Symbol Editor can be launched from the KiCad Project Manager or from the Schematic Editor (Tools → Symbol Editor).

In general, the flow for designing a symbol involves:

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

In addition to the toolbars, there are collapsible panels for the symbol tree and Properties Manager on the left. The bottom of the window contains a message panel that shows details about the selected object.

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

Clicking on a symbol name opens that symbol in the editor, and hovering the cursor over the name of a symbol displays a preview of the 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.

To save the symbol changes to a new symbol, click File → Save Copy As…​. The symbol can be saved in the current library or a different library, and 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 symbol library file which will contain only one symbol.

You can create a new symbol library by clicking File → New Library…​. At this point you must choose whether the new library should be added to the global symbol library table or the project symbol library table. Libraries in the global library table will be available to all projects, while libraries in the project library table will only be available in the current project.

Following selection of the library table, you must choose a name and location for the new library. A new, empty library will be created at the specified location.

To create a new symbol in the current symbol library, click the button. You will be asked for a number of symbol properties.

There are also several graphical options.

These properties can also be changed later in the Symbol Properties window.

A new symbol will be created using the properties above and will appear in the editor as shown below.

The blue cross in the center is the symbol anchor, which specifies the symbol origin i.e. the coordinates (0, 0). The anchor can be repositioned by selecting the button and clicking on the new desired anchor position.

Symbol properties are set when the symbol is created but they can be modified at any point. To change the symbol properties, click on the button to show the Symbol Properties dialog. You can also double click an empty spot in the editing canvas.

It is important to set the number of units and check all units are interchangeable and has alternate body style, as applicable, because these settings affect how pins and graphics are added to each symbol unit.

If you change the number of units per package after adding the pins to the symbol, you will need to do extra work to add pins and graphics for the additional units. The pins and graphics would have been automatically added to each unit had these properties been correctly set initially. Nevertheless, it is possible to modify these properties at any time.

The graphic options Show pin number and Show pin name define the visibility of the pin number and pin name text. The option Place pin names inside defines the pin name position relative to the pin body. The pin names will be displayed inside the symbol outline if the option is checked. In this case the Pin Name Position Offset property defines the shift of the text away from the body end of the pin. A value from 0.02 to 0.05 inches is usually reasonable.

The example below shows a symbol with the Place pin name inside option unchecked. Notice the position of the names and pin numbers.

Symbols contain multiple fields, which are named values containing information related to the symbol. Fields can be displayed on the schematic or hidden and only shown in the symbol’s properties. Some fields have special meaning to KiCad: Reference and Footprint are both critical for creating a PCB, for example. Other fields may contain information that is important for a design but is not interpreted by KiCad, like pricing or stock information for a part.

Any fields defined in a library symbol will be included in the symbol when it is added to a schematic. You can also add new fields to symbols in the schematic. Whether they are in the library symbol or not, these fields can then be edited on a per-symbol basis in the schematic. They are also transferred to the symbol’s corresponding footprint in the PCB.

All library symbols are defined with five default fields: Reference, Value, Footprint, Datasheet, and Description, which are added whenever a symbol is created. These default fields cannot be deleted. Only the Reference field is required to have a value: the contents of a library symbol’s Reference field is used as the reference designator prefix when the symbol is added to a schematic. In the schematic, the symbol’s Reference field contains the entire reference designator.

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.

The Description field can contain text describing the symbol such as the component function, distinguishing features, and package options. Together with the symbol’s name and keywords, text in this field is used when searching for symbols in the Symbol Chooser or Symbol Editor. Before KiCad version 8.0, this was a dedicated property (like the symbol name and keywords) rather than a symbol field.

Symbols defined in libraries are typically defined with only these five 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 added to every symbol in the schematic, not just all symbols of one type.

To edit an existing symbol field, double-click the field, select it or hover and press E, or right-click on the field text and select Properties…​.

To add new fields, delete optional fields, or edit existing fields, use the icon on the main tool bar to open the Symbol Properties dialog. Fields can be arbitrarily named, but names starting with ki_, e.g. ki_description, are reserved by KiCad and should not be used for user fields.

Fields have a number of properties, each of which is shown as a column in the properties grid. Not all columns are shown by default; columns can be shown or hidden by right clicking on the grid header and selecting or deselecting columns from the menu.

The footprint filters tab is used to define which footprints are appropriate to use with the symbol. The filters can be applied in the Footprint Assignment tool so that only appropriate footprints are displayed for each symbol.

Multiple footprint filters can be defined. Footprints that match any of the filters will be displayed; if no filters are defined, then all footprints will be displayed.

Filters can use wildcards: * matches any number of characters, including zero, and ? matches zero or one characters. For example, SOIC-* would match the SOIC-8_3.9x4.9mm_P1.27mm footprint as well as any other footprint beginning with SOIC-. The filter SOT?23 matches SOT23 as well as SOT-23.

Symbols can have more than one unit per package, each with different graphics and pin configurations. This is often used for logic gates, opamps, or other components that have multiple subunits within one physical package. Symbols can also have up to two body styles, a standard symbol and an alternate symbol often referred to as a "De Morgan equivalent".

For example, consider a relay with two switches, which can be designed as a symbol with one body style and 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, no mattery how many units or body styles are used. 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…​.

Use the unit selection dropdown to select the unit you wish to edit.

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

If the symbol has an alternate body style defined, one body style must be selected for editing at a time. To edit the normal representation, click the icon. To edit the alternate representation, click on the icon.

Graphical elements create the visual representation of a symbol and contain no electrical connection information. You can draw new graphic shapes using the buttons on the right toolbar. The following types of objects are available:

Each graphic item (line, arc, circle, etc.) can be defined as common to all units and/or body styles or specific to a given unit and/or body style.

Element options can be quickly accessed by right-clicking on the element to display the context menu for the selected element. You can also double-left-click on an element to modify its properties, or edit its properties using the Properties Manager pane.

Below is the properties dialog for a polygon element.

The properties of a graphic element are:

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.

A pin is defined by its graphical representation, its name, and its number. The pin’s name and number can contain letters, numbers, and symbols, but not spaces. For the Electrical Rules Check (ERC) tool to be useful, the pin’s electrical type (input, output, tri-state…​) must also be defined correctly. If this type is not defined properly, the schematic ERC check results may be invalid.

Important notes:

Power symbols are symbols that are used to label a wire as part of a global power net, like VCC or GND. The power symbol’s Value field determines the net label. 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.

Power symbols consist of a single pin of type Power Input. They must also have the Define as power symbol property checked.

Below is an example of a GND power symbol.

To create a power symbol, use the following steps:

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

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: