Symbols and Symbol Libraries

KiCad organizes symbols into symbol libraries, which hold collections of symbols. Each symbol in a schematic is uniquely identified by a full name that is composed of a library nickname and a symbol name. For example, the identifier Audio:AD1853 refers to the AD1853 symbol in the Audio library.

Managing symbol libraries

KiCad uses a table of symbol libraries to map a symbol library nickname to an underlying symbol library on disk. Kicad uses a global symbol library table as well as a table specific to each project. To edit either symbol library table, use PreferencesManage Symbol Libraries…​.

sym lib table dlg

The global symbol library table contains the list of libraries that are always available regardless of the currently loaded project. The table is saved in the file sym-lib-table in the KiCad configuration folder. The location of this folder depends on the operating system being used.

The project specific symbol library table contains the list of libraries that are available specifically for the currently loaded project. If there are any project-specific symbol libraries, the table is saved in the file sym-lib-table in the project folder.

KiCad’s symbol library management system allows directly using many types of symbol libraries, including formats that are native to other non-KiCad EDA tools:

  • KiCad symbol libraries (.kicad_sym files)

  • KiCad Legacy symbol libraries (.lib files)

  • Altium Designer libraries (.SchLib or .IntLib files)

  • CADSTAR Schematic Archive libraries (.lib files)

  • KiCad database library configuration files (.kicad_dbl files)

  • Eagle libraries (.xml files)

  • EasyEDA (JLCEDA) Standard Edition libraries (.json files)

  • EasyEDA (JLCEDA) Professional Edition libraries (.elibz, .epro, or .zip files)

  • KiCad HTTP library configuration files (.kicad_httplib files)

Non-KiCad symbol libraries, including KiCad Legacy symbol libraries, can be migrated to KiCad .kicad_sym format using the Migrate Libraries button (see the migrating libraries section).

KiCad only supports writing to KiCad’s native .kicad_sym format symbol libraries. All other symbol library formats are read-only. To modify a non-KiCad format symbol library, you must first convert it to KiCad format.

Initial Configuration

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.

Managing Table Entries

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 Folder icon button and selecting a library or clicking the Plus icon 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 Delete icon button.

The Up icon and Down icon 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.

Path Variable Substitution

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 PreferencesConfigure 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.

Usage Patterns

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.

Migrating symbol libraries to KiCad format

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.

As with most KiCad files, newer versions of KiCad can open older-format library files, but older versions of KiCad cannot read files once they have been saved by a newer version of KiCad.

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.

Legacy Project Remapping

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:

  • the original libraries used in the schematic are still available and unchanged from when the symbol was added to the schematic.

  • all rescue operations were performed when detected to create a rescue library or keep the existing rescue library up to date.

  • the integrity of the project symbol cache library has not been corrupted.

The remapping will make a back up of all the files that are changed during remapping in the rescue-backup folder in the project folder. Always make a back up of your project before remapping just in case something goes wrong.

The rescue operation is performed even if it has been disabled to ensure the correct symbols are available for remapping. Do not cancel this operation or the remapping will fail to correctly remap schematics symbols. Any broken symbol links will have to be fixed manually.

If the original libraries have been removed and the rescue was not performed, the cache library can be used as a recovery library as a last resort. Copy the cache library to a new file name and add the new library file to the top of the library list using a version of KiCad prior to the symbol library table implementation.

Creating and editing symbols

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

  • Graphical items (lines, circles, arcs, text, etc.) that determine how symbol looks in a schematic.

  • Pins, which have both graphic properties (line, clock, inverted, low level active, etc.) and electrical properties (input, output, bidirectional, etc.) used by the Electrical Rules Check (ERC) tool.

  • Fields, such as references, values, corresponding footprint names for PCB design, etc.

A symbol library is composed of one or more symbols. Generally the symbols are logically grouped by function, type, and/or manufacturer. Each symbol library is a single file with the .kicad_sym extension.

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.

Symbol Editor overview

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 (ToolsSymbol Editor).

In general, the flow for designing a symbol involves:

  • Defining if the symbol is made up of one or more units.

  • Defining if the symbol has an alternate body style (also known as a De Morgan representation).

  • Designing its symbolic representation using lines, rectangles, circles, polygons and text.

  • Adding pins by carefully defining each pin’s graphical elements, name, number, and electrical property (input, output, tri-state, power output, etc.).

  • Determining if the symbol should be derived from another symbol with the same graphical design and pin definition.

  • Adding optional fields such as the name of the footprint used by the PCB design software and/or defining their visibility.

  • Documenting the symbol by adding a description string and links to data sheets, etc.

  • Saving it in the desired library.

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.

Symbol Editor main window
Top toolbar

The main toolbar is at the top of the main window. It has buttons for the undo/redo commands, zoom commands, symbol properties dialogs, and unit/representation management controls.

New symbol icon

Create a new symbol in the selected library.

Save icon

Save the currently selected library. All modified symbols in the library will be saved.

Undo icon

Undo last edit.

Redo icon

Redo last undo.

Refresh icon

Refresh display.

Zoom in icon

Zoom in.

Zoom out icon

Zoom out.

Zoom to fit page icon

Zoom to fit symbol in display.

Zoom to selection icon

Zoom to fit selection.

Rotate counterclockwise icon

Rotate counter-clockwise.

Rotate clockwise icon

Rotate clockwise.

Mirror horizontally icon

Mirror horizontally.

Mirror vertically icon

Mirror vertically.

Symbol properties icon

Edit the current symbol properties.

Pin table icon

Edit the symbol’s pins in a tabular interface.

Datasheet icon

Open the symbol’s datasheet, if it is defined.

ERC icon

Test the current symbol for design errors.

Normal body style icon

Select the normal body style. The button is disabled if the current symbol does not have an alternate body style.

Alternate body style icon

Select the alternate body style. The button is disabled if the current symbol does not have an alternate body style.

Unit dropdown

Select the unit of a multi-unit symbol to display. The drop down control will be disabled if the current symbol is not derived from a symbol with multiple units.

Synchronized pin edit mode icon

Enable synchronized pins edit mode. When this mode is enabled, any pin modifications are propagated to all other symbol units. Pin number changes are not propagated. This mode is automatically enabled for symbols with multiple interchangeable units and cannot be enabled for symbols with only one unit.

Add symbol to schematic icon

Insert current symbol into the schematic.

Left toolbar display controls

The left toolbar provides options to change the display of items in the Symbol Editor.

Grid icon

Toggle grid visibility on and off.

Grid override icon

Toggle grid overrides on and off.

Inch unit icon

Set units to inches.

Millimeter unit icon

Set units to mils (0.001 inch).

Millimeter unit icon

Set units to millimeters.

Cursor shape icon

Toggle full screen cursor on and off.

Show pintype icon

Toggle display of pin electrical types.

Symbol tree icon

Toggle display of library and symbol tree.

Symbol tree icon

Toggle display of properties manager pane.

Right toolbar tools

Placement and drawing tools are located in the right toolbar.

Cursor icon

Select tool. Right-clicking with the select tool opens the context menu for the object under the cursor. Left-clicking with the select tool displays the attributes of the object under the cursor in the message panel at the bottom of the main window. Double-left-clicking with the select tool will open the properties dialog for the object under the cursor.

Pin icon

Pin tool. Left-click to add a new pin.

Text icon

Graphical text tool. Left-click to add a new graphical text item.

Textbox icon

Graphical textbox tool. Left-click to add a new graphical textbox item.

Add rectangle icon

Rectangle tool. Left-click to begin drawing the first corner of a graphical rectangle. Left-click again to place the opposite corner of the rectangle.

Add circle icon

Circle tool. Left-click to begin drawing a new graphical circle from the center. Left-click again to define the radius of the circle.

Add arc icon

Arc tool. Left-click to begin drawing a new graphical arc item from the first arc end point. Left-click again to define the second arc end point. Adjust the radius by dragging the arc center point.

Add line icon

Connected line tool. Left-click to begin drawing a new graphical line item in the current symbol. Left-click for each additional connected line. Double-left-click to complete the line.

Add line icon

Connected line tool. Left-click to begin drawing a new graphical line item in the current symbol. Left-click for each additional connected line. Double-left-click to complete the line.

Anchor icon

Anchor tool. Left-click to set the anchor position of the symbol.

Delete icon

Delete tool. Left-click to delete an object from the current symbol.

Browsing, modifying, and saving symbols

The Symbol tree icon 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.

Some symbols are derived from other symbols. Derived symbol names are displayed in italics in the treeview. If a derived symbol is opened, its symbol graphics will not be editable. Its symbol fields will be editable as normal. To edit the graphics of a base symbol and all of its derived symbols, open the base 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 Save icon icon.

Saving a modified symbol also saves all other modified symbols in the same library.

To save the symbol changes to a new symbol, click FileSave 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 FileExportSymbol…​. This file will be a standard symbol library file which will contain only one symbol.

Creating a new symbol library

You can create a new symbol library by clicking FileNew 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.

symbol editor new library

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.

Creating a new symbol

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

  • A symbol name

  • An optional base symbol to derive the new symbol from. The new symbol will use the base symbol’s graphical shape and pin configuration, but other symbol information can be modified in the derived symbol. The base symbol must be in the same library as the new derived symbol.

  • The reference designator prefix (U, C, R…​).

  • The number of units per package, and whether those units are interchangeable (for example a 7400 quad NAND symbol could have 4 units, one for each gate).

  • If an alternate body style (sometimes referred to as a "De Morgan equivalent") is desired.

  • Whether the symbol is a power symbol. Power symbols appear in the Add Power Symbol dialog in the Schematic editor, make global net connections based on their value, cannot be assigned a footprint, and are excluded from the PCB and bill of materials.

  • Whether the symbol should be excluded from the bill of materials.

  • Whether the symbol should be excluded from the PCB.

There are also several graphical options.

  • The offset between the end of each pin and its pin name.

  • Whether the pin number and pin name should be displayed.

  • Whether the pin names should be displayed alongside the pins or at the ends of the pins inside the symbol body.

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

New symbol properties

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

Newly created symbol

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 Anchor icon button and clicking on the new desired anchor position.

Editing Symbol Properties

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 Symbol properties icon button to show the Symbol Properties dialog. You can also double click an empty spot in the editing canvas.

Symbol Properties

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.

Place pin name inside unchecked
Symbol Name and Keywords

Symbol name is the symbol’s name in the library. Symbols are identified by a combination of the library and symbol name.

In previous versions of KiCad, the symbol name was linked to the Value field. This link is removed in KiCad 7.0 and later.

The keywords should contain additional terms related to the component. Keywords are primarily used, in combination with the symbol name and the Description field, for searching for the symbol in the Symbol Chooser and the Symbol Editor. Those three items are also displayed when you select a symbol in the Symbol Chooser.

Symbol Fields

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.

Symbol fields are different than graphic text. In addition to being named, fields can be moved and edited in the schematic, while symbol text can only be edited in the symbol editor.

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.

A convenient way to create additional empty symbol fields is to use define field name templates. Field name templates define empty fields that are added to each symbol when it is inserted into the schematic. Field name templates can be defined globally (for all schematics) in the Schematic Editor Preferences, or they can be defined locally (specific to each project) in the Schematic Setup dialog.
If you want to manage a large amount of component data in symbol fields, consider using database libraries.

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 Component properties icon 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.

Footprint Filters

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.

Footprint filters

Symbol Units and Alternate Body Styles

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 EditSet Unit Display Name…​.

Use the unit selection dropdown 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 Normal representation icon icon. To edit the alternate representation, click on the Alternate representation icon icon.

Synchronized Pins Edit Mode can be enabled by clicking the Synchronized pins edit mode icon icon. In this mode, pin modifications are propagated between symbol units; changes made in one unit will be reflected in the other units as well. When this mode is disabled, pin changes made in one unit do not affect other units. This mode is enabled automatically when All units are interchangeable is checked, but it can be disabled. The mode cannot be enabled when All units are interchangeable is unchecked or when the symbol only has one unit.
Example of a Symbol With Multiple Noninterchangeable Units

For an example of a symbol with multiple units that are not interchangeable, consider a relay with 3 units per package: a coil, switch 1, and switch 2.

The three units are not all the same, so All units are interchangeable should be deselected in the Symbol Properties dialog. Alternatively, this option could have been specified when the symbol was initially created.

Uncheck all units are interchangeable
Unit A
Relay unit A
Unit B
Relay unit B
Unit C
Relay unit C

Unit A does not have the same symbol and pin layout as Units B and C, so the units are not interchangeable.

Symbol Graphics

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:

  • Lines (line icon) and polygons (polygon icon) defined by start and end points.

  • Rectangles (rectangle icon) defined by two diagonal corners.

  • Circles (circle icon) defined by the center and radius.

  • Arcs (arc icon) defined by the starting and ending point of the arc and its center.

  • Graphical text (Text icon) and textboxes (textbox icon), which is automatically oriented to be readable, even when the symbol is mirrored. Note that graphic text items are not the same as symbol fields.

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.

Graphic line properties

The properties of a graphic element are:

  • Border determines whether the the shape’s outline should be drawn.

  • Width and color define the line width and color of the border. A border width of 0 uses the schematic’s default symbol line width. Style determines the line style of the border (solid, dashed, dotted, etc.).

  • Fill Style determines if the shape defined by the graphical element is to be drawn unfilled or filled. The fill color can be the color theme’s body outline color, body background color, or a custom color.

  • Common to all units in symbol determines if the graphical element is drawn for each unit in symbol with more than one unit per package or if the graphical element is only drawn for the current unit.

  • Common to all body styles (De Morgan) determines if the graphical element is drawn for each symbolic representation in symbols with an alternate body style or if the graphical element is only drawn for the current body style.

  • Private to Symbol Editor causes the shape to be visible only when the symbol is edited in the Symbol Editor. The shape will be hidden when the symbol is added to a schematic.

Symbol Pins

You can create and insert a pin by clicking on the Pin icon 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:

  • Symbol pins are matched to footprint pads by number. The pin number in the symbol must match the corresponding pad number in the footprint.

  • Do not use spaces in pin names and numbers. Spaces will be automatically replaced with underscores (_).

  • To define a pin name with an inverted signal (overbar) use the ~ (tilde) character followed by the text to invert in braces. For example ~{FO}O would display FO O.

  • If the pin name is empty, the pin is considered unnamed.

  • Pin names can be repeated in a symbol.

  • Pin numbers must be unique in a symbol.

Pin Properties
Pin properties

The pin properties dialog allows you to edit all of the characteristics of a pin. This dialog pops up automatically when you create a pin or when double-clicking on an existing pin. This dialog allows you to modify:

  • The pin name and text size.

  • The pin number and text size.

  • The pin length.

  • The pin electrical type and graphical style.

  • Unit and alternate representation membership.

  • Pin visibility.

  • Alternate pin definitions.

Pin Graphic Styles

The different pin graphic styles are shown in the figure below. These styles are purely graphical and do not affect the pin’s electrical type.

Pin graphic styles
Pin Electrical Types

Each pin in a symbol has an electrical type, such as input, output, or tri-state.

Choosing the correct electrical type is important for the schematic ERC tool. ERC will check that pins are connected appropriately, for example ensuring that input pins are driven and power inputs receive power from an appropriate source.

You can use the Pin Conflicts Map in the schematic editor to configure which pin types are allowed to connect and which will conflict. The default Pin Conflicts settings are briefly explained below. For more information, see the ERC documentation.

Additionally, some pin types have special behavior outside of ERC. In the router, pads corresponding to a free pin can be connected to copper of any other net without causing a DRC error, and multiple pads corresponding to a single unconnected pin do not need to be connected to each other in the board.

Pin Type



A pin which is exclusively an input. The default Pin Conflicts settings allow input pins to connect to most other types of pin.


A pin which is exclusively an output. The default Pin Conflicts settings allow output pins to connect to most types of pin that aren’t also outputs.


A pin that can be either an input or an output, such as a microcontroller data bus pin. The default Pin Conflicts settings allow bidirectional pins to connect to most other types of pins, though there are a few more restrictions than with input pins.


A three state output pin (high, low, or high impedance). The default Pin Conflicts settings allow tri-state pins to connect to most other types of pins, but warnings are generated when they are connected to most types of output or power pins.


A pin that is not connected to active electronics, for example pins on a resistor or connector. The default Pin Conflicts settings allow passive pins to connect to most other types of pin.


A pin that does not electrically affect the operation of the device. These pins typically represent package leads that are not internally connected to the chip. The default Pin Conflicts settings allow free pins to connect to most other types of pin.

In the PCB editor, pads corresponding to free pins can be connected to copper of any other net without causing a DRC error.


A pin which has an unspecified type. With the default Pin Conflicts settings, ERC generates warnings when unspecified pins are connected to most other types of pins.

Power input

A pin that powers the device. The default Pin Conflicts settings allow power input pins to connect to most other pin types. However, power input pins that are not connected to a power output pin generate an ERC violation.

Additionally, power input pins that are marked invisible are automatically connected to the net with the same name as the pin. This behavior is supported primarily for legacy projects and is not recommended for new designs. See the Hidden Power Pin section for more information.

Power output

A pin that provides power to other pins, such as a regulator output. The default Pin Conflicts settings allow power output pins to connect to most types of output pins, but not input pins.

Open collector

An open collector logic output. The default Pin Conflicts settings allow open collector pins to connect to most input pins and other open collector pins, but not to most other types of outputs.

Open emitter

An open emitter logic output. The default Pin Conflicts settings allow open collector pins to connect to most input pins and other open emitter pins, but not to most other types of outputs.


A pin that should not be connected to anything. ERC does not allow pins of type unconnected to connect to any other type of pin, and ERC will not generate an "unconnected pin" violation when pins of this type are left unconnected. Unconnected pins are not configurable in the ERC Pin Conflicts map.

If a footprint has multiple pads corresponding to a single unconnected pin, the pads do not need to be connected to each other in the board.

When multiple pins of type unconnected are stacked in a symbol, they are connected to separate nets, whereas stacked pins of other types are connected to the same net.

Note that this pin type is different than placing a no connect flag on a pin in the schematic. The unconnected pin type indicates that the pin should never be connected in any schematic, while a no connect flag indicates that the pin is intentionally unconnected in the current schematic.

Pushing Pin Properties to Other Pins

You can apply the length, name size, or number size of a pin to the other pins in the symbol by right clicking the pin and selecting Push Pin Length, Push Pin Name Size, or Push Pin Number Size, respectively. All other pins in the symbol will be updated.

Defining Pins for Multiple Units and Alternate Symbolic Representations

Symbols with multiple units and/or graphical representations are particularly problematic when creating and editing pins. Most commonly, pins are specific to each symbol unit (because each unit has a different set of pins) and to each body style (because the form and position is different between the normal body style and the alternate form).

The symbol library editor allows the simultaneous creation of pins. By default, changes made to a pin are made for all units of a multiple unit symbol and to both representations for symbols with an alternate symbolic representation. The only exception to this is the pin’s graphical type and name, which remain unlinked between symbol units and body styles. This dependency was established to allow for easier pin creation and editing in most cases. This dependency can be disabled by toggling the Synchronized pin edit mode icon icon on the main tool bar. This will allow you to create pins for each unit and representation completely independently.

Pins can be common or specific to different units. Pins can also be common to both symbolic representations or specific to each symbolic representation. When a pin is common to all units, it only has to drawn once. Pins are set as common or specific in the pin properties dialog.

An example is the output pin in the 7400 quad dual input NAND gate. Since there are four units and two symbolic representations, there are eight separate output pins defined in the symbol definition. When creating a new 7400 symbol, unit A of the normal symbolic representation will be shown in the library editor. To edit the pin style in the alternate symbolic representation, it must first be enabled by clicking the Alternate representation icon button on the tool bar. To edit the pin number for each unit, select the appropriate unit using the unit selection dropdown drop down control.

Pin Table

Another way to edit pins is to use the Pin Table, which is accessible via the Pin table icon icon. The Pin Table displays all of the pins in the symbol and their properties in a table view, so it is useful for making bulk pin changes.

Any pin property can be edited by clicking on the appropriate cell. Pins can be added and removed with the Plus icon and Trash icon icons, respectively.

You can edit the same property for multiple pins simultaneously by grouping pins. Pins can be automatically grouped by name, or you manually group several pins by selecting them and clicking Group Selected. Click the small refresh 16 button to clear the manual grouping. You can also filter the table to only display pins in certain units.

Columns of the pin table can be shown or hidden by right-clicking on the header row and checking or unchecking additional columns. Some columns are hidden by default.

The screenshot below shows the pin table for a dual opamp.

Pin table
Alternate Pin Function Definitions

Pins can have alternate pin function definitions added to them. Alternate pin functions allow a user to select a different name, electrical type, and graphical style for a pin when the symbol has been placed in the schematic. This can be used for pins that have multiple functions, such as microcontroller pins.

