Podręcznik użytkownika

This manual is in the process of being revised to cover the latest stable release version of KiCad. It contains some sections that have not yet been completed. We ask for your patience while our volunteer technical writers work on this task, and we welcome new contributors who would like to help make KiCad’s documentation better than ever.

This document is Copyright © 2010-2022 by its contributors as listed below. You may distribute it and/or modify it under the terms of either the GNU General Public License (http://www.gnu.org/licenses/gpl.html), version 3 or later, or the Creative Commons Attribution License (http://creativecommons.org/licenses/by/3.0/), version 3.0 or later.

Wszystkie znaki towarowe użyte w tym dokumencie należą do ich właścicieli.


Jean-Pierre Charras, Fabrizio Tappero, Wayne Stambaugh, Graham Keeth


Kerusey Karyu <[email protected]>, 2014-2015.


The KiCad project welcomes feedback, bug reports, and suggestions related to the software or its documentation. For more information on how to sumbit feedback or report an issue, please see the instructions at https://www.kicad.org/help/report-an-issue/

Introduction to the KiCad Schematic Editor


The KiCad Schematic Editor is a schematic capture software distributed as a part of KiCad and available under the following operating systems:

  • Linux

  • Apple macOS

  • Windows

Regardless of the OS, all KiCad files are 100% compatible from one OS to another.

The Schematic Editor is an integrated application where all functions of drawing, control, layout, library management and access to the PCB design software are carried out within the editor itself.

The KiCad Schematic Editor is intended to cooperate with the KiCad PCB Editor, which is KiCad’s printed circuit design software. It can also export netlist files, which lists all the electrical connections, for other packages.

The Schematic Editor includes a symbol library editor, which can create and edit symbols and manage libraries. It also integrates the following additional but essential functions needed for modern schematic capture software:

  • Sprawdzanie poprawności projektu (DRC) dla zautomatyzowanego procesu kontroli poprawności połączeń, czy testowania niepołączonych wejść elementów.

  • Generowanie wydruków w różnych formatach (Postscript, PDF, HPGL oraz SVG).

  • Tworzenie list materiałowych (za pomocą skryptów Python lub XSLT, które pozwalają na różnorodną jej konfigurację).

The Schematic Editor supports multi-sheet schematics in several ways:

  • Flat hierarchies (schematic sheets are not explicitly connected in a master diagram).

  • Simple hierarchies (each schematic sheet is used only once).

  • Complex hierarchies (some schematic sheets are used multiple times).

Hierarchical schematics are described in detail later in the manual.

Konfiguracja początkowa

When the Schematic Editor is run for the first time, if the the global symbol library table file sym-lib-table is not found in the KiCad configuration folder then KiCad will ask how to create this file:

symbol library table initial configuration

The first option is recommended (Copy default global symbol library table (recommended)). The default symbol library table includes all of the standard symbol libraries that are installed as part of KiCad.

If this option is disabled, KiCad was unable to find the default global symbol library table. This probably means you did not install the standard symbol libraries with KiCad, or they are not installed where KiCad expects to find them. On some systems the KiCad libraries are installed as a separate package.

  • If you have installed the standard KiCad symbol libraries and want to use them, but the first option is disabled, select the second option and browse to the sym-lib-table file in the directory where the KiCad libraries were installed.

  • If you already have a custom symbol library table that you would like to use, select the second option and browse to your sym-lib-table file.

  • If you want to construct a new symbol library table from scratch, select the third option.

Symbol library management is described in more detail later.

The Schematic Editor User Interface

Schematic Editor overview

The main Schematic Editor user interface is shown above. The center contains the main editing canvas, which is surrounded by:

  • Top toolbars (file management, zoom tools, editing tools)

  • Left toolbar (display options)

  • Message panel and status bar at bottom

  • Right panel (drawing and design tools)

The editing canvas displays the schematic being designed. You can pan and zoom to different parts of the schematic and open any schematic sheet in the design.

By default, dragging with the middle or right mouse button will pan the canvas view and scrolling the mouse wheel will zoom the view in or out. You can change this behavior in the Mouse and Touchpad section of the preferences (see Configuration and Customization for details).

Several other zoom tools are available in the top toolbar:

  • Zoom In icon zooms in on the center of the viewport.

  • Zoom Out icon zooms out from the center of the viewport.

  • Zoom to Page icon zooms to fit the frame around the drawing sheet.

  • Zoom to Objects icon zooms to fit the items within the drawing sheet.

  • Zoom to Selection icon allows you to draw a box to determine the zoomed area.

The cursor’s current position is displayed at the bottom of the window (X and Y), along with the current zoom factor (Z), the cursor’s relative position (dx, dy, and dist), the grid setting, and the display units.

The relative coordinates can be reset to zero by pressing Space. This is useful for measuring distance between two points or aligning objects.

Klawisze skrótów

The Ctrl+F1 shortcut displays the current hotkey list. The default hotkey list is included in the Actions Reference section of the manual.

The hotkeys described in this manual use the key labels that appear on a standard PC keyboard. On an Apple keyboard layout, use the Cmd key in place of Ctrl, and the Option key in place of Alt.

Many actions do not have hotkeys assigned by default, but hotkeys can be assigned or redefined using the hotkey editor (PreferencesPreferences…​Hotkeys).

Many of the actions available through hotkeys are also available in context menus. To access the context menu, right-click in the editing canvas. Different actions will be available depending on what is selected or what tool is active.

Hotkeys are stored in the file user.hotkeys in KiCad’s configuration directory. The location is platform-specific:

  • Windows: %APPDATA%\kicad\6.0\user.hotkeys

  • Linux: ~/.config/kicad/6.0/user.hotkeys

  • macOS: ~/Library/Preferences/kicad/6.0/user.hotkeys

KiCad can import hotkey settings from a user.hotkeys file using the Import Hotkeys button in the hotkey editor.

Mouse operations and selection

Selecting items in the editing canvas is done with the left mouse button. Single-clicking on an object will select it and dragging will perform a box selection. A box selection from left to right will only select items that are fully inside the box. A box selection from right to left will select any items that touch the box. A left-to-right selection box is drawn in yellow, with a cursor that indicates exclusive selection, and a right-to-left selection box is drawn in blue with a cursor that indicates inclusive selection.

The selection action can be modified by holding modifier keys while clicking or dragging. The following modifier keys apply when clicking to select single items:

Modifier Keys (Windows) Modifier Keys (Linux) Modifier Keys (macOS) Selection Effect




Add the item to the existing selection.




Remove the item from the existing selection.

long click

long click or Alt

long click or Option

Clarify selection from a pop-up menu.




Highlight the net of the selected copper item.

The following modifier keys apply when dragging to perform a box selection:

Modifier Keys (Windows) Modifier Keys (Linux) Modifier Keys (macOS) Selection Effect

Shift or Ctrl

Shift or Ctrl

Shift or Ctrl

Add item(s) to the existing selection.




Remove item(s) from the existing selection.

Selecting an object displays information about the object in the message panel at the bottom of the window. Double-clicking an object opens a window to edit the object’s properties.

Pressing Esc will always cancel the current tool or operation and return to the selection tool. Pressing Esc while the selection tool is active will clear the current selection.

Left toolbar display controls

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

grid visibility icon

Turns grid display on/off.

Note: by default, hiding the grid will disable grid snapping. This behavior can be changed in the Display Options section of Preferences.

inch unit icon

mil unit icon

millimeter unit icon

Display/entry of coordinates and dimensions in inches, mils, or millimeters.

cursor shape icon

Switches between full-screen and small editing cursor (crosshairs).

hidden pin icon

Turns invisible pin display on/off.

free angle wire icon

Switches between free angle and horizontal/vertical placement of new wires, buses, and graphical lines.

Tworzenie i edycja schematu


A schematic designed with KiCad is more than a simple graphic representation of an electronic device. It is normally the entry point of a development chain that allows for:

Schemat składa się głównie z elementów, połączeń między nimi, etykiet, węzłów, magistral i portów zasilania. Dla zwiększenia czytelności schematu, można umieścić elementy graficzne takie jak: wejścia do magistral, komentarze i linie przerywane do budowy ramek.

Symbols are added to the schematic from symbol libraries. After the schematic is made, the set of connections and footprints is imported into the PCB editor for designing a board.

Schematics can be contained in a single sheet or split among multiple sheets. In KiCad, multi-sheet schematics are organized hierarchically, with a root sheet and sub-sheet(s). Each sheet is its own .kicad_sch file and is itself a complete KiCad schematic. Working with hierarchical schematics is described in the Hierarchical Schematics chapter.

Schematic editing operations

Schematic editing tools are located in the right toolbar. When a tool is activated, it stays active until a different tool is selected or the tool is canceled with the Esc key. The selection tool is always activated when any other tool is canceled.

Selection tool icon

Selection tool (the default tool)

Highlight net icon

Highlight a net by marking its wires and net labels with a different color. If the PCB Editor is also open then copper corresponding to the selected net will be highlighted as well. Net highlighting can be cleared by clicking with the highlight tool in an empty space, or by using the Clear Net Highlighting hotkey (~).

New Symbol icon

Display the symbol selector dialog to place a new symbol.

Add Power icon

Display the power symbol selector dialog to place a new power symbol.

Draw Wire icon

Draw a wire.

Draw Bus icon

Draw a bus.

Draw wire to bus icon

Draw wire-to-bus entry points. These elements are only graphical and do not create a connection, thus they should not be used to connect wires together.

draw no connect flag icon

Place a "No Connect" flag. These flags should be placed on symbol pins which are meant to be left unconnected. "No connect" flags indicate to the Electrical Rule Checker that the pin is intentionally unconnected and not an error.

place junction icon

Place a junction. This connects two crossing wires or a wire and a pin, which can sometimes be ambiguous without a junction (i.e. if a wire end or a pin is not directly connected to another wire end).

Local label icon

Place a local label. Local labels connect items located in the same sheet. For connections between two different sheets, use global or hierarchical labels.

Global label icon

Place a global label. All global labels with the same name are connected, even when located on different sheets.

Hierarchical label icon

Place a hierarchical label. Hierarchical labels are used to create a connection between a subsheet and the sheet’s parent sheet. See the Hierarchical Schematics section for more information about hierarchical labels, sheets, and pins.

Hierarchical subsheet icon

Place a hierarchical subsheet. You must specify the file name for this subsheet.

Import hierarchical label icon

Import a hierarchical pin from a subsheet. This command can be executed only on hierarchical subsheets. It will create hierarchical pins corresponding to hierarchical labels placed in the target subsheet.

draw dashed line icon

Draw lines.

Note: Lines are graphical objects and are not the same as wires placed with the Wire tool. They do not connect anything.

place text icon

Place a text comment.

place bitmap icon

Place a bitmap image.

interactive delete tool icon

Delete clicked items.


In the Schematic Editor the cursor always moves over a grid. The grid can be customized:

  • Size can be changed using the right click menu or using ViewGrid Properties…​.

  • Color can be changed in the Colors page of the Preferences dialog (menu PreferencesGeneral Options).

  • Visibility can be switched using the left-hand toolbar button.

The default grid size is 50 mil (0.050") or 1.27 millimeters.

This is the recommended grid for placing symbols and wires in a schematic, and for placing pins when designing a symbol in the Symbol Editor.

Wires connect with other wires or pins only if their ends coincide exactly. Therefore it is very important to keep symbol pins and wires aligned to the grid. It is recommended to always use a 50 mil grid when placing symbols and drawing wires because the KiCad standard symbol library and all libraries that follow its style also use a 50 mil grid. Using a grid size other than 50 mil will result in schematics without proper connectivity!

Smaller grids can also be used, but this is intended only for text and symbol graphics, and not recommended for placing pins and wires.

Symbols, wires, and other elements that are not aligned to the grid can be snapped back to the grid by selecting them, right clicking, and clicking Align Elements to Grid.


Schematic elements such as symbols, wires, text, and graphic lines are snapped to the grid when moving, dragging, and drawing them. Additionally, the wire tool snaps to pins even when grid snapping is disabled. Both grid and pin snapping can be disabled while moving the mouse by using the modifier keys in the table below.

On Apple keyboards, use the Cmd key instead of Ctrl.
Modifier Key Effect


Disable grid snapping.


Disable snapping wires to pins.

Working with symbols

Placing symbols

To load a symbol into your schematic you can use the icon New Symbol icon. A dialog box allows you to type the name of the symbol to load.

Okno dialogowe wyboru symboli

The Choose Symbols dialog will filter symbols by name, keywords, and description according to what you type into the search field.

Some advanced filters are available:

  • Wildcards: use the characters ? and * respectively to mean "any single character or no characters" and "any number of any characters, including none".

  • Key-value pairs: if a library part’s description or keywords contain a tag of the format "Key:123", you can match relative to that by typing "Key>123" (greater than), "Key<123" (less than), etc. Numbers may include one of the following case-insensitive suffixes:

























  • Regular expressions: if you’re familiar with regular expressions, these can be used too. The regular expression flavor used is the wxWidgets Advanced Regular Expression style, which is similar to Perl regular expressions.

If the symbol specifies a default footprint, this footprint will be previewed in the lower right. If the symbol includes footprint filters, alternate footprints that satisfy the footprint filters can be selected in the footprint dropdown menu at right.

After selecting a symbol to place, the symbol will be attached to the cursor. Left clicking the desired location in the schematic places the symbol into the schematic. Before placing the symbol in the schematic, you can rotate it, mirror it, and edit its fields, by either using the hotkeys or the right-click context menu. These actions can also be performed after placement.

Poniższy obrazek pokazuje symbol podczas operacji wstawiania go do schematu:

Komponent w trakcie wstawiania

If the Place repeated copies option is checked, after placing a symbol KiCad will start placing another copy of the symbol. This process continues until the user presses Esc.

For symbols with multiple units, if the Place all units option is checked, after placing the symbol KiCad will start placing the next unit in the symbol. This continues until the last unit has been placed or the user presses Esc.

Placing power ports

A power port symbol is a symbol representing a connection to a power net. The symbols are grouped in the power library, so they can be placed using the symbol chooser. However, as power placements are frequent, the Add Power icon tool is available. This tool is similar, except that the search is done directly in the power library and any other library that contains power symbols.

Moving symbols

Symbols can be moved using the Move (M) or Drag (G) tools. These tools act on the selected symbol, or if no symbol is selected they act on the symbol under the cursor.

The Move tool moves the symbol itself without maintaining wired connections to the symbol pins.

The Drag tool moves the symbol without breaking wired connections to its pins, and therefore moves the connected wires as well.

You can also Drag symbols by clicking and dragging them with the mouse, depending on the Left button drag gesture setting in the Mouse and Touchpad section of Preferences.

Symbols can also be rotated (R) or mirrored in the X (X) or Y (Y) directions.

Editing symbol properties

A symbol’s fields can be edited in the symbol’s Properties window. Open the Symbol Properties window for a symbol with the E hotkey or by double-clicking on the symbol.

Okno edycja głównych właściwości symboli

The Symbol Properties window displays all the fields of a symbol in a table. New fields can be added, and existing fields can be deleted, edited, reordered, moved, or resized.

Każde pole może być widoczne lub nie oraz wyświetlane poziomo lub pionowo. Wyświetlana pozycja jest zawsze pokazywana dla normalnie wyświetlanego elementu (bez obrotu lub lustra) i odnosi się do punktu aktywnego elementu.

The position and orientation properties of each field may be hidden in this dialog. They can be shown by right-clicking on the column header of the fields table and enabling the "Orientation", "X Position", and/or "Y Position" columns. Other columns can be shown or hidden as desired.

The "Update Symbol from Library…​" button is used to update the schematic’s copy of the symbol to match the copy in the library. The "Change Symbol…​" button is used to swap the current symbol to a different symbol in the library.

"Edit Symbol…​" opens the Symbol Editor to edit the copy of the symbol in the schematic. Note that the original symbol in the library will not be modified. The "Edit Library Symbol…​" button opens the Symbol Editor to edit the original symbol in the library. In this case, the symbol in the schematic will not be modified until the user clicks the "Update Symbol from Library…​" button.

Editing symbol fields individually

An individual symbol text field can be edited directly with the E hotkey (with a field selected instead of a symbol) or by double-clicking on the field.

Some symbol fields have their own hotkey to edit them directly. With the symbol selected, the Reference, Value, and Footprint fields can be edited with the U, V, or F hotkeys, respectively.

Edit Value Field dialog

The options in this dialog are the same as those in the full Symbol Properties dialog, but are specific to a single field.

Symbol fields can be automatically moved to an appropriate location with the Autoplace Fields action (select a symbol and press O). Field autoplacement is configurable in the Schematic Editor’s Editing Options, including a setting to always autoplace fields.

Symbol Fields Table

The Symbol Fields Table allows you to view and modify field values for all symbols in a spreadsheet interface. You can open the Symbol Fields Table with the Symbol Fields Table icon button.

Symbol Fields Table

Cells are navigated with the arrow keys, or with Tab / Shift+Tab to move right / left and Enter / Shift+Enter to move down / up, respectively.

A range of cells can be selected by clicking and dragging. The whole range of selected cells will be copied (Ctrl+C) or pasted into (Ctrl+V) on a copy or paste action. Copying a range of cells from the table can be useful for creating a BOM. More details of copying and pasting cells are described below.

Any symbol field can be shown or hidden using the Show checkboxes on the left, or by right-clicking on the header of the table. New symbol fields can be added using the Add Field…​ button.

Similar symbols can optionally be grouped by any symbol field using the Group By checkboxes. Grouped symbols are shown in a single row in the table. The grouped row can be expanded to show the individual symbols by clicking the arrow at the left of the row.

Tricks to simplify filling fields

There are several special copy/paste methods in the spreadsheet for pasting values into larger regions, including auto-incrementing pasted cells. These features may be useful when pasting values that are shared in several symbols.

These methods are illustrated below.

1. Copy (Ctrl+C) 2. Select target cells 3. Paste (Ctrl+V)
















Te techniki są również dostępne w innych oknach dialogowych zawierających tabele.

Reference Designators and Symbol Annotation

Reference designators are unique identifiers for components in a design. They are often printed on a PCB and in assembly diagrams, and allow you to match symbols in a schematic to the corresponding components on a board.

In KiCad, reference designators consist of a letter indicating the type of component (R for resistor, C for capacitor, U for IC, etc.) followed by a number. If the symbol has multiple units then the reference designator will also have a trailing letter indicating the unit. Symbols that don’t have a reference designator set have a ? character instead of the number. Reference designators must be unique.

Reference designators can set manually by editing a symbol’s reference designator field, or automatically using the Annotation tool.

The process of setting a symbol’s reference designator is called annotation.

Numeracja komponentów

The Annotation tool automatically assigns reference designators to symbols in the schematic. To launch the Annotation tool, click the Annotate icon button in the top toolbar.

annotate dialog

The tool provides several options to control how symbols are annotated.

Scope: Selects whether annotation is applied to the entire schematic, to only the current sheet, or to only the selected symbols.

Options: Selects whether annotation should apply to all symbols and reset *existing reference designators, or apply only to unannotated symbols.

Order: Chooses the direction of numbering. If symbols are sorted by X position, all symbols on the left side of a schematic sheet will be lower numbered than symbols on the right side of the sheet. If symbols are sorted by Y position, all symbols on the top of a sheet will be lower numbered than symbols at the bottom of the sheet.

Numbering: Selects the starting point for numbering reference designators. The lowest unused number above the starting point is picked for each reference designator. The starting point can be an arbitrary number (typically zero), or it can be the sheet number multiplied by 100 or 1000 so that each part’s reference designator corresponds to the schematic page it is on.

The Clear Annotation button clears all reference designators in the selected scope.

Annotation messages can be filtered with the checkboxes at the bottom or saved to a report using the Save…​ button.

Electrical Connections

There are two primary ways to establish connections: wires and labels. Both are shown in the schematic below.

Zwykłe etykiety

Connections can also be made with buses and with implicit connections via hidden power pins.

This section will also discuss two special types of symbols that can be added with the "Power port" button on the right toolbar:

  • Power ports: symbols for connecting wires to a power or ground net.

  • PWR_FLAG: a specific symbol for indicating that a net is powered when it is not connected to a power output pin (for example, a power net that is supplied by an off-board connector).

Label Connections

Labels are used to assign net names to wires and pins. Wires with the same net name are considered to be connected. A net can only have one name. If two different labels are placed on the same net, an ERC violation will be generated. Only one of the net names will be used in the netlist. The final net name is determined according to the rules described below.

There are three types of labels, each with a different connection scope.

  • Local labels, also referred to simply as labels, only make connections within a sheet. Add a local label with the Local Label icon button in the right toolbar.

  • Global labels make connections anywhere in a schematic, regardless of sheet. Add a global label with the Global Label icon button in the right toolbar.

  • Hierarchical labels connect to hierarchical sheet pins and are used in hierarchical schematics for connecting child sheets to their parent sheet. Add a hierarchical label with the Hierarchical Label icon button in the right toolbar.

Labels that have the same name will connect, regardless of the label type, if they are in the same sheet.

After using the appropriate button or hotkey to create a label, the Label Properties dialog appears.

Global Label Properties dialog

The Label field sets the label’s text, which determines the net that the label assigns to its attached wire. Label text supports markup for overbars, subscripts, etc., as well as variable substitution. Use the Syntax help link in the dialog for a summary.

Justification sets the position of the label’s connection point relative to the label’s text. For example, when Align right is selected the connection point will be to the right of the text.

Text size and Style control the appearance of the label’s text. Shape controls the shape of the outline around the label; this is purely visual and has no electrical consequence. Local labels do not have an outline, and therefore do not have Shape options.

Global labels have additional settings to control margins around the label text in the Schematic Setup dialog.

After accepting the label properties, the label is attached to the cursor for placement. The connection point for a label is the small square in the corner of the label. The square disappears when the label is connected to a wire or the end of a pin.

Unconnected label

The connection point’s position relative to the label text can be changed by choosing a different label orientation in the label’s properties, or by mirroring/rotating the label.

The Label Properties dialog can be accessed at any time by selecting a label and using the E hotkey, double-clicking on the label, or with Properties…​ in the right-click context menu.

Wire Connections

To establish a connection, a segment of wire must be connected by its end to another segment or to a pin. Only wire ends create connections; if a wire crosses the middle of another wire, a connection will not be made.

Unconnected wire ends have a small square that indicates the connection point. The square disappears when a connection is made to the wire end. Unconnected pins have a circle, which also disappears when a connection is made.

Wires connect with other wires or pins only if their ends coincide exactly. Therefore it is important to keep symbol pins and wires aligned to the grid. It is recommended to always use a 50 mil grid when placing symbols and drawing wires because the KiCad standard symbol library and all libraries that follow its style also use a 50 mil grid.
Symbols, wires, and other elements that are not aligned to the grid can be snapped back to the grid by selecting them, right clicking, and selecting Align Elements to Grid.
Drawing and editing wires

To begin connecting elements with wire, use the Wire tool line tool icon in the right toolbar (w). Wires can also be automatically started by clicking on an unconnected symbol pin or wire end.

Wires can be moved using the Move (M) or Drag (G) tools. As with symbols, the Move tool moves only the selected segment, without maintaining existing connections to other segments. The Drag tool maintains existing connections.

If a segment is selected or the cursor is over the middle of a wire, the move/drag action will move the entire segment. If the cursor is over a corner or wire end, the move/drag action will act on one end of the segment.

Wire Junctions

Wires that cross are not implicitly connected. It is necessary to join them by explicitly adding a junction dot if a connection is desired (Add Junction icon button in the right toolbar). Junction dots will be automatically added to wires that start or end on top of an existing wire.

Junction dots are used in the schematic figure above on the wires connected to P1 pins 18, 19, 20, 21, 22, and 23.

Bus Connections

Buses are a way to group related signals in the schematic in order to simplify complicated designs. Buses can be drawn like wires using the bus tool bus tool icon, and are named using labels the same way signal wires are.

In the following schematic, many pins are connected to buses, which are the thick blue lines in the center.

Przykład schematu z wykorzystaniem magistral
Składniki magistral

There are two types of bus in KiCad 6.0 and later: vector buses and group buses.

Magistrala wektorowa to kolekcja sygnałów, których nazwa składa się z takiego samego przedrostka i kończy przyrostkiem z unikalną liczbą. Magistrale wektorowe są nazywane wg schematu <PREFIX>[M..N] gdzie PREFIX to dowolna nazwa sygnału, M to pierwsza liczba przyrostka, a N to ostatnia liczba. Na przykład, magistrala DATA[0..7] zawiera grupę sygnałów DATA0, DATA1, itd. aż do DATA7. Nie ma znaczenia jak wartości M oraz N zostały zdefiniowane, byle by nie były one wartościami ujemnymi.

Magistrala grupowa to kolekcja różnych sygnałów bądź magistral wektorowych. Magistrale grupowe można użyć do zgrupowania razem sygnałów posiadających różne nazwy. Magistrale grupowe używają specjalnego zapisu etykiet:


Sygnały w grupie są wymienione wewnątrz nawiasów klamrowych ({}) oddzielonych spacjami. Opcjonalna nazwa grupy występuje przed otwierającym nawiasem klamrowym. Jeśli magistrala grupowa nie ma nazwy, wynikowe sieci w obwodzie drukowanym będą po prostu nazwami sygnałów wewnątrz grupy. Jeśli magistrala grupowa ma nazwę, wynikowe sieci będą miały nazwę jako prefiks z kropką (.) oddzielającą prefiks od nazwy sygnału.

Na przykład magistrala {SCL SDA} posiada dwa sygnały, stąd na liście sieci będą to sygnały SCL i ` SDA`. Magistrala USB1{DP DM} wygeneruje zaś sieci o nazwie USB1.DP i ` USB1.DM`. W przypadku projektów z większymi magistralami, które występują powtórnie w kilku podobnych obwodach, zastosowanie tej techniki może zaoszczędzić czas.

Magistrale grupowe mogą również zawierać magistrale wektorowe. Na przykład magistrala MEMORY{A[7..0] D[7..0] OE WE} zawiera zarówno magistrale wektorowe, jak i zwykłe sygnały co spowoduje utworzenie sieci takich jak: MEMORY.A7 i ` MEMORY.OE` na PCB.

Bus wires can be drawn and connected in the same manner as signal wires, including using junctions to create connections between crossing wires. Like signals, buses cannot have more than one name — if two conflicting labels are attached to the same bus, an ERC violation will be generated.

Połączenia pomiędzy składnikami magistral

Pins connected between the same members of a bus must be connected by labels. It is not possible to connect a pin directly to a bus; this type of connection will be ignored by KiCad.

W powyższym przykładzie, połączenia wykonane są za pomocą etykiet umieszczonych na połączeniach podłączonych do wyprowadzeń. Połączenia poprzez wejścia do magistral (odcinki połączeń pod kątem 45 stopni) mają wyłącznie wartość estetyczną, i nie są konieczne na poziomie czystego schematu.

In fact, using the repetition command (Insert), connections can be very quickly made in the following way, if component pins are aligned in increasing order (a common case in practice on components such as memories, microprocessors…​):

  • Place the first label (for example PCA0)

  • Use the repetition command as much as needed to place members. KiCad will automatically create the next labels (PCA1, PCA2…​) vertically aligned, theoretically on the position of the other pins.

  • Narysować połączenie pod pierwszą z etykiet. Następnie użyć polecenia powtarzania umieszczając dalsze połączenia pod etykietami.

  • W razie potrzeby umieścić wejścia do magistrali w ten sam sposób (Umieścić pierwsze wejście, a następnie użyć polecenia powtarzania).

In the Schematic EditorEditing Options section of the Preferences menu, you can set the repetition parameters:

  • Horizontal pitch

  • Vertical pitch

  • Label increment (labels can be incremented or decremented by 1, 2, 3, etc.)

Wyprowadzanie sygnałów z magistral

The unfold tool allows you to quickly break out signals from a bus. To unfold a signal, right-click on a bus object (a bus wire, etc) and choose Unfold from Bus. Alternatively, use the Unfold Bus hotkey (default: C) when the cursor is over a bus object. The menu allows you to select which bus member to unfold.

Po wybraniu sygnału z magistrali, następne kliknięcie umieści etykietę sygnału magistrali w żądanym miejscu. Narzędzie automatycznie wygeneruje wejście do magistrali i połączenie prowadzące do miejsca gdzie znajdować się będzie etykieta. Po umieszczeniu etykiety możesz kontynuować umieszczanie dodatkowych segmentów połączenia (Na przykład, aby połączyć się z pinem komponentu) i dokończyć połączenie w dowolny sposób.

Aliasy magistral

Aliasy magistrali to skróty, które umożliwiają wydajniejszą pracę z magistralami o dużych grupach. Pozwalają one zdefiniować magistralę grupową i nadać jej krótką nazwę, która może być następnie używana zamiast pełnej nazwy grupy na schemacie.

To create bus aliases, open the Bus Definitions dialog in the Tools menu.

Okno z definicjami magistral

Alias może mieć dowolną dozwoloną nazwę sygnału. Korzystając z okna dialogowego, można dodawać sygnały lub magistrale wektorowe do aliasu. Jako skrót można wpisać lub wkleić listę sygnałów i/lub magistral oddzieloną spacjami, a wszystkie one zostaną dodane do definicji aliasu. W tym przykładzie zdefiniujemy alias o nazwie USB z elementami DP, DM i ` VBUS`.

Po zdefiniowaniu aliasu można go użyć jako etykiety magistrali grupowej, umieszczając nazwę aliasu w nawiasach klamrowych na magistrali grupowej: {USB}. Ma to taki sam efekt, jak etykietowanie magistrali {DP DM VBUS}. Można także dodać nazwę prefiksu do grupy, na przykład USB1 {USB}, co skutkuje nazwami sieci takimi jak USB1.DP, tak jak opisano to wcześniej. W przypadku skomplikowanych magistral używanie aliasów może znacznie skrócić etykiety na schemacie. Pamiętaj, że aliasy są tylko skrótem, a nazwa aliasu nie jest dołączana do listy sieci.

Aliasy magistral są zapisywane w pliku schematu. Wszelkie aliasy utworzone na danym arkuszu schematu są dostępne do użytku w dowolnym innym arkuszu schematu, który znajduje się w tej samej strukturze hierarchicznej.

Magistrale posiadające więcej niż jedną etykietę

Program KiCad w wersji 5.0 i wcześniejszych pozwalał na łączenie sygnałów magistral z różnymi etykietami i łączył je podczas tworzenia listy sieci. To zachowanie zostało usunięte w programie KiCad 6.0, ponieważ jest niekompatybilne z magistralami grupowymi, a także prowadzi do mylących list sieci, ponieważ nazwa którą dany sygnał odbierze, nie była do przewidzenia.

Jeśli otwarto projekt, który wykorzystywał tę funkcję w nowszej wersji programu, pojawi się okno dialogowe Migracja magistral, które przeprowadzi użytkownika przez aktualizację schematu, tak aby na danym zestawie sygnałów magistrali istniała tylko jedna etykieta.

Okno migracji do nowego systemu magistral

Dla każdego zestawu sygnałów magistrali, który ma więcej niż jedną etykietę, należy wybrać etykietę, która zostanie zachowana. Lista rozwijana z nazwami pozwala wybrać jedną z etykiet, istniejącą w projekcie lub wybrać inną nazwę, wprowadzając ją ręcznie w polu nowej nazwy.

Hidden Power Pins

When the power pins of a symbol are visible, they must be connected, as with any other signal. However, symbols such as gates and flip-flops are sometimes drawn with hidden power input pins which are connected implicitly.

KiCad automatically connects invisible pins with type "power input" to a global net with the same name as the pin. For example, if a symbol has a hidden power input pin named VCC, this pin will be globally connected to the VCC net on all sheets.

Hidden pins can be shown in the schematic by checking the Show hidden pins option in the Schematic EditorDisplay Options section of the preferences, or by selecting ViewShow hidden pins. There is also a toggle icon hidden pin 24 on the left toolbar.

It may be necessary to join power nets of different names (for example, GND in TTL components and VSS in MOS components). To accomplish this, add a power port symbol for each net and connect them with a wire.

If hidden power pins are used, it is not recommended to use local labels for power connection, as they will not connect to hidden power pins on other sheets.

Care must be taken with hidden power input pins because they can create unintentional connections. By nature, hidden pins are invisible and do not display their pin name. This makes it easy to accidentally connect two power pins to the same net. For this reason, using invisible power pins in symbols is not recommended outside of power port symbols, and is only supported for compatibility with legacy designs and symbols.

Power Ports

Power ports are symbols that are conventionally used to represent a connection to a power net, such as VCC or GND. In addition to being a visual indicator that the attached net is a power rail, power ports make global connections: two power ports with the same pin name connect to each other anywhere in the schematic, regardless of sheet.

In the figure below, power port symbols are used to connect the positive and negative terminals of the capacitors to the VCC and GND nets, respectively.

Przykład portu zasilania

In the KiCad standard library, power ports are found in the power library, but power port symbols can be created in any library. To create a custom power port, make a new symbol with a power input pin that is set to be invisible. Name the pin according to the desired power net. In addition, set the "Define as power symbol" symbol property. As described in the hidden power pins section, invisible power input pins make global connections based on the hidden power pin’s name. The process of creating a power port is described in more detail in the Symbol Editor section.

The connected net name is determined by the power port’s pin name, not the name or value of the symbol. This means that power port net names can only be changed in the symbol editor, not in the schematic.

Net name assignment rules

Every net in the schematic is assigned a name, whether that name is specified by the user or automatically generated by KiCad.

When multiple labels are attached to the same net, the final net name is determined in the following order, from highest priority to lowest:

  1. Etykiety globalne

  2. Power ports

  3. Local labels

  4. Etykiety hierarchiczne

  5. Hierarchical sheet pins

If there are multiple labels of one type attached to a net, the names are sorted alphabetically and the first is used.

If a net travels through multiple sheets in a hierarchy, and has no global label or power port, it will take its name from the highest level of the hierarchy where it has a hierarchical label or local label. As described above, local labels take priority over hierarchical labels.

If none of the labels above are attached to a net, the net’s name is automatically generated based on the connected symbol pins.


Two PWR_FLAG symbols are visible in the screenshot above. They indicate to ERC that the two power nets VCC and GND are actually connected to a power source, as there is no explicit power source such as a voltage regulator output attached to either net.

Without these two flags, the ERC tool would diagnose: Error: Input Power pin not driven by any Output Power pins.

The PWR_FLAG symbol is found in the power symbol library. The same effect can be achieved by connecting any power output pin to the net.

No-connection flag

No-connection flags (No-connection icon) are used to indicate that a pin is intentionally unconnected. These flags do not have any effect on the schematic’s connectivity, but they prevent "unconnected pin" ERC warnings for pins that are intentionally unconnected.

Graphical items

Text and graphic lines

It can be useful to place annotations such as text fields and frames to aid in understanding the schematic. Text fields (text 24) and graphic lines (add dashed line 24) are intended for this use, as opposed to labels and wires, which are connection elements.

The image below shows graphic lines and text in addition to wires, local labels, and hierarchical labels.

Przykład ramki z komentarzem


The title block is edited with the Page Settings tool (Page Settings tool).

Okno dialogowe ustawienia strony

Each field in the title block can be edited, as well as the paper size and orientation. If the "Export to other sheets" option is checked for a field, that field will be updated in the title block of all sheets, rather than only the current sheet.

You can set the date to today’s or any other date by pressing the left arrow button by "Issue Date", but the date in the schematic will not be automatically updated.

A drawing sheet template file can also be selected.

Ramka tytułowa

The sheet number (Sheet X/Y) is automatically updated, but sheet page numbers can also be manually set using EditEdit Sheet Page Number…​.

Schematic Setup

The Schematic Setup window is used to set schematic options that are specific to the currently active schematic. For example, the Schematic Setup window contains formatting options, electrical rule configuration, netclass setup, and schematic text variable setup.

Odzyskiwanie symboli z pamięci cache

By default, KiCad loads symbols from the project libraries according to the set paths and library order. This can cause a problem when loading a very old project: if the symbols in the library have changed or have been removed or the library no longer exists since they were used in the project, the ones in the project would be automatically replaced with the new versions. The new versions might not line up correctly or might be oriented differently leading to a broken schematic.

When a project is saved, a cache library with the contents of the current library symbols is saved along with the schematic. This allows the project to be distributed without the full libraries. If you load a project where symbols are present both in its cache and in the system libraries, KiCad will scan the libraries for conflicts. Any conflicts found will be listed in the following dialog:

Okno odzyskiwania konfliktowych symboli

You can see in this example that the project originally used a diode with the cathode facing up, but the library now contains one with the cathode facing down. This change would break the schematic! Pressing OK here will cause the symbol cache library to be saved into a special rescue library and all the symbols are renamed to avoid naming conflicts.

If you press Cancel, no rescues will be made, so KiCad will load all the new components by default. If you save the schematic at this point, your cache will be overwritten and the old symbols will not be recoverable. If you have saved the schematic, you can still go back and run the rescue function again by selecting "Rescue Cached Components" in the "Tools" menu to call up the rescue dialog again.

Jeśli użytkownik nie chce by to okno dialogowe się pokazywało, może zaznaczyć opcję "Nie pokazuj ponownie". Będzie to oznaczało, że operacje porównania nie będą przeprowadzane i nowe symbole będą ładowane domyślnie. Opcję tą można wyłączyć w oknie ustawień bibliotek.

Schematy o strukturze hierarchicznej


In KiCad, multi-sheet schematics are hierarchical: there is a single root sheet, and additional sheets are created as subsheets of either the root sheet or another subsheet. Sheets can be included in a hierarchy multiple times, if desired.

Carefully drawing a schematic as a hierarchical design improves schematic legibility and reduces repetitive drawing.

Creating a hierarchical schematic starts from the root sheet. The process is to create a subsheet, then draw the circuit in the subsheet and make the necessary electrical connections between sheets. Connections can be made between nets in a subsheet and nets in the parent sheet using hierarchical pins and labels, or between any two nets in the hierarchy using global labels.

Adding sheets to a design

You can add a subsheet to a design with the Add Hierarchical Sheet tool (S hotkey, or the Add Hierarchical Sheet icon button in the right toolbar). Launch the tool, then click twice in the canvas to draw the upper left and lower right corners of the subsheet symbol. Make the sheet outline large enough to fit the hierarchical pins you will add later.

Drawing a hierarchical sheet

The Sheet Properties dialog will appear and prompt you for a sheet name and filename.

Hierarchical sheet properties

The sheet name must be unique, as it is used in the full net name for any nets in the subsheet. For example, a net with the local label net1 in the sheet sheet1 would have a full net name of /sheet1/net1. The sheet name is also used to refer to the sheet in various places in the GUI, including the title block and the hierarchy navigator.

The sheet filename specifies the file that the new sheet will be saved to or loaded from. The path to the sheet file can be relative or absolute. It is usually preferable to save subsheet files in the project directory and use a relative path so that the project is portable.

A single sheet file can be used more than once in a project by specifying the same filename for each repeated sheet; the circuit drawn in the sheet will be instantiated once per usage, and any edits in once instance will be reflected in the other instances.

Sheet files can be shared between multiple projects to allow design reuse between projects. However, this is not recommended due to path portability concerns and the risk of unintentionally changing other projects while editing a shared sheet.

The sheet’s page number is configurable here. The page number is displayed in the sheet title block and the hierarchy navigator, and sheets are sorted by page number in the hierarchy navigator and when printing or plotting.

Several graphical options are also available. Border width sets the width of the border around the sheet shape. Border color and Background fill set the color for the border and fill of the sheet shape, respectively. If no color is set, a checkerboard swatch is shown and the default values from the color theme are used.

The Sheet Properties dialog can be accessed at any time by selecting a sheet symbol and using the E hotkey, or by right-clicking on a sheet symbol and selecting Properties…​.

You can enter a hierarchical sheet from the parent sheet by double-clicking the child sheet’s shape, or right-clicking the child sheet and selecting Enter Sheet.

Return to the parent sheet by using the Leave sheet icon button in the top toolbar, or by right-clicking in an empty part of the schematic and clicking Leave Sheet.

Alternatively, you can jump to any sheet with the hierarchy navigator. To open the hierarchy navigator, click the Hierarchy navigator icon button in the top toolbar. Each sheet in the design is displayed as an item in the tree. Clicking a sheet name opens that sheet in the editing canvas.

hierarchy navigator

By default, the hierarchy navigator closes after a new sheet is opened. It can be configured to always remain open by selecting the Keep hierarchy navigator open option in the Editing Options section of the Schematic Editor preferences.

Electrical connections between sheets

Label overview

Electrical connections between sheets are made with labels. There are several kinds of labels in KiCad, each with a different connection scope.

  • Local labels only make connections within a sheet. Therefore local labels cannot be used to connect between sheets. Local labels are added with the Local Label icon button.

  • Global labels make connections anywhere in a schematic, regardless of sheet. Global labels are added with the Global Label icon button.

  • Hierarchical labels connect to hierarchical sheet pins accessible in the parent sheet. Hierarchical designs rely on hierarchical labels and pins to make connections between parent sheets and child sheets; you can think of hierarchical pins as defining the interface for a sheet. Hierarchical labels are added with the Hierarchical Label icon button.

Labels that have the same name will connect, regardless of the label type, if they are in the same sheet.
Hidden power pins can also be considered global labels, because they connect anywhere in the schematic hierarchy.

Hierarchical sheet pins

After placing hierarchical labels within the subsheet, matching hierarchical pins can be added to the subsheet symbol in the parent sheet. You can then make connections to the hierarchical pins with wires, labels, and buses. Hierarchical pins in a subsheet symbol are connected to the matching hierarchical labels in the subsheet itself.

Hierarchical labels must be defined in the subsheet before the corresponding hierarchical sheet pin can be imported in the sheet symbol.
hierarchical sheet symbol with pins

For every hierarchical label in the subsheet, import the corresponding hierarchical pin into the sheet symbol by clicking the Import Hierarchical Pin icon button in the right toolbar, then clicking on the sheet symbol. A sheet pin for the first unmatched hierarchical label will be attached to the cursor, where it can be placed anywhere along the border of the sheet symbol. Clicking again with the tool will continue to import additional sheet pins until there are no more hierarchical pins to import from the subsheet. Sheet pins can also be imported by selecting Import Sheet Pin in a sheet symbol’s right-click context menu.

You can edit the properties of a sheet pin in the Sheet Pin Properties dialog. Open this dialog by double-clicking a sheet pin, selecting a sheet pin and using the E hotkey, or right-clicking a sheet pin and selecting Properties…​.

Sheet Pin Properties dialog

The sheet pin’s name can be edited in the textbox or by selecting from the dropdown list of hierarchical labels in the subsheet. A sheet pin’s name has to match the corresponding hierarchical label in the subsheet, so if a pin name is changed the label must change as well.

The connection type changes the shape of the sheet pin, and has no electrical effect. It can be set to Input, Output, Bidirectional, Tri-state, or Passive. The pin’s text size can also be changed.

Hierarchical design examples

Hierarchical designs can be put into one of several categories:

  • Simple: each sheet is used only once.

  • Complex: some sheets are instantiated multiple times.

  • Flat: a sub-case of a simple hierarchy, without connections between subsheets and their parent. Flat hierarchies can be used to represent a non-hierarchical design.

Each hierarchy model can be useful; the most appropriate one depends on the design.

Simple hierarchy

An example of a simple hierarchy is the video demo project included with KiCad. The root sheet contains seven unique subsheets, each with hierarchical labels and sheet pins linking the sheets to each other in the root sheet. Two of the subsheet symbols are shown below.

Simple hierarchy from video demo project

Hierarchia złożona

The complex_hierarchy demo project is an example of a complex hierarchy. The root sheet contains two subsheet symbols, which both refer to the same sheet file (ampli_ht.kicad_sch). This allows the design to include two copies of the same amplifier circuit. Although the two sheet symbols refer to the same filename, the sheet names are unique (ampli_ht_vertical and ampli_ht_horizontal). Inside each subsheet the circuits are identical except for the reference designators, which as always are unique.

This project contains no sheet pin connections. The only connections between the root sheet and the subsheets are global power connections made with power port symbols. However, sheets in a complex hierarchy could include sheet pin connections if appropriate for the design.

Complex hierarchy from complex_hierarchy demo project

Hierarchia płaska

The flat_hierarchy demo project is an example of a flat hierarchy. The root sheet contains two unique subsheet symbols with no hierarchical sheet pins. The root sheet in this project does nothing except hold the subsheets, and the subsheets are used only as additional pages in the schematic.

This is the simplest way to create multi-page schematics in KiCad.
Flat hierarchy from flat_hierarchy demo project

Inspecting a schematic

Find tool

The Find tool searches for text in the schematic, including reference designators, pin names, symbol fields, and graphic text. When the tool finds a match, the canvas is zoomed and centered on the match and the text is highlighted. Launch the tool using the Find icon button in the top toolbar.

Główne okno narzędzia wyszukiwania

The Find tool has several options:

Match case: Selects whether the search is case-sensitive.

Words: When selected, the search will only match the search term with complete words in the schematic. When unselected, the search will match if the search term is part of a larger word in the schematic.

Wildcards: When selected, wildcards can be used in the search terms. ? matches any single character, and * matches any number of characters. Note that when this option is selected, partial matches are not returned: searching for abc* will match the string abcd, but searching for abc will not.

Search pin names and numbers: Selects whether the search should apply to pin names and numbers.

Search hidden fields: Selects whether the search should apply only to visible fields or if it should include hidden symbol fields.

Search the current sheet only: Selects whether the search should be limited to the current schematic sheet or to the entire schematic.

There is also a Find and Replace tool which is activated with the Find and Replace icon button in the top toolbar. This tool behaves the same as the Find tool, but additionally can replace some or all matches with different text.

Find and Replace dialog

If the Replace matches in reference designators option is checked, reference designators will be modified if they contain matching text. Otherwise reference designators will not be affected.

Net highlighting

An electrical net can be highlighted in the schematic editor to visualize all of the places it appears in the schematic. Net highlighting can be activated in the Schematic Editor or by highlighting the corresponding net in the PCB editor when cross-probe highlighting is enabled (see below). When net highlighting is active, the highlighted net will be shown in a different color. By default this color is pink, but it is configurable in the Color section of the Preferences dialog.

Nets can be highlighted by clicking on a wire or pin using the Highlight Net tool in the right toolbar (Net Highlight icon). Alternatively, the Highlight Net hotkey (`) highlights the net under the cursor. If there are no nets or pins under the cursor, any existing highlighting will be cleared. The highlighting can also be cleared by using the Clear Net Highlight action (hotkey ~).

Cross-probing from the PCB

KiCad allows bi-directional cross-probing between the schematic and the PCB. There are several different types of cross-probing.

Selection cross-probing allows you to select a symbol or pin in the schematic to select the corresponding footprint or pad in the PCB (if one exists) and vice-versa. By default, cross-probing will result in the display centering on the cross-probed item and zooming to fit. This behavior can be disabled in the Display Options section of the Preferences dialog.

Highlight cross-probing allows you to highlight a net in the schematic and PCB at the same time. If the option "Highlight cross-probed nets" is enabled in the Display Options section of the Preferences dialog, highlighting a net or bus in the schematic editor will cause the corresponding net or nets to be highlighted in the PCB editor, and vice versa.

Kontrola reguł projektowych - Electrical Rules Check

The Electrical Rules Check (ERC) tool performs an automatic check of your schematic. The ERC checks for any errors in your sheet, such as unconnected pins, unconnected hierarchical symbols, shorted outputs, etc. ERC output is reported as errors or warnings depending on the severity of the issue detected.

Naturally, an automatic check is not infallible, and it is not possible to detect all design errors. Such a check is still very useful, because it allows you to detect many oversights and small errors. All detected issues should be checked and addressed before proceeding.

The quality of the ERC is directly related to the care taken in declaring electrical pin properties during symbol library creation.

ERC can be started by clicking on the ERC icon button in the top toolbar and clicking the Run ERC button.

Główne okno narzędzia ERC

Any warnings or errors are reported in the Violations tab, and markers for each violation are placed in the schematic so that they point to the relevant part of the schematic. Warnings are indicated by yellow arrows, and errors have red arrows. Excluded violations are shown as green arrows.

Selecting a violation in the ERC window jumps to the selected violation marker in the schematic.

The numbers at the bottom of the window show the number of errors, warnings, and exclusions. Each type of violation can be filtered from the list using the respective checkboxes. Clicking Delete Markers will clear all violations until ERC is run again.

Violations can be right-clicked in the dialog to ignore them or change their severity:

Ignore ERC warning
  • Exclude this violation: ignores this particular violation, but does not affect any other violations.

  • Change severity: changes a type of violation from warning to error, or error to warning. This affects all violations of a given type.

  • Ignore all: ignores all violations of a given type.

ERC example

Znaczniki ERC

Here you can see three errors:

  • Two outputs have been connected together (red arrow at right).

  • Two inputs have been left unconnected (red arrows at left).

Selecting an ERC marker displays a description of the violation in the message pane at the bottom of the window.

ERC violation description in message pane

Power pins and power flags

It is common to have an "Input Power pin not driven by any Output Power pins" error on power pins, as shown in the example below, even though the power pins seem to be properly connected to a power rail. This happens in designs where the power is provided through connectors or other components that are not marked as power outputs. In these cases ERC won’t detect any Output Power pins connected to the net and will determine the Input Power pin is not driven by a power source.

Power pins and error flags

To avoid this warning, connect the net to PWR_FLAG symbol on such a power net as shown in the following example. The PWR_FLAG symbol is found in the power symbol library. Alternatively, connect any power output pin to the net; PWR_FLAG is simply a symbol with a single power output pin.

Power pins with PWR_FLAGs

Ground nets often need a PWR_FLAG as well, because voltage regulators have outputs declared as power outputs, but their ground pins are typically marked as power inputs. Therefore grounds can appear unconnected to a source unless a PWR_FLAG symbol is used.

For more information about power pins and power flags, see the PWR_FLAG documentation.

ERC Configuration

The Pin Conflicts Map panel in Schematic Setup allows you to configure connectivity rules to define electrical conditions for errors and warnings based on what types of pins are connected to each other.

Schematic ERC Pin Conflicts Map

Poszczególne reguły mogą zostać zmienione poprzez kliknięcie na wybranym polu na powyższej matrycy. Kolejne kliknięcia pozwalają na wybranie: brak błędu (zielony), ostrzeżenie (żółty, W) i błąd (czerwony, E). Zmiany odbywają się w zamkniętym cyklu, zatem aby wrócić do poprzedniego stanu należy ponownie kliknąć (jedno- lub dwukrotnie).

Schematic ERC severity settings

The Violation Severity panel in Schematic Setup lets you configure what types of ERC messages should be reported as Errors, Warnings or ignored.

Plik raportu ERC

An ERC report file can be generated and saved by clicking the Save…​ button in the ERC dialog. The file extension for ERC report files is .rpt. Here is an example ERC report file.

ERC report (Fri 21 Oct 2022 02:07:05 PM EDT, Encoding UTF8)

***** Sheet /
[pin_not_driven]: Input pin not driven by any Output pins
    ; Severity: error
    @(149.86 mm, 60.96 mm): Symbol U1B [74LS00] Pin 4 [, Input, Line]
[pin_not_connected]: Pin not connected
    ; Severity: error
    @(149.86 mm, 60.96 mm): Symbol U1B [74LS00] Pin 4 [, Input, Line]
[pin_not_connected]: Pin not connected
    ; Severity: error
    @(149.86 mm, 66.04 mm): Symbol U1B [74LS00] Pin 5 [, Input, Line]
[pin_to_pin]: Pins of type Output and Output are connected
    ; Severity: error
    @(165.10 mm, 63.50 mm): Symbol U1B [74LS00] Pin 6 [, Output, Inverted]
    @(165.10 mm, 46.99 mm): Symbol U1A [74LS00] Pin 3 [, Output, Inverted]
[pin_not_driven]: Input pin not driven by any Output pins
    ; Severity: error
    @(149.86 mm, 66.04 mm): Symbol U1B [74LS00] Pin 5 [, Input, Line]

 ** ERC messages: 5  Errors 5  Warnings 0

Assigning Footprints

Before routing a PCB, footprints need to be selected for every component that will be assembled on the board. Footprints define the copper connections between physical components and the routed traces on a circuit board.

Some symbols come with footprints pre-assigned, but for many symbols there are multiple possible footprints, so the user needs to select the appropriate one.

KiCad offers several ways to assign footprints:

  • Właściwości symbolu

    • Symbol Properties Dialog

    • Symbol Fields Table

  • While placing symbols

  • Footprint Assignment Tool

Each method will be explained below. Which to use is a matter of preference; one method may be more convenient depending on the situation. All of these methods are equivalent in that they store the name of the selected footprint in the symbol’s Footprint field.

The Footprint Library Table needs to be configured before footprints can be assigned. For information on configuring the Footprint Library Table, please see the PCB Editor manual.

Assigning Footprints in Symbol Properties

A symbol’s Footprint field can be edited directly in the symbol’s Properties window.

Assigning footprint in Symbol Properties

Clicking the library icon button in the Footprint field opens the Footprint Library Browser, which shows the available footprints and footprint libraries. Single clicking a footprint name selects the footprint and displays it in the preview pane on the right, while double clicking on a footprint closes the browser and sets the symbol’s Footprint field to the selected footprint.

Selecting a footprint in Footprint Library Browser

Assigning Footprints with the Symbol Fields Table

Rather than editing the properties of each symbol individually, the Symbol Fields Table can be used to view and edit the properties of all symbols in the design in one place. This includes assigning footprints by editing the Footprint field of each symbol.

The Symbol Fields Table is accessed with ToolsEdit Symbol Fields…​, or with the Symbol Fields Table Icon button on the top toolbar.

The Footprint field behaves the same here as in the Symbol Properties window: it can be edited directly, or footprints can be selected visually with the Footprint Library Browser.

Bulk editing footprint assignments with the Symbol Fields Table

For more information on the Symbol Fields Table, see the section on editing symbol properties.

Assigning Footprints While Placing Symbols

Footprints can be assigned to symbols when the symbol is first added to the schematic.

Some symbols are defined with a default footprint. These symbols will have this footprint preassigned when they are added to the schematic. The default footprint is shown in the Add Symbol dialog. For symbols without a default symbol defined, the footprint dropdown will say "No default footprint", and the footprint preview canvas will say "No footprint specified".

Default footprint in Add Symbol dialog

Symbols can have footprint filters that specify which footprints are appropriate to use with that symbol. If footprint filters are defined for the selected symbol, all footprints that match the footprint filters will appear as options in the footprint dropdown. The selected footprint will be displayed in the preview canvas and will be assigned to the symbol when the symbol is added to the schematic.

Footprint options will not appear in the footprint dropdown unless the footprint libraries are loaded. Footprint libraries are loaded the first time the Footprint Editor or Footprint Library Browser are opened in a session.

For more information on footprint filters, see the Symbol Editor Documentation.

Assigning Footprints with the Footprint Assignment Tool

The Footprint Assignment Tool allows you to associate symbols in your schematic to footprints used when laying out the printed circuit board. It provides footprint list filtering, footprint viewing, and 3D component model viewing to help ensure the correct footprint is associated with each component.

Components can be assigned to their corresponding footprints manually or automatically by creating equivalence files (.equ files). Equivalence files are lookup tables associating each component with its footprint.

Run the tool with ToolsAssign Footprints…​, or by clicking the Footprint Assignment Tool icon icon in the top toolbar.

Footprint Assignment Tool Overview

The image below shows the main window of the Footprint Assignment Tool.

The main window of the Footprint Assignment Tool
  • The left pane contains the list of available footprint libraries associated with the project.

  • The center pane contains the list of symbols in the schematic.

  • The right pane contains the list of available footprints loaded from the project footprint libraries.

  • The bottom pane describes the filters that have been applied to the footprint list and prints information about the footprint selected in the rightmost pane.

The top toolbar contains the following commands:

save 24

Transfer the current footprint associations to the schematic.

library table 24

Edit the global and project footprint library tables.

icon footprint browser 24

View the selected footprint in the footprint viewer.

left 24

Select the previous symbol without a footprint association.

right 24

Select the next symbol without a footprint association.

undo 24

Undo last edit.

redo 24

Redo last edit.

auto associate 24

Perform automatic footprint association using an equivalence file.

delete association 24

Delete all footprint assignments.

module filtered list 24

Filter footprint list by footprint filters defined in the selected symbol.

module pin filtered list 24

Filter footprint list by pin count of the selected symbol.

module library list 24

Filter footprint list by selected library.

The following table lists the keyboard commands for the Footprint Assignment Tool:

Right Arrow / Tab

Activate the pane to the right of the currently activated pane. Wrap around to the first pane if the last pane is currently activated.

Left Arrow

Activate the pane to the left of the currently activated pane. Wrap around to the last pane if the first pane is currently activated.

Up Arrow

Select the previous item of the currently selected list.

Down Arrow

Select the next item of the currently selected list.

Page Up

Select the item one full page upwards of the currently selected item.

Page Down

Select the item one full page downwards of the currently selected item.


Select the first item of the currently selected list.


Select the last item of the currently selected list.

Manually Assigning Footprints with the Footprint Assignment Tool

To manually associate a footprint with a component, first select a component in the component (middle) pane. Then select a footprint in the footprint (right) pane by double-clicking on the name of the desired footprint. The footprint will be assigned to the selected component, and the next component without an assigned footprint is automatically selected.

If no footprints appear in the footprint pane, check that the footprint filter options are correctly applied.

When all components have footprints assigned to them, click the OK button to save the assignments and exit the tool. Alternatively, click Cancel to discard the updated assignments, or Apply, Save Schematic & Continue to save the new assignments without exiting the tool.

Filtrowanie listy footprintów

There are four filtering options which restrict which footprints are displayed in the footprint pane. The filtering options are enabled and disabled with three buttons and a textbox in the top toolbar.

  • module filtered list 24: Activate filters that can be defined in each symbol. For example, an opamp symbol might define filters that show only SOIC and DIP footprints.

  • module pin filtered list 24: Only show footprints that match the selected symbol’s pin count.

  • module library list 24: Only show footprints from the library selected in the left pane.

  • Entering text in the textbox hides footprints that do not match the text. This filter is disabled when the box is empty.

When all filters are disabled, the full footprint list is shown.

The applied filters are described in the bottom pane of the window, along with the number of footprints that meet the selected filters. For example, when the symbol’s footprint filters and pin count filters are enabled, the bottom pane prints the footprint filters and pin count:

Filter details when symbol footprint filters and pin count filter are enabled

Multiple filters can be used at once to help narrow down the list of possibly appropriate footprints in the footprint pane. The symbols in KiCad’s standard library define footprint filters that are designed to be used in combination with the pin count filter.

Automatically Assigning Footprints with the Footprint Assignment Tool

The Footprint Assignment Tool allows you to store footprint assignments in an external file and load the assignments later, even in a different project. This allows you to automatically associate symbols with the appropriate footprints.

The external file is referred to as an equivalence file, and it stores a mapping of a symbol value to a corresponding footprint. Equivalence files typically use the .equ file extension. Equivalence files are plain text files with a simple syntax, and must be created by the user using a text editor. The syntax is described below.

You can select which equivalence files to use by clicking PreferencesManage Footprint Association Files in the Footprint Assignment Tool.

Managing equivalence files
  • Add new equivalence files by clicking the Add button.

  • Remove the selected equivalence file by clicking the Remove button.

  • Change the priority of equivalence files by clicking the Move Up and Move Down buttons. If a symbol’s value is found in multiple equivalence files, the footprint from the last matching equivalence file will override earlier equivalence files.

  • Open the selected equivalence file by clicking the Edit File button.

Relevant environment variables are shown at the bottom of the window. When the Relative path option is checked, these environment variables will automatically be used to make paths to selected equivalence files relative to the project or footprint libraries.

Once the desired equivalence files have been loaded in the correct order, automatic footprint association can be performed by clicking the Perform automatic footprint assignment icon button in the top toolbar of the Footprint Assignment Tool.

All symbols with a value found in a loaded equivalence file will have their footprints automatically assigned. However, symbols that already have footprints assigned will not be updated.

Format plików

Equivalence files consist of one line for each symbol value. Each line has the following structure:

'<symbol value>' '<footprint library>:<footprint name>'

Each name/value must be surrounded by single quotes (') and separated by one or more spaces. Lines starting with # are comments.

For example, if you want all symbols with the value LM4562 to be assigned the footprint Package_SO:SOIC-8_3.9x4.9_P1.27mm, the line in the equivalence file should be:

'LM4562' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'

Poniżej znajduje się przykład pliku przypisań:

#integrated circuits (smd):
'74LV14' 'Package_SO:SOIC-14_3.9x8.7mm_P1.27mm'
'EL7242C' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'DS1302N' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'LM324N' 'Package_SO:SOIC-14_3.9x8.7mm_P1.27mm'
'LM358' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'LTC1878' 'Package_SO:MSOP-8_3x3mm_P0.65mm'
'24LC512I/SM' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'LM2903M' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'LT1129_SO8' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'LT1129CS8-3.3' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'LT1129CS8' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'LM358M' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'TL7702BID' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'TL7702BCD' 'Package_SO:SOIC-8_3.9x4.9_P1.27mm'
'U2270B' 'Package_SO:SOIC-16_3.9x9.9_P1.27mm'

'LP2985LV' 'Package_TO_SOT_SMD:SOT-23-5_HandSoldering'

Podgląd bieżącego footprintu

The Footprint Assignment Tool contains a footprint viewer. Clicking the footprint viewer icon button in the top toolbar launches the footprint viewer and shows the selected footprint.

Podgląd footprintu

The top toolbar contains the following commands:

refresh 24

Refresh view

zoom in 24

Zoom in

zoom out 24

Zoom out

zoom fit in page 24

Zoom to fit drawing in display area

shape 3d 24

Show 3D viewer

The left toolbar contains the following commands:

cursor 24

Use the select tool

measurement 24

Interactively measure between two points

grid 24

Display grid dots or lines

polar coord 24

Switch between polar and cartesian coordinate systems

unit inch 24

Use inches

unit mil 24

Display coordinates in mils (1/1000 of an inch)

unit mm 24

Display coordinates in millimeters

cursor shape 24

Toggle display of full-window crosshairs

pad number 24

Toggle between drawing pads in sketch or normal mode

pad sketch 24

Toggle between drawing pads in normal mode or outline mode

text sketch 24

Toggle between drawing text in normal mode or outline mode

show mod edge 24

Toggle between drawing graphic lines in normal mode or outline mode

Podgląd bieżącego modelu 3D

Clicking the 3D Viewer icon button opens the footprint in the 3D model viewer.

If a 3D model does not exist for the current footprint, only the footprint itself will be shown in the 3D Viewer.
Podgląd 3D

The 3D Viewer is described in the PCB Editor manual.

Transferring designs between schematic and PCB

Update PCB from Schematic

Use the Update PCB from Schematic tool to sync design information from the Schematic Editor to the Board Editor. The tool can be accessed with ToolsUpdate PCB from Schematic (F8) in both the schematic and board editors. You can also use the Update PCB from Schematic icon icon in the top toolbar of the Board Editor.

Update PCB from Schematic is the preferred way to transfer design information from the schematic to the PCB. In older versions of KiCad, the equivalent process was to export a netlist from the Schematic Editor and import it into the Board Editor. It is no longer necessary to use a netlist file.
Update PCB from schematic

The tool adds the footprint for each symbol to the board and transfers updated schematic information to the board. In particular, the board’s net connections are updated to match the schematic.

The changes that will be made to the PCB are listed in the Changes To Be Applied pane. The PCB is not modified until you click the Update PCB button.

You can show or hide different types of messages using the checkboxes at the bottom of the window. A report of the changes can be saved to a file using the Save…​ button.


The tool has several options to control its behavior.

Option Description

Re-link footprints to schematic symbols based on their reference designators

Footprints are normally linked to schematic symbols via a unique identifier created when the symbol is added to the schematic. A symbol’s unique identifier cannot be changed.

If checked, each footprint in the PCB will be re-linked to the symbol that has the same reference designator as the footprint.

If unchecked, footprints and symbols will be linked by unique identifier as usual, rather than by reference designator. Each footprint’s reference designator will be updated to match the reference designator of its linked symbol.

This option should generally be left unchecked. It is useful for specific workflows that rely on changing the links between schematic symbols and footprints, such as refactoring a schematic for easier layout or replicating layout between identical channels of a design.

Delete footprints with no symbols

If checked, any footprint in the PCB without a corresponding symbol in the schematic will be deleted from the PCB. Footprints with the "Not in schematic" attribute will be unaffected.

If unchecked, footprints without a corresponding symbol will not be deleted.

Replace footprints with those specified in the schematic

If checked, footprints in the PCB will be replaced with the footprint that is specified in the corresponding schematic symbol.

If unchecked, footprints that are already in the PCB will not be changed, even if the schematic symbol is updated to specify a different footprint.

Update Schematic from PCB

TODO: write this section

Backannotation with CMP files

Select changes can also be synced from the PCB back to the schematic by exporting a CMP file from the PCB editor (FileExportFootprint Association (.cmp) File…​) and importing it in the Schematic Editor (FileImportFootprint Assignments…​).

This method can only sync changes made to footprint assignments and footprint fields. It is recommended to use the Update Schematic from PCB tool instead.

Generating Outputs


KiCad can print the schematic to a standard printer using FilePrint…​.

Print dialog

Printing options

Print sheet reference and title block: Include the drawing sheet border and title block in the printed schematic.

Print in black and white only: Print the schematic in black and white rather than color.

Print background color: Include the background color in the printed schematic. This option is only enabled if Print in black and white only is disabled.

Use a different color theme for printing: Select a different color scheme for printing than the one selected for display in the Schematic Editor.

Page Setup…​: Opens a page setup dialog for setting paper size and orientation.

Preview: Opens a print preview dialog.

Close: Closes the dialog without printing.

Print: Opens the system print dialog.

Printing uses platform- and printer-specific drivers and may have unexpected results. When printing to a file, Plotting is recommended instead of Printing.


KiCad can plot schematics to a file using FilePlot…​.

The supported output formats are Postscript, PDF, SVG, DXF, and HPGL.

Plot dialog

The Output Messages pane displays messages about the generated files. Different kinds of messages can be shown or hidden using the checkboxes, and the messages can be saved to a file using the Save…​ button.

The Plot Current Page button plots the current page of the schematic. The Plot All Pages button plots all pages of the schematic. One file is generated for each page, except for PDF output, which plots each schematic page as a separate page in a single PDF file.

Plotting options

Output directory: Specify the location to save plotted files. If this is a relative path, it is created relative to the project directory.

Output Format: Select the format to plot in. Some formats have different options than others.

Page size: Sets the page size to use for the plotted output. This can be set to match the schematic size or to another sheet size.

Plot drawing sheet: Include the drawing sheet border and title block in the printed schematic.

Output mode: Sets the output to color or black and white. Not all output formats support color.

Plot background color: Includes the schematic background color in the plotted output. The background color will not be plotted if the output format does not support color or the output mode is black and white.

Color theme: Selects the color theme to use for the plotted output.

Default line width: Selects the default width for lines without a specified thickness (lines that have thickness set to 0). Lines that have a set thickness will be plotted at that thickness instead.

Position and units: Sets the plotter origin and units. This option only applies for HPGL output.

Pen width: Sets the plotter’s pen width. This option only applies for HPGL output.

Generating a Bill of Materials

KiCad can generate a Bill of Materials using ToolsGenerate BOM…​ or the BOM icon button on the top toolbar. The generated BOM lists all of the components in the design.

Główne okno narzędzia BOM

The BOM tool uses an external script to process the design information into the desired output format. Several BOM generator scripts are included with KiCad, and users can also create their own. BOM generator scripts generally use Python or XSLT, but other tools can be used as long as you can specify a command line for KiCad to execute when running the generator.

You can select which BOM generator to use in the BOM generator scripts list. The rest of the dialog displays information about the selected generator. You can change the displayed name of the generator with the Generator nickname textbox.

The pane at right displays information about the selected script. When the generator is executed, the right pane instead displays output from the script.

The text box at the bottom contains the command that KiCad will use to execute the generator. It is automatically populated when a script is selected, but the command may need to be hand-edited for some generators. KiCad saves the command line for each generator when the BOM tool is closed, so command line customizations are preserved. For more details about the command line, see the advanced documentation.

On Windows, the BOM Generator dialog has an additional option Show console window. When this option is unchecked, BOM generators run in a hidden console window and any output is redirected and printed in the dialog. When this option is checked, BOM generators run in a visible console window, which may be necessary if the generator plugin provides a graphical user interface.

BOM generator scripts

By default, the BOM tool presents two output script options.

  • bom_csv_grouped_by_value outputs a CSV with two sections. The first section contains every component in the design, with a single component on each line. The second section also contains every component, but components are grouped by symbol name, value, and footprint. The columns in the BOM are:

    • Line item number

    • Quantity

    • Reference designator(s)

    • Value

    • Symbol library and symbol name

    • Footprint

    • Datasheet

    • Any other symbol fields

  • bom_csv_grouped_by_value_with_fp outputs a CSV with a single section containing every component in the design. Components are grouped by value and footprint. The columns in the BOM are:

    • Reference designator(s)

    • Quantity

    • Value

    • Symbol name

    • Footprint

    • Symbol description

    • Vendor

Additional generator scripts are installed with KiCad but are not populated in the generator script list by default. The location of these scripts depends on the operating system and may vary based on installation location.

Operating System Location


C:\Program Files\KiCad\6.0\bin\scripting\plugins\





Additional scripts can be added to the list of BOM generator scripts by clicking the Plus icon button. Scripts can be removed by clicking the Delete icon button. The Edit icon button opens the selected script in a text editor.

For more information on creating and using custom BOM generators, see the advanced documentation.


A netlist is a file which describes electrical connections between symbol pins. These connections are referred to as nets. Netlist files contain:

  • A list of symbols and their pins.

  • A list of connections (nets) between symbol pins.

Many different netlist formats exist. Sometimes the symbols list and the list of nets are two separate files. This netlist is fundamental in the use of schematic capture software, because the netlist is the link with other electronic CAD software, such as PCB layout software, simulators, and programmable logic compilers.

KiCad supports several netlist formats:

  • KiCad format, which can be imported by the KiCad PCB Editor. However, the "Update PCB from Schematic" tool should be used instead of importing a KiCad netlist into the PCB editor.

  • OrCAD PCB2 format, for designing PCBs with OrCAD.

  • CADSTAR format, for designing PCBs with CADSTAR.

  • Spice format, for use with various external circuit simulators.

In KiCad version 5.0 and later, it is not necessary to create a netlist for transferring a design from the schematic editor to the PCB editor. Instead, use the "Update PCB from Schematic" tool.
Other software tools that use netlists may have restrictions on spaces and special characters in component names, pins, nets, and other fields. For compatibility, be aware of such restrictions in other tools you plan to use, and name components, nets, etc. accordingly.

Format listy sieci

Netlists are exported with the Export Netlist dialog (FileExportNetlist…​).

KiCad netlist export

KiCad supports exporting netlists in several formats: KiCad, OrcadPCB2, CADSTAR, and Spice. Each format can be selected by selecting the corresponding tab at the top of the window. Some netlist formats have additional options.

Clicking the Export Netlist button prompts for a netlist filename and saves the netlist.

Netlist generation can take up to several minutes for large schematics.

Custom generators for other netlist formats can be added by clicking the Add Generator…​ button. Custom generators are external tools that are called by KiCad, for example Python scripts or XSLT stylesheets. For more information on custom netlist generators, see the section on adding custom netlist generators.

Spice Netlist Format
Spice netlist export

The Spice netlist format offers several options.

When the Reformat passive symbol values box is checked, passive symbol values will be adjusted to be compatible with Spice. Specifically:

  • μ and M as unit prefixes are replaced with u and Meg, respectively

  • Units are removed (e.g. 4.7kΩ is changed to 4.7k)

  • Values in RKM format are rewritten to be Spice-compatible (e.g. 4u7 is changed to 4.7u)

The Spice netlist exporter also provides an easy way to simulate the generated netlist with an external simulator. This can be useful for running a simulation without using KiCad’s internal ngspice simulator, or for running an ngspice simulation with options that are not supported by KiCad’s simulator tool.

Enter the path to the external simulator in the text box, with %I representing the generated netlist. Click the Create Netlist and Run Simulator Command button to generate the netlist and automatically run the simulator.

The default simulator command (spice "%I") must be adjusted to point to a simulator installed on your system.

Spice simulators expect simulation commands (.PROBE, .AC, .TRAN, etc.) to be included in the netlist. Any text line included in the schematic diagram starting with a period (.) will be included in the netlist. If a text object contains multiple lines, only the lines beginning with a period will be included.

.include directives for including model library files are automatically added to the netlist based on the Spice model settings for the symbols in the schematic.

Przykłady list sieci

Below is the schematic from the sallen_key project included in KiCad’s simulation demos.

sallen_key demo schematic

The KiCad format netlist for this schematic is as follows:

(export (version "E")
    (source "/usr/share/kicad/demos/simulation/sallen_key/sallen_key.kicad_sch")
    (date "Sun 01 May 2022 03:14:05 PM EDT")
    (tool "Eeschema (6.0.4)")
    (sheet (number "1") (name "/") (tstamps "/")
        (source "sallen_key.kicad_sch")
        (comment (number "1") (value ""))
        (comment (number "2") (value ""))
        (comment (number "3") (value ""))
        (comment (number "4") (value ""))
        (comment (number "5") (value ""))
        (comment (number "6") (value ""))
        (comment (number "7") (value ""))
        (comment (number "8") (value ""))
        (comment (number "9") (value "")))))
    (comp (ref "C1")
      (value "100n")
      (libsource (lib "sallen_key_schlib") (part "C") (description ""))
      (property (name "Sheetname") (value ""))
      (property (name "Sheetfile") (value "sallen_key.kicad_sch"))
      (sheetpath (names "/") (tstamps "/"))
      (tstamps "00000000-0000-0000-0000-00005789077d"))
    (comp (ref "C2")
      (value "100n")
        (field (name "Fieldname") "Value")
        (field (name "SpiceMapping") "1 2")
        (field (name "Spice_Primitive") "C"))
      (libsource (lib "sallen_key_schlib") (part "C") (description ""))
      (property (name "Fieldname") (value "Value"))
      (property (name "Spice_Primitive") (value "C"))
      (property (name "SpiceMapping") (value "1 2"))
      (property (name "Sheetname") (value ""))
      (property (name "Sheetfile") (value "sallen_key.kicad_sch"))
      (sheetpath (names "/") (tstamps "/"))
      (tstamps "00000000-0000-0000-0000-00005789085b"))
    (comp (ref "R1")
      (value "1k")
        (field (name "Fieldname") "Value")
        (field (name "SpiceMapping") "1 2")
        (field (name "Spice_Primitive") "R"))
      (libsource (lib "sallen_key_schlib") (part "R") (description ""))
      (property (name "Fieldname") (value "Value"))
      (property (name "SpiceMapping") (value "1 2"))
      (property (name "Spice_Primitive") (value "R"))
      (property (name "Sheetname") (value ""))
      (property (name "Sheetfile") (value "sallen_key.kicad_sch"))
      (sheetpath (names "/") (tstamps "/"))
      (tstamps "00000000-0000-0000-0000-0000578906ff"))
    (comp (ref "R2")
      (value "1k")
        (field (name "Fieldname") "Value")
        (field (name "SpiceMapping") "1 2")
        (field (name "Spice_Primitive") "R"))
      (libsource (lib "sallen_key_schlib") (part "R") (description ""))
      (property (name "Fieldname") (value "Value"))
      (property (name "SpiceMapping") (value "1 2"))
      (property (name "Spice_Primitive") (value "R"))
      (property (name "Sheetname") (value ""))
      (property (name "Sheetfile") (value "sallen_key.kicad_sch"))
      (sheetpath (names "/") (tstamps "/"))
      (tstamps "00000000-0000-0000-0000-000057890691"))
    (comp (ref "U1")
      (value "AD8051")
        (field (name "Spice_Lib_File") "ad8051.lib")
        (field (name "Spice_Model") "AD8051")
        (field (name "Spice_Netlist_Enabled") "Y")
        (field (name "Spice_Primitive") "X"))
      (libsource (lib "sallen_key_schlib") (part "Generic_Opamp") (description ""))
      (property (name "Spice_Primitive") (value "X"))
      (property (name "Spice_Model") (value "AD8051"))
      (property (name "Spice_Lib_File") (value "ad8051.lib"))
      (property (name "Spice_Netlist_Enabled") (value "Y"))
      (property (name "Sheetname") (value ""))
      (property (name "Sheetfile") (value "sallen_key.kicad_sch"))
      (sheetpath (names "/") (tstamps "/"))
      (tstamps "00000000-0000-0000-0000-00005788ff9f"))
    (comp (ref "V1")
      (value "AC 1")
      (libsource (lib "sallen_key_schlib") (part "VSOURCE") (description ""))
      (property (name "Sheetname") (value ""))
      (property (name "Sheetfile") (value "sallen_key.kicad_sch"))
      (sheetpath (names "/") (tstamps "/"))
      (tstamps "00000000-0000-0000-0000-000057336052"))
    (comp (ref "V2")
      (value "DC 10")
        (field (name "Fieldname") "Value")
        (field (name "Spice_Node_Sequence") "1 2")
        (field (name "Spice_Primitive") "V"))
      (libsource (lib "sallen_key_schlib") (part "VSOURCE") (description ""))
      (property (name "Fieldname") (value "Value"))
      (property (name "Spice_Primitive") (value "V"))
      (property (name "Spice_Node_Sequence") (value "1 2"))
      (property (name "Sheetname") (value ""))
      (property (name "Sheetfile") (value "sallen_key.kicad_sch"))
      (sheetpath (names "/") (tstamps "/"))
      (tstamps "00000000-0000-0000-0000-0000578900ba"))
    (comp (ref "V3")
      (value "DC 10")
        (field (name "Fieldname") "Value")
        (field (name "Spice_Node_Sequence") "1 2")
        (field (name "Spice_Primitive") "V"))
      (libsource (lib "sallen_key_schlib") (part "VSOURCE") (description ""))
      (property (name "Fieldname") (value "Value"))
      (property (name "Spice_Primitive") (value "V"))
      (property (name "Spice_Node_Sequence") (value "1 2"))
      (property (name "Sheetname") (value ""))
      (property (name "Sheetfile") (value "sallen_key.kicad_sch"))
      (sheetpath (names "/") (tstamps "/"))
      (tstamps "00000000-0000-0000-0000-000057890232")))
    (libpart (lib "sallen_key_schlib") (part "C")
        (fp "C?")
        (fp "C_????_*")
        (fp "C_????")
        (fp "SMD*_c")
        (fp "Capacitor*"))
        (field (name "Reference") "C")
        (field (name "Value") "C"))
        (pin (num "1") (name "") (type "passive"))
        (pin (num "2") (name "") (type "passive"))))
    (libpart (lib "sallen_key_schlib") (part "Generic_Opamp")
        (field (name "Reference") "U")
        (field (name "Value") "Generic_Opamp"))
        (pin (num "1") (name "+") (type "input"))
        (pin (num "2") (name "-") (type "input"))
        (pin (num "3") (name "V+") (type "power_in"))
        (pin (num "4") (name "V-") (type "power_in"))
        (pin (num "5") (name "") (type "output"))))
    (libpart (lib "sallen_key_schlib") (part "R")
        (fp "R_*")
        (fp "Resistor_*"))
        (field (name "Reference") "R")
        (field (name "Value") "R"))
        (pin (num "1") (name "") (type "passive"))
        (pin (num "2") (name "") (type "passive"))))
    (libpart (lib "sallen_key_schlib") (part "VSOURCE")
        (field (name "Reference") "V")
        (field (name "Value") "VSOURCE")
        (field (name "Fieldname") "Value")
        (field (name "Spice_Primitive") "V")
        (field (name "Spice_Node_Sequence") "1 2"))
        (pin (num "1") (name "") (type "input"))
        (pin (num "2") (name "") (type "input")))))
    (library (logical "sallen_key_schlib")
      (uri "/usr/share/kicad/demos/simulation/sallen_key/sallen_key_schlib.kicad_sym")))
    (net (code "1") (name "/lowpass")
      (node (ref "C1") (pin "1") (pintype "passive"))
      (node (ref "U1") (pin "2") (pinfunction "-") (pintype "input"))
      (node (ref "U1") (pin "5") (pintype "output")))
    (net (code "2") (name "GND")
      (node (ref "C2") (pin "2") (pintype "passive"))
      (node (ref "V1") (pin "2") (pintype "input"))
      (node (ref "V2") (pin "2") (pintype "input"))
      (node (ref "V3") (pin "1") (pintype "input")))
    (net (code "3") (name "Net-(C1-Pad2)")
      (node (ref "C1") (pin "2") (pintype "passive"))
      (node (ref "R1") (pin "1") (pintype "passive"))
      (node (ref "R2") (pin "2") (pintype "passive")))
    (net (code "4") (name "Net-(C2-Pad1)")
      (node (ref "C2") (pin "1") (pintype "passive"))
      (node (ref "R2") (pin "1") (pintype "passive"))
      (node (ref "U1") (pin "1") (pinfunction "+") (pintype "input")))
    (net (code "5") (name "Net-(R1-Pad2)")
      (node (ref "R1") (pin "2") (pintype "passive"))
      (node (ref "V1") (pin "1") (pintype "input")))
    (net (code "6") (name "VDD")
      (node (ref "U1") (pin "3") (pinfunction "V+") (pintype "power_in"))
      (node (ref "V2") (pin "1") (pintype "input")))
    (net (code "7") (name "VSS")
      (node (ref "U1") (pin "4") (pinfunction "V-") (pintype "power_in"))
      (node (ref "V3") (pin "2") (pintype "input")))))

In Spice format, the netlist is as follows:

.title KiCad schematic
.include "ad8051.lib"
XU1 Net-_C2-Pad1_ /lowpass VDD VSS /lowpass AD8051
C2 Net-_C2-Pad1_ GND 100n
C1 /lowpass Net-_C1-Pad2_ 100n
R2 Net-_C2-Pad1_ Net-_C1-Pad2_ 1k
R1 Net-_C1-Pad2_ Net-_R1-Pad2_ 1k
V1 Net-_R1-Pad2_ GND AC 1
.ac dec 10 1 1Meg

Managing Symbol Libraries

Biblioteki symboli przechowują zbiory symboli używanych podczas tworzenia schematów. Każdy symbol na schemacie jest jednoznacznie identyfikowany za pomocą pełnej nazwy, która składa się z nazwy skrótowej biblioteki i nazwy symbolu. Przykładowo Audio:AD1853.

Tabele Bibliotek Symboli

KiCad uses a table of symbol libraries to map symbol libraries to a library nickname. 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…​.

Okno ustawień bibliotek

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.

Konfiguracja początkowa

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 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.

Substytucja zmiennych środowiskowych

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:

  • ${KIPROJMOD} points to the current project directory and cannot be modified.

  • ${KICAD6_FOOTPRINT_DIR} points to the default location of KiCad’s standard footprint libraries.

  • ${KICAD6_SYMBOL_DIR} points to the default location of KiCad’s standard symbol libraries.

  • ${KICAD6_3DMODEL_DIR} points to the default location of KiCad’s standard 3D model libraries.

  • ${KICAD6_TEMPLATE_DIR} points to the default location of KiCad’s standard template library.

${KIPROJMOD} cannot be redefined, but the other environment variables can be redefined and new environment variables added in the PreferencesConfigure 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.

${KIPROJMOD} 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. One of the most powerful features of the symbol library table is environment variable substitution. This allows for definition of custom paths to where symbol libraries are stored in environment variables. Environment variable substitution is supported by using the syntax ${ENV_VAR_NAME} in the library path.

Zakres stosowania

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.

Każda z tych metod ma swoje wady i zalety. Zdefiniowanie wszystkich bibliotek w tabeli globalnej oznacza, że będą one zawsze dostępne w razie potrzeby. Wadą tego rozwiązania jest to, że czas ich ładowania znacznie wzrośnie.

Definiowanie wszystkich bibliotek symboli w ustawieniach konkretnego projektu oznacza, że ładowane są tylko biblioteki wymagane dla projektu co zmniejsza ich czas ładowania. Wadą jest to, że zawsze należy pamiętać o skonfigurowaniu wymaganych bibliotek dla każdego projektu.

Jednym ze sposobów użycia mogłoby być zdefiniowanie powszechnie używanych bibliotek globalnie, a bibliotek wymaganych tylko dla projektu w tabelach bibliotek specyficznych dla projektu. Nie pod tym względem żadnych ograniczeń.

Migrating Legacy 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.

Remapowanie projektów z poprzednich wersji

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:

  • oryginalne biblioteki użyte w schemacie są nadal dostępne i niezmienione od momentu dodania symbolu do schematu.

  • wszystkie operacje ratunkowe zostały wykonane po wykryciu potrzeby utworzenia biblioteki ratunkowej lub aktualizacji istniejącej biblioteki ratunkowej.

  • integralność symboli bibliotecznych w pamięci podręcznej projektu nie została naruszona.

Remapowanie spowoduje utworzenie kopii zapasowej wszystkich plików, które zostały zmienione podczas ponownego mapowania w folderze rescue-backup w folderze projektu. Zawsze należy utworzyć kopie zapasowe projektu przed zmianą przypisań na wypadek gdyby coś poszło nie tak.

Operacja odzyskiwania jest wykonywana nawet jeśli została wyłączona, aby zabezpieczyć poprawność symboli do procesu ponownego mapowania. Nie powinno się anulować tej operacji, inaczej ponowne mapowanie się nie powiedzie. Wszelkie uszkodzone łącza symboliczne muszą wtedy zostać naprawione ręcznie.

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.

Symbol Editor

Podstawowe informacje na temat bibliotek

A symbol is a schematic element which contains a graphical representation, electrical connections, and text fields describing the symbol. Symbols used in a schematic are stored in symbol libraries. 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. The symbol editing tool provides a simple way to manage symbols and symbol libraries.

Biblioteki symboli - Przegląd

Biblioteka symboli składa się z jednego bądź wielu komponentów. Generalnie, komponenty są logicznie pogrupowane biorąc pod uwagę np. ich funkcję, typ, bądź producenta.

Symbol znajdujący się w bibliotece jest złożony z:

  • 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.

  • Pól (tekstowych) takich jak oznaczenie, wartość, nazwa footprintu potrzebna do wstawienia go na płytkę.

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.

Do poprawnego tworzenia symboli wymagane jest:

  • Zdefiniowanie ogólnych właściwości: czy posiada wiele części składowych.

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

  • Projektowanie wyglądu (z wyjątkiem pinów) z użyciem linii, prostokątów, okręgów, wielokątów i tekstów.

  • Dodanie wyprowadzeń, dokładnie określając ich projekt graficzny, nazwę oraz numer pinu, a także ich właściwości elektryczne (wejście, wyjście, trzy-stanowe, port zasilania, itp.).

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

  • Dodanie pól w razie potrzeby (jest to opcjonalne, nazwa modułu jest wykorzystywany przez oprogramowanie PCB) i/lub określenie ich widoczności.

  • Dokumentowanie składnika np. poprzez dodanie słów kluczowych i adresu dokumentacji w sieci lub na lokalnym nośniku.

  • Zapisanie go do wybranej biblioteki.

Edytor bibliotek symboli - Przegląd

Widok głównego okna edytora bibliotek symboli znajduje się poniżej. Edytor składa się z trzech pasków narzędzi z szybkim dostępem do podstawowych narzędzi i obszaru podglądu/edycji komponentów. Nie wszystkie polecenia są dostępne na paskach narzędzi, ale można uzyskać do nich dostęp za pomocą menu.

Symbol Editor main window

Główny pasek menu

The main tool bar is located at the top of the main window. It consists of the undo/redo commands, zoom commands, symbol properties dialogs, and unit/representation management controls.

Symbol Editor toolbar

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 tablular interface.

Datasheet icon

Open the symbol’s datasheet. The button will be disabled if no datasheet is defined for the current symbol.

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 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.

Pasek narzędzi edycji symbolu

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

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.

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.

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.

Pasek opcji

The vertical tool bar located on the left hand side of the main window allows you to set some of the editor drawing options.

Grid icon

Toggle grid visibility 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 libraries and symbols.

Wybór bibliotek i zarządzanie nimi

The selection of the current library is possible via the Symbol tree icon icon which shows you all available libraries and allows you to select one. When a symbol is loaded or saved, it will be put in this library. The library name of a symbol is the contents of its Value field.

Wybór i zapis symbolu

Wybór symbolu

Clicking the Symbol tree icon icon on the left tool bar toggles the treeview of libraries and symbols. Clicking on a symbol opens that 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.
Zapisywanie symbolu

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. The modifications will be written to the existing symbol.

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 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 FileExportSymbol…​. This file will be a standard library file which will contain only one symbol.

Tworzenie symboli biblliotecznych

Tworzenie nowego symbolu

A new symbol can be created by clicking the New symbol icon icon. You will be asked for a number of symbol properties.

  • A symbol name (this name is used as the default value for the Value field in the schematic editor)

  • 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 is made of 4 units per package).

  • 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 Port" dialog in the Schematic editor, their Value fields are not editable in the schematic, they cannot be assigned a footprint and they are not added to the PCB, and they are not included in the 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

Nowy symbol będzie utworzony z użyciem powyższych właściwości i pojawi się w oknie edycyjnym jak pokazano poniżej.

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 icon and clicking on the new desired anchor position.

Tworzenie nowego symbolu na podstawie innego

Często symbol który chcemy utworzyć bardzo przypomina inny symbol, który znajduje się już w bibliotece. W tym przypadku łatwiej jest zmodyfikować istniejący symbol.

  • Załadować symbol który będzie użyty jako wzorcowy.

  • Save a new copy of the symbol using FileSave As…​. The Save As dialog will prompt for a name for the new symbol and the library to save it in.

  • Wykonać niezbędne edycje.

  • Save the modified symbol.

Właściwości symbolu

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 icon to show the dialog below.

Właściwości symbolu

It is important to correctly set the number of units per package and the alternate symbolic representation, if enabled, because when pins are edited or created the corresponding pins for each unit will be affected. If you change the number of units per package after pin creation and editing, there will be additional work to specify the pins and graphics for the new unit. 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.

Poniższy przykład pokazuje symbol, w którym opcja "Umieść nazwę pinu wewnątrz" została odznaczona. Należy zwrócić uwagę na położenie nazw i numerów pinów.

Place pin name inside unchecked
Symbol Name, Description, and Keywords

The symbol’s name is the same as the Value field. When the symbol name is changed the value also changes, and vice versa. The symbol’s name in the library also changes accordingly.

The symbol description should contain a brief description of the component, such as the component function, distinguishing features, and package options. The keywords should contain additional terms related to the component. Keywords are used primarily to assist in searching for the symbol.

Searching for a symbol in the add a symbol dialog

A symbol’s name, description, and keywords are all used when searching for symbols in the Symbol Editor and Add a Symbol dialog. The description and keywords are displayed in the Symbol Library Browser and Add a Symbol dialog.

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

Symbole wieloczęściowe i podwójna reprezentacja

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. Use the images/toolbar_libedit_part.png dropdown shown below to select the unit you wish to edit.

Selecting a symbol unit

Elementy graficzne symbolu

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

  • Linie i linie łamane są definiowane poprzez punkty startowe i końcowe.

  • Prostokąty są definiowane przez punkty dwóch przeciwległych narożników.

  • Okręgi są definiowane przez punkt centralny i promień.

  • Łuki są definiowane przez punkt początkowy i końcowy łuku oraz ich punkt centralny. Kąt rozwarcia łuku może zawierać się w przedziale 0° to 180°.

Pasek narzędzi po prawej stronie głównego okna pozwala na umieszczanie w polu roboczym wszystkich podstawowych elementów graficznych potrzebnych do zaprojektowania symbolu w obu jego postaciach.

Przynależność elementów graficznych

Każdy z elementów graficznych (linia, łuk, okrąg, itd.) może być określona jako część wspólna dla wszystkich części składowych lub stylów, albo specyficzna dla nich. Opcje dotyczące przynależności elementu graficznego można łatwo wyświetlić klikając prawym klawiszem myszy nad wybranym elementem wywołując menu podręczne. Poniżej przykład menu dla elementu typu linia.

Graphic line context menu

Można także kliknąć dwukrotnie na taki element by zmodyfikować jego właściwości. Poniżej przykład dla elementu typu linia łamana.

Graphic line properties

Głównymi właściwościami dla elementów graficznych są:

  • "Line width" defines the width of the element’s line in the current drawing units.

  • "Fill Style" determines if the shape defined by the graphical element is to be drawn unfilled, background filled, or foreground filled.

  • "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.

Tekst jako grafika w symbolu

The Text icon icon allows for the creation of graphical text. Graphical text is automatically oriented to be readable, even when the symbol is mirrored. Please note that graphical text items are not the same as symbol fields.

Symbole wieloczęściowe, podwójna reprezentacja symboli

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.

Consider for instance 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).

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.

"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.
Elementy geometryczne w symbolach

Shown below are properties for a graphic body element. In the relay example above, the three units have different symbolic representations. Therefore, each unit was created separately and the graphical body elements have the "Common to all units in symbol" setting disabled.

Disable common to all units in symbol

Tworzenie i edycja wyprowadzeń (pinów)

You can click on the Pin icon icon to create and insert a pin. The editing of all pin properties is done by double-clicking on the pin or right-clicking on the pin to open the pin context menu. Pins must be created carefully, because any error will have consequences on the PCB design. Any pin already placed can be edited, deleted, and/or moved.

Wyprowadzenia - Informacje podstawowe

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.

Ważne uwagi:

  • 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 (overline) 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.

Właściwości wyprowadzeń

Pin properties

Okno z właściwościami pinu pozwala na zmiany charakterystycznych cech wyprowadzeń. Okno to ukazuje się zawsze podczas tworzenia nowego pinu, albo gdy w pin zostanie kliknięty dwukrotnie myszą. Jego zawartość pozwala na zdefiniowanie lub modyfikację parametrów takich jak:

  • The pin name and text size.

  • The pin number and text size.

  • The pin length.

  • The pin electrical type and graphical style.

  • Przynależność do części i alternatywnej reprezentacji.

  • Pin visibility.

  • Alternate pin definitions.

Pin Graphic Styles

Shown in the figure below are the different pin graphic styles. The choice of graphic style does not have any influence on the pin’s electrical type.

Pin graphic styles

Typy elektryczne

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.

Pin Type



A pin which is exclusively an input.


A pin which is exclusively an output.


A pin that can be either an input or an output, such as a microcontroller data bus pin.


A three state output pin (high, low, or high impedance)


A passive symbol pin: resistors, connectors, etc.


A pin that can be freely connected to any other pin without electrical concerns.


A pin for which the ERC check does not matter.

Power input

A symbol’s power pin. As a special case, power input pins that are marked invisible are automatically connected to the net with the same name. See the Power Ports section for more information.

Power output

A pin that provides power to other pins, such as a regulator output.

Open collector

An open collector logic output.

Open emitter

An open emitter logic output.


A pin that should not be connected to anything.

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.

Pin context menu

Określanie pinów w symbolach wieloczęściowych i podwójna reprezentacja

Symbols with multiple units and/or graphical representations are particularly problematic when creating and editing pins. The majority of 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 images/toolbar_libedit_alias.png 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.

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 quad opamp.

Pin table

Alternate Pin Definitions

Pins can have alternate pin definitions added to them. Alternate pin definitions 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 definitions 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 definitions are selected in the Schematic Editor once the symbol has been placed in the schematic. The alternate pin is assigned in the Alternate Pin Assignments tab of the Symbol Properties dialog. Alternate definitions are selectable in the dropdown in the Alternate Assignment column.

Selecting an alternate pin definition

Pola symboli

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 and value fields are required.

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.

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.

Edycja pól symboli

By dokonać edycji istniejącego pola symbolu, należy kliknąć prawym klawiszem na polu tekstowym by wywołać menu kontekstowe pokazane poniżej.

Symbol field context menu

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 are text information associated a the symbol. Do not confuse them with text in the graphic representation of a symbol.

Ważne uwagi:

  • Modifying the Value field changes the name of the symbol. The symbol’s name in the library will change when the symbol is saved.

  • The Symbol Properties dialog must be used to edit a field that is empty or has the invisible attribute enabled because such fields cannot be clicked on.

  • The footprint is defined as an absolute footprint using the LIBNAME:FOOTPRINTNAME format where LIBNAME is the name of the footprint library defined 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.

Creating Power Port Symbols

Power ports, or power symbols, are symbols that are used to label a wire as part of a power net, like VCC or GND. The behavior of power ports 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 Port" dialog for convenient access.

Below is an example of a GND power symbol.

Editing a power symbol

Power port 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.

If the power symbol has the "Define as power symbol" property checked, the power input pin does not need to be marked invisible. However, the convention is to make these pins invisible anyway.
Power symbol pin

By utworzyć port zasilania, należy wykonać następujące kroki:

  • Add a pin of type "Power input", with "Visible" unchecked, and the pin named according to the desired net. Make the pin number 1, the length 0, and set the graphic style to "Line". The pin name establishes the connection to the net; in this case the pin will automatically connect to the net GND. The pin number, length, and line style do not matter electrically.

  • Place the pin on the symbol anchor.

  • Use the shape tools to draw the symbol graphics.

  • Set the symbol value. The symbol value does not matter electrically, but it is displayed in the schematic. To eliminate confusion, it should match the pin name (which determines the connected net name).

  • Check the "Define as power symbol" box in Symbol Properties window. This makes the symbol appear in the "Add Power Port" dialog, makes the Value field read-only in the schematic, prevents the symbol from being assigned a footprint, and excludes the symbol from the board, BOM, and netlists.

  • 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 port 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 port’s reference does not begin with #, the character will be inserted automatically when the annotation or footprint assignment tools are run.

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

The connected net name is determined by the power port’s pin name, not the name or value of the symbol. When modifying an existing power port symbol, make sure to rename the pin so that the new symbol connects to the appropriate power net. This means that power port net names can only be changed in the symbol editor, not in the schematic.

Przeglądanie bibliotek symboli


The Symbol Library Browser allows you to quickly examine the content of symbol libraries. The Symbol Library Viewer can be accessed by clicking Library viewer icon icon on the main toolbar, ViewSymbol Library Browser…​, or clicking Select With Browser in the "Choose Symbol" window.

Okno przeglądarki

Ekran główny

Wybór biblioteki

By sprawdzić zawartość biblioteki należy wybrać ją z listy znajdującej się po lewej stronie okna. Wszystkie symbole zostaną pokazane na drugiej liście. Należy wybrać nazwę symbolu by móc go podejrzeć w panelu po prawej stronie.

Wybór symbolu

Pasek narzędzi Przeglądarki Bibliotek Symboli

Podstawowy pasek narzędzi wygląda następująco.


Dostępne polecenia to:

Symbol selection icon

Selection of the symbol which can be also selected in the displayed list.

Previous symbol icon

Display previous symbol.

Next symbol icon

Display next symbol.

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

Zoom tools.

morgan1 24 morgan2 24

Selection of the representation (normal or alternate) if an alternate representation exists.


Selection of the unit for symbols that contain multiple units.


If they exist, display the associated documents.

Add symbol to schematic icon

Close the browser and place the selected symbol in the schematic.


KiCad provides an embedded electrical circuit simulator using ngspice as the simulation engine.

Podczas pracy z symulatorem przydatna może być oficjalna biblioteka pspice. Zawiera ona popularne symbole używane do symulacji, takie jak źródła napięcia/prądu lub tranzystory z pinami ponumerowanymi tak, aby pasowały do specyfikacji węzłów ngspice.

Istnieje również kilka projektów demonstracyjnych ilustrujących możliwości symulatora. Znajdziesz je w katalogu demos/simulation.

Przypisywanie modeli

Przed uruchomieniem symulacji komponenty muszą mieć przypisany modele Spice.

Każdy komponent może mieć przypisany tylko jeden model, nawet jeśli komponent składa się z wielu jednostek. W takim przypadku pierwsza jednostka powinna mieć określony model.

Komponenty pasywne z referencją pasującą do typu urządzenia w zapisie Spice (R* dla rezystorów, C* dla kondensatorów, L* dla cewek indukcyjnych) będą miały przypisane modele niejawnie i będą używać pola Wartość do określania ich właściwości.

Należy pamiętać, że w Spice zapis 'M' oznacza mili, a 'Meg' odpowiada Mega. Jeśli wolisz użyć 'M' do wskazania prefiksu Mega, możesz o tym zdecydować w ustawieniach symulatora.

Informacje o modelu Spice są zapisywane jako tekst w polach symboli, dlatego możesz je zdefiniować w edytorze symboli lub edytorze schematów. Otwórz okno dialogowe właściwości symbolu i kliknij przycisk "Edytuj model Spice", aby otworzyć okno dialogowe "Edytora Modeli Spice".

Okno dialogowe "Edytor Modelu Spice" ma trzy zakładki odpowiadające różnym typom modeli. Istnieją dwie opcje wspólne dla wszystkich typów modeli:

Disable symbol for simulation

When checked the component is excluded from simulation.

Alternate node sequence

Allows one to override symbol pin to model node mapping. To define a different mapping, specify pin numbers in order expected by the model.


* connections:
* 1: non-inverting input
* 2: inverting input
* 3: positive power supply
* 4: negative power supply
* 5: output
.subckt tl071 1 2 3 4 5

Generic operational amplifier symbol

To match the symbol pins to the Spice model nodes shown above, one needs to use an alternate node sequence option with value: "1 3 5 2 4". It is a list of pin numbers corresponding to the Spice model nodes order.


Zakładka Pasywne pozwala użytkownikowi przypisać pasywny model (rezystor, kondensator lub cewka) do komponentu. Jest to rzadko używana opcja, ponieważ zwykle elementy pasywne mają niejawnie przypisane modele, chyba że odniesienie do komponentu nie jest zgodne z rzeczywistym typem urządzenia.

Jawnie zdefiniowane model pasywne mają pierwszeństwo przed tymi, które są domyślnie przypisane. Oznacza to, że po przypisaniu pasywnego modelu, pola Odnośnik i Wartość nie są brane pod uwagę podczas symulacji. Może to prowadzić do niejasnej sytuacji, gdy przypisana wartość modelu nie jest zgodna z tą wyświetlaną na schemacie.
Zakładka edytora modelu pasywnego


Wybór typu elementu (rezystor, kondensator lub cewka).


Definiuje właściwości komponentu (rezystancja, pojemność lub indukcyjność). Wartość może używać popularnych przedrostków jednostek Spice (wymienionych poniżej pola wprowadzania tekstu) i powinien używać kropki jako separatora dziesiętnego. Zauważ, że interpreter Spice nie działa poprawnie gdy przedrostki przeplatają się w wartości (np. 1k5).


Zakładka Model służy do przypisania półprzewodnika lub złożonego modelu zdefiniowanego w zewnętrznym pliku biblioteki. Biblioteki modeli Spice są często oferowane przez producentów urządzeń.

Główny widżet tekstowy wyświetla wybraną zawartość z pliku bibliotecznego. Powszechną praktyką jest umieszczanie opisu modeli w plikach biblioteki, w tym kolejności węzłów.

Zakładka edytora modelu półprzewodnikowego lub złożonego


Ścieżka do pliku bibliotecznego Spice. Ten plik będzie używany przez symulator, tak jak jest dodawany za pomocą dyrektywy .include.


Wybrany model komponentu. Po wybraniu pliku lista jest wypełniana modelami do wyboru.


Wybór typu modelu (inny układ, BJT, MOSFET lub dioda). Zwykle jest ustawiony automatycznie po wybraniu modelu.


Zakładka Źródło służy do przypisania modelu źródła zasilania lub sygnału. Dostępne są dwie sekcje: Analiza DC/AC oraz Analiza czasowa. Każdy definiuje parametry źródłowe dla odpowiedniego typu symulacji.

Opcja Typ źródła jest aktywna dla wszystkich typów symulacji.

Zakładka edytora modeli źródeł

Więcej na temat źródeł w dokumentacji ngspice, rodział 4 (Voltage and Current Sources).

Dyrektywy Spice

It is possible to add Spice directives by placing them in text fields on a schematic sheet. This approach is convenient for defining the default simulation type. This functionality is limited to Spice directives starting with a dot (e.g. .tran 10n 1m), it is not possible to place additional components using text fields.


Aby uruchomić symulację, otwórz okno dialogowe Symulator Spice wybierając menu NarzędziaSymulator w oknie edytora schematów.

Główne okno symulacji

Okno dialogowe posiada kilka sekcji:

Menu Plik

Nowy wykres

Tworzy nową kartę w panelu wykresów.

Otwórz skoroszyt

Otwiera listę kreślonych sygnałów.

Zapisz skoroszyt

Zapisuje listę kreślonych sygnałów.

Zapisz jako obraz

Eksportuje aktywny wykres do pliku .png.

Zapisz jako plik .csv

Eksportuje aktywne punkty danych surowych wykresu do pliku .csv.

Wyjdź z symulacji

Zamyka okno dialogowe.


Uruchom symulację

Wykonuje symulację przy użyciu bieżących ustawień.

Dodaj sygnały…​

Otwiera okno dialogowe wyboru sygnałów do kreślenia.

Sondy ze schematu

Uruchamia narzędzie typu Sonda.

Dostrój wartość komponentu

Uruchom narzędzie Tuner.

Pokaż listę sieci SPICE…​

Otwiera okno dialogowe pokazujące wygenerowaną listę sieci symulowanego obwodu.


Otwiera okno dialogowe ustawień symulacji.

Menu Widok


Powiększa aktywny wykres.


Zmniejsza aktywny wykres.

Dopasuj do ekranu

Dostosuj ustawienie powiększenia, aby wyświetlić wszystkie wykresy.

Pokaż siatkę

Włącza widoczność siatki.

Pokaż legendę

Przełącz widoczność legendy wykresu.

Pasek narzędziowy

Pasek narzędziowy symulatora

Ten pasek umożliwia dostęp do głównych funkcji symulatora.

Uruchom/Zatrzymaj symulację

Uruchamia lub zatrzymuje symulację.

Dodaj sygnały

Otwiera okno dialogowe wyboru sygnałów do wykreślenia.


Uruchamia narzędzie Sonda.


Uruchamia narzędzie do dostrajania.


Otwiera okno dialogowe ustawień symulacji.

Panel wykresu

Pokazuje wyniki symulacji w formie wykresów. W oddzielnych zakładkach można otworzyć wiele wykresów, ale tylko aktywny jest aktualizowany podczas przeprowadzania symulacji. W ten sposób można porównać wyniki symulacji dla różnych przebiegów.

Wykresy można dostosowywać, zmieniając widoczność siatki i legendy za pomocą menu menu Widok. Kiedy legenda jest widoczna, można ją przeciągnąć, aby zmienić jej położenie.

Interakcje w panelu wykresu:

  • kółko myszy służy do przybliżania/oddalania

  • kliknięcie prawym przyciskiem myszy otwiera menu kontekstowe w celu dostosowania widoku

  • zaznaczenie prostokątnego wyboru pozwala powiększyć wybrany obszar

  • przeciągnięcie kursora zmienia jego położenie

Konsola wyjściowa

Konsola wyjścia wyświetla komunikaty z symulatora. Zaleca się sprawdzanie konsoli, aby mieć pewność że nie ma błędów ani ostrzeżeń.

Lista sygnałów

Pokazuje listę sygnałów pokazywanych w aktywnym wykresie.

Interakcje na liście sygnałów:

  • kliknięcie prawym przyciskiem myszy otwiera menu kontekstowe w celu ukrycia sygnału lub przełączenia krusora

  • podwójne kliknięcie ukrywa sygnał

Lista kursorów

Wyświetla listę kursorów i ich współrzędne. Każdy sygnał może mieć wyświetlany jeden kursor. Widoczność kursorów ustawiana jest za pomocą listy sygnałów.

Panel dostrajania

Wyświetla komponenty pobrane za pomocą narzędzia Dostrajanie. Panel dostrajania pozwala użytkownikowi szybko modyfikować wartości komponentów i obserwować ich wpływ na wyniki symulacji - za każdym razem, gdy wartość składnika jest zmieniana, symulacja jest ponownie uruchamiana, a wykresy są aktualizowane.

Z każdym komponentem jest powiązane kilka kontrolek:

  • Górne pole tekstowe określa maksymalną wartość komponentu.

  • Środkowe pole tekstowe określa aktualną wartość komponentu.

  • Dolne pole tekstowe określa minimalną wartość komponentu.

  • Suwak pozwala użytkownikowi modyfikować wartość komponentu w sposób płynny.

  • Przycisk Zapisz modyfikuje wartość komponentu na schemacie do tej wybranej za pomocą suwaka.

  • Przycisk X usuwa komponent z panelu Dostrajanie i przywraca jego oryginalną wartość.

Trzy pola tekstowe rozpoznają przedrostki jednostek używanych przez Spice.

Narzędzie Dostrajanie

Narzędzie dostrajania pozwala użytkownikowi na wybór komponentu, którego wartość chce dostroić.

Aby wybrać komponent by go dostroić, należy kliknąć go w edytorze schematów gdy narzędzie Dostrajanie jest aktywne. Wybrane komponenty pojawią się w panelu Dostrajanie. Tylko pasywne komponenty mogą być dostrajane.

Narzędzie Sonda

Narzędzie Sonda zapewnia przyjazny dla użytkownika sposób wyboru sygnałów w celu umieszczenia ich na wykresie.

Aby dodać sygnał do wykresu, kliknij odpowiednie połączenie w edytorze schematów gdy narzędzie jest aktywne.

Ustawienia symulacji

Okno dialogowe ustawień symulatora

Okno ustawień symulacji pozwala użytkownikowi ustawić typ symulacji i jej parametry. Dostępne są cztery zakładki:

  • AC

  • Przenoszenie DC

  • Analiza czasowa

  • Własne

Pierwsze trzy zakładki zawierają formularze w których można określić parametry symulacji. Ostatnia zakładka umożliwia użytkownikowi wpisanie również niestandardowych dyrektyw Spice. Więcej informacji o typach i parametrach symulacji można znaleźć w dokumentacji ngspice, rozdział 1.2.

Alternatywnym sposobem konfigurowania symulacji jest wpisanie dyrektyw Spice w pola tekstowe na schemacie. Wszystkie dyrektywy pochodzące z pól tekstowych związane z typem symulacji są zastępowane przez ustawienia wybrane w oknie dialogowym. Oznacza to, że gdy rozpoczniemy korzystać z okna dialogowego symulacji, wartości te zastąpią dyrektywy na schemacie do czasu, aż symulator nie zostanie ponownie otwarty.

Istnieją dwie opcje wspólne dla wszystkich typów symulacji:

Dostosuj wartości symboli pasywnych

Zastąp wartości symboli pasywnych by dokonać często wykonywanej konwersji wartości do ich notacji w Spice.

Dodaj pełną ścieżkę do dyrektyw .include wprowadzające nowe biblioteki

Łączy nazwy plików bibliotek modeli Spice z pełną ścieżką dostępu. Normalnie, pełna ścieżka jest wymagana przez ngspice by mógł uzyskać dostęp do pliku biblioteki.

Advanced Topics

Configuration and Customization

TODO: write this section

Text variables

TODO: write this section

Custom Netlist and BOM Formats

KiCad can output netlists and BOMs in various formats, and users can define new formats if desired.

The process of exporting a netlist is described in the netlist export section. BOM output is described in the BOM export section.

The following section describes how to create an exporter for a new output format.

Adding new netlist generators

New netlist generators are added to the Export Netlist dialog by clicking the Add Generator…​ button.

Custom Netlist Generator

New generators require a name and a command. The name is shown in the tab label, and the command is run whenever the Export Netlist button is clicked.

When the netlist is generated, KiCad creates an intermediate XML file which contains all of the netlist information from the schematic. The generator command is then run in order to transform the intermediate netlist into the desired netlist format.

The netlist command must be set up properly so that the netlist generator script takes the intermediate netlist file as input and outputs the desired netlist file. The exact netlist command will depend on the generator script used. The command format is described below.

Python and XSLT are commonly used tools to create custom netlist generators.

Adding a new BOM generator

KiCad also uses the intermediate netlist file to generate BOMs with the Generate BOM tool.

Główne okno narzędzia BOM

Additional scripts can be added to the list of BOM generator scripts by clicking the Plus icon button. Scripts can be removed by clicking the Delete icon button. The Edit icon button opens the selected script in a text editor.

Generator scripts written in Python and XSLT can contain a header comment that describes the generator’s functionality and usage. This header comment is displayed in the BOM dialog as the description for each generator. The header comment must contain the string @package. Everything following that string until the end of the comment is used as the description for the generator.

KiCad automatically fills the command line field when a new generator script is added, but the command line might need to be adjusted by hand depending on the generator script. KiCad attempts to automatically determine the output file extension from the example command line in the generator script’s header.

Generator command line format

The command line for a netlist or BOM exporter defines the command that KiCad will run to generate the selected output file.

For a netlist exporter using xsltproc, an example is:

xsltproc -o %O.net /usr/share/kicad/plugins/netlist_form_pads-pcb.asc.xsl %I

For a BOM exporter using Python, an example is:

/usr/bin/python3 /usr/share/kicad/plugins/bom_csv_grouped_by_value.py "%I" "%O.csv"

It is recommended to surround arguments in the command line with quotes (") in case they contain spaces or other special characters.

Some character sequences like %I and %O have a special meaning in the command line, because KiCad replaces them with a filename or path before executing the command.

Parameter Replaced with…​ Description


<project path>/<project name>.xml

Absolute path and filename of the intermediate netlist file, which is the input to the BOM or netlist generator plugin


<project path>/<project name>

Absolute path and filename of the output BOM or netlist file (without file extension). An appropriate file extension may need to be specified after the %O sequence.


<project name>

Base filename of the output BOM or netlist file (without path or file extension). An appropriate file extension may need to be specified after the %B sequence.


<project path>

Absolute path of the project directory, without trailing slash.

Plik pośredniej listy sieci

When exporting BOM files and netlists, KiCad creates an intermediate netlist file and then runs a separate tool which post-processes the intermediate netlist into the desired netlist or BOM format.

The intermediate netlist uses XML syntax. It contains a large amount of data about the design. Depending on the output (BOM or netlist), different subsets of the complete intermediate netlist file will be included in the final output file.

The structure of the intermediate netlist file is described in detail below.

Because the conversion from intermediate netlist file to output netlist or BOM is a text-to-text transformation, the post-processing filter can be written using Python, XSLT, or any other tool capable of taking XML as input.

XSLT is not recommended for new netlist or BOM exporters; Python or another tool should be used instead. Beginning with KiCad 7, xsltproc is no longer installed with KiCad, although it can be installed separately. Nevertheless, several examples of netlist exporters using XSLT are included below.

Plik pośredni listy sieci

Poniższy przykład ukazuje ideę samego pliku pośredniego.

<?xml version="1.0" encoding="utf-8"?>
<export version="D">
    <date>29/08/2010 21:07:51</date>
    <tool>eeschema (2010-08-28 BZR 2458)-unstable</tool>
    <comp ref="P1">
      <libsource lib="conn" part="CONN_4"/>
      <sheetpath names="/" tstamps="/"/>
    <comp ref="U2">
      <libsource lib="74xx" part="74LS74"/>
      <sheetpath names="/" tstamps="/"/>
    <comp ref="U1">
      <libsource lib="74xx" part="74LS04"/>
      <sheetpath names="/" tstamps="/"/>
    <comp ref="C1">
      <libsource lib="device" part="CP"/>
      <sheetpath names="/" tstamps="/"/>
    <comp ref="R1">
      <libsource lib="device" part="R"/>
      <sheetpath names="/" tstamps="/"/>
    <net code="1" name="GND">
      <node ref="U1" pin="7"/>
      <node ref="C1" pin="2"/>
      <node ref="U2" pin="7"/>
      <node ref="P1" pin="4"/>
    <net code="2" name="VCC">
      <node ref="R1" pin="1"/>
      <node ref="U1" pin="14"/>
      <node ref="U2" pin="4"/>
      <node ref="U2" pin="1"/>
      <node ref="U2" pin="14"/>
      <node ref="P1" pin="1"/>
    <net code="3" name="">
      <node ref="U2" pin="6"/>
    <net code="4" name="">
      <node ref="U1" pin="2"/>
      <node ref="U2" pin="3"/>
    <net code="5" name="/SIG_OUT">
      <node ref="P1" pin="2"/>
      <node ref="U2" pin="5"/>
      <node ref="U2" pin="2"/>
    <net code="6" name="/CLOCK_IN">
      <node ref="R1" pin="2"/>
      <node ref="C1" pin="1"/>
      <node ref="U1" pin="1"/>
      <node ref="P1" pin="3"/>
Struktura ogólna

Plik pośredni listy sieci posiada 5 sekcji:

  • Sekcja nagłówka.

  • Sekcja komponentów.

  • Sekcja elementów bibliotecznych.

  • Sekcja bibliotek.

  • Sekcja sieci połączeń.

The file content has the delimiter <export>

<export version="D">
Sekcja nagłówka

The header has the delimiter <design>

<date>21/08/2010 08:12:08</date>
<tool>eeschema (2010-08-09 BZR 2439)-unstable</tool>

Sekcja ta może być widoczna jako komentarze.

Sekcja komponentów

The component section has the delimiter <components>

<comp ref="P1">
<libsource lib="conn" part="CONN_4"/>
<sheetpath names="/" tstamps="/"/>

Jest to lista na której znajdują się poszczególne komponenty schematu. Każdy komponent jest opisany w następujący sposób:

<comp ref="P1">
<libsource lib="conn" part="CONN_4"/>
<sheetpath names="/" tstamps="/"/>
Element name Element description


name of the lib where this component was found.


component name inside this library.


path of the sheet inside the hierarchy: identify the sheet within the full schematic hierarchy.


timestamp of the component.

Note about time stamps for components

To identify a component in a netlist and therefore on a board, the timestamp reference is used as unique for each component. However KiCad provides an auxiliary way to identify a component which is the corresponding footprint on the board. This allows the re-annotation of components in a schematic project and does not lose the link between the component and its footprint.

Znacznik czasowy jest unikalnym identyfikatorem dla każdego składnika lub arkusza schematu w projekcie. Jednak w złożonych hierarchiach, w tym samym arkuszu składnik może być używany więcej niż raz, a zatem arkusz ten zawiera elementy o tym samym znaczniku czasowym.

A given sheet inside a complex hierarchy has an unique identifier: its sheetpath. A given component (inside a complex hierarchy) has a unique identifier: the sheetpath and its timestamp.

Sekcja elementów bibliotecznych

The libparts section has the delimiter <libparts>, and the content of this section is defined in the schematic libraries.

<libpart lib="device" part="CP">
  <description>Condensateur polarise</description>
    <field name="Reference">C</field>
    <field name="Valeur">CP</field>
    <pin num="1" name="1" type="passive"/>
    <pin num="2" name="2" type="passive"/>
Element name Element description


The symbol’s footprint filters. Each footprint filter is in a separate <fp> tag.


The symbol’s fields. Each field’s name and value is given in a separate `<field name="fieldname">…​</field> tag.


The symbol’s pins. Each pin is given in a separate <pin num="pinnum" type="pintype"/> tag. Possible pintypes are described below.

Possible electrical pin types are:

Pintype Description


Usual input pin


Usual output


Input or Output


Bus input/output


Usual ends of passive components


Unknown electrical type

Power input

Power input of a component

Power output

Power output like a regulator output

Open collector

Open collector often found in analog comparators

Open emitter

Open emitter sometimes found in logic

Not connected

Must be left open in schematic

Sekcja bibliotek

The libraries section has the delimiter <libraries>. This section contains the list of schematic libraries used in the project.

  <library logical="device">
  <library logical="conn">
Sekcja sieci

The nets section has the delimiter <nets>. This section describes the connectivity of the schematic by listing all nets and the pins connected to each net.

  <net code="1" name="GND">
    <node ref="U1" pin="7"/>
    <node ref="C1" pin="2"/>
    <node ref="U2" pin="7"/>
    <node ref="P1" pin="4"/>
  <net code="2" name="VCC">
    <node ref="R1" pin="1"/>
    <node ref="U1" pin="14"/>
    <node ref="U2" pin="4"/>
    <node ref="U2" pin="1"/>
    <node ref="U2" pin="14"/>
    <node ref="P1" pin="1"/>

Poszczególne sieci są pogrupowane wewnątrz tagu <net>:

<net code="1" name="GND">
  <node ref="U1" pin="7"/>
  <node ref="C1" pin="2"/>
  <node ref="U2" pin="7"/>
  <node ref="P1" pin="4"/>
Element name Element Description

net code

an internal identifier for this net


the net name


the pin (identified by pin) of a symbol (identified by ref) which is connected to the net

Example netlist exporters

Some example netlist exporters using XSLT are included below.

XSLT itself is an XML language very suitable for XML transformations. The xsltproc program can be used to read the Intermediate XML netlist input file, apply a style-sheet to transform the input, and save the results in an output file. Use of xsltproc requires a style-sheet file using XSLT conventions. The full conversion process is handled by KiCad, after it is configured once to run xsltproc in a specific way.

The document that describes XSL Transformations (XSLT) is available here: http://www.w3.org/TR/xslt

When writing a new netlist exporter, consider using Python or another tool rather than XSLT.
PADS netlist example using XSLT

The following example shows how to create an exporter for the PADS netlist format using xlstproc.

The PADS netlist format is comprised of two sections:

  • A list of footprints

  • A list of nets, together with the pads connected to each net.

Below is an XSL style-sheet which converts the intermediate netlist file to the PADS netlist format.

<?xml version="1.0" encoding="ISO-8859-1"?>
<!--XSL style sheet to Eeschema Generic Netlist Format to PADS netlist format
    Copyright (C) 2010, SoftPLC Corporation.
    GPL v2.

    How to use:

<!DOCTYPE xsl:stylesheet [
  <!ENTITY nl  "&#xd;&#xa;"> <!--new line CR, LF -->

<xsl:stylesheet version="1.0" xmlns:xsl="http://www.w3.org/1999/XSL/Transform">
<xsl:output method="text" omit-xml-declaration="yes" indent="no"/>

<xsl:template match="/export">
    <xsl:apply-templates select="components/comp"/>
    <xsl:apply-templates select="nets/net"/>

<!-- for each component -->
<xsl:template match="comp">
    <xsl:text> </xsl:text>
    <xsl:value-of select="@ref"/>
    <xsl:text> </xsl:text>
        <xsl:when test = "footprint != '' ">
            <xsl:apply-templates select="footprint"/>

<!-- for each net -->
<xsl:template match="net">
    <!-- nets are output only if there is more than one pin in net -->
    <xsl:if test="count(node)>1">
        <xsl:text>*SIGNAL* </xsl:text>
            <xsl:when test = "@name != '' ">
                <xsl:value-of select="@name"/>
                <xsl:value-of select="@code"/>
        <xsl:apply-templates select="node"/>

<!-- for each node -->
<xsl:template match="node">
    <xsl:text> </xsl:text>
    <xsl:value-of select="@ref"/>
    <xsl:value-of select="@pin"/>


And here is the PADS netlist output file after running xsltproc:

P1 unknown
U2 unknown
U1 unknown
C1 unknown
R1 unknown


Polecenie które dokonało takiej konwersji wygląda następująco:

kicad\\bin\\xsltproc.exe -o test.net kicad\\bin\\plugins\\netlist_form_pads-pcb.xsl test.tmp

Cadstar netlist example using XSLT

The following example shows how to create an exporter for the Cadstar netlist format using xlstproc.

The Cadstar format is comprised of two sections:

  • The footprint list

  • The Nets list: grouping pads references by nets

Below is an XSL style-sheet which converts the intermediate netlist file to the Cadstar netlist format.

<?xml version="1.0" encoding="ISO-8859-1"?>
<!--XSL style sheet to Eeschema Generic Netlist Format to CADSTAR netlist format
    Copyright (C) 2010, Jean-Pierre Charras.
    Copyright (C) 2010, SoftPLC Corporation.
    GPL v2. -->

<!DOCTYPE xsl:stylesheet [
  <!ENTITY nl  "&#xd;&#xa;"> <!--new line CR, LF -->

<xsl:stylesheet version="1.0" xmlns:xsl="http://www.w3.org/1999/XSL/Transform">
<xsl:output method="text" omit-xml-declaration="yes" indent="no"/>

<!-- Netlist header -->
<xsl:template match="/export">
    <xsl:apply-templates select="design/date"/>  <!-- Generate line .TIM <time> -->
    <xsl:apply-templates select="design/tool"/>  <!-- Generate line .APP <eeschema version> -->
    <xsl:apply-templates select="components/comp"/>  <!-- Generate list of components -->
    <xsl:apply-templates select="nets/net"/>          <!-- Generate list of nets and connections -->

 <!-- Generate line .TIM 20/08/2010 10:45:33 -->
<xsl:template match="tool">
    <xsl:text>.APP "</xsl:text>

 <!-- Generate line .APP "eeschema (2010-08-17 BZR 2450)-unstable" -->
<xsl:template match="date">
    <xsl:text>.TIM </xsl:text>

<!-- for each component -->
<xsl:template match="comp">
    <xsl:text>.ADD_COM </xsl:text>
    <xsl:value-of select="@ref"/>
    <xsl:text> </xsl:text>
        <xsl:when test = "value != '' ">
            <xsl:text>"</xsl:text> <xsl:apply-templates select="value"/> <xsl:text>"</xsl:text>

<!-- for each net -->
<xsl:template match="net">
    <!-- nets are output only if there is more than one pin in net -->
    <xsl:if test="count(node)>1">
    <xsl:variable name="netname">
            <xsl:when test = "@name != '' ">
                <xsl:value-of select="@name"/>
                <xsl:value-of select="@code"/>
        <xsl:apply-templates select="node" mode="first"/>
        <xsl:value-of select="$netname"/>
        <xsl:apply-templates select="node" mode="others"/>

<!-- for each node -->
<xsl:template match="node" mode="first">
    <xsl:if test="position()=1">
       <xsl:text>.ADD_TER </xsl:text>
    <xsl:value-of select="@ref"/>
    <xsl:value-of select="@pin"/>
    <xsl:text> </xsl:text>

<xsl:template match="node" mode="others">
        <xsl:when test='position()=1'>
        <xsl:when test='position()=2'>
           <xsl:text>.TER     </xsl:text>
           <xsl:text>         </xsl:text>
    <xsl:if test="position()>1">
        <xsl:value-of select="@ref"/>
        <xsl:value-of select="@pin"/>


Poniżej znajduje się plik wyjściowy dla programu Cadstar.

.TIM 21/08/2010 08:12:08
.APP "eeschema (2010-08-09 BZR 2439)-unstable"
.ADD_COM U2 "74LS74"
.ADD_COM U1 "74LS04"

.TER     C1.2
.TER     U1.14
.ADD_TER U1.2 "N-4"
.TER     U2.3
.TER     U2.5
.TER     C1.1

OrcadPCB2 netlist example using XSLT

This format has only one section which is the footprint list. Each footprint includes a list of its pads with reference to a net.

Below is an XSL style-sheet which converts