Alternate pin functions are added in the Pin Properties dialog as shown below. Each alternate definition contains a pin name, electrical type, and graphic style. This microcontroller pin has all of its peripheral functions defined in the symbol as alternate pin names.

Alternate pin definitions

Alternate pin functions are selected in the Schematic Editor once the symbol has been placed in the schematic. The alternate pin is assigned in the Pin Functions tab of the Symbol Properties dialog. Alternate definitions are selectable in the dropdown in the Alternate Assignment column. You can also select an alternate pin by right-clicking the pin and selecting a new function from the Pin Function menu.

Selecting an alternate pin definition

Creating Power Symbols

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.

In previous versions of KiCad, a power symbol’s pin needed to be both a power input pin and invisible, and the pin’s name determined the name of the net that the power symbol connected with. Beginning in KiCad version 8, the pin in a power symbol does not need to be invisible, and the net is determined by the power symbol’s Value field.

Below is an example of a GND power symbol.

Editing a power symbol
Power symbol pin

To create a power symbol, use the following steps:

  • Add a pin of type Power input. Make the pin number 1, the length 0, set the graphic style to Line, and make the pin visible. The pin number, name, length, and line style do not matter electrically.

  • Place the pin on the symbol anchor. This is not required but makes it easier to place the power symbol in the schematic.

  • Use the shape tools to draw the symbol graphics.

  • Set the symbol value to the desired net name. The symbol value is electrically important: it determines the symbol’s connected net name. This field can be changed later, after the symbol has been placed in the schematic, which will change which net the symbol connects to.

  • Check the Define as power symbol box in Symbol Properties window. This makes the symbol appear in the Add Power Symbol dialog, prevents the symbol from being assigned a footprint, and excludes the symbol from the board, BOM, and netlists.

  • Also deselect the Show pin number and Show pin name options in the Symbol Properties window. This is not necessary but improves the symbol’s appearance.

  • Set the symbol reference and uncheck the Show box. The reference text is not important except for the first character, which should be #. For the power symbol shown above, the reference could be #GND. Symbols with references that begin with # are not added to the PCB, are not included in Bill of Materials exports or netlists, and they cannot be assigned a footprint in the footprint assignment tool. If a power symbol’s reference does not begin with #, the character will be inserted automatically when the annotation or footprint assignment tools are run.

Checking Symbols

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

symbol checker detecting an off-grid pin

The symbol checker checks for:

  • Pins that are off-grid (pins are considered off grid if their position is not a multiple of the current symbol editor grid. It is strongly recommended to use a 50 mil grid for symbol pins)

  • Pins that are duplicated

  • Issues with graphical shapes, such as zero-sized shapes

  • Illegal reference designator prefixes: reference designator prefixes should not end with a number or ?

  • Incorrectly designed power symbols. Power symbols should have:

    • A single unit

    • No alternate body styles

    • A single pin which is either of type Power Output (see PWR_FLAG) or visible and of type Power Input (see power symbols)

  • Hidden Power Input pins in non-power symbols: these create implicit connections and are not recommended

In previous versions of KiCad, power symbols required an invisible power input pin so that they would make a global connection. In KiCad 8, the power input pin does not need to be invisible. Therefore the symbol checker will report if invisible power input pins are detected.

Browsing symbol libraries

The Symbol Library Browser allows you to quickly examine the contents of symbol libraries. The Symbol Library Viewer can be accessed by clicking Library viewer icon icon on the main Symbol Editor toolbar or with ViewSymbol Library Browser.

To examine the contents of a library, select a library from the list in the left hand pane. All symbols in the selected library will appear in the second pane. Select a symbol name to view the symbol.

Symbol Library Browser

Double clicking the name of a symbol or using the Add symbol to schematic icon button adds the symbol to the schematic.

The top toolbar contains the following commands:

Previous symbol icon

Select previous symbol in library.

Next symbol icon

Select next symbol in library.

refresh 24 zoom in 24 zoom out 24 zoom fit in page 24

Zoom tools.

morgan1 24 morgan2 24

Select standard or alternate De Morgan representation of symbol, if applicable.

symbol editor unit selector

Select the unit of a multi-unit symbol.


Open the symbol’s datasheet, if it is defined.

Add symbol to schematic icon

Insert current symbol into the schematic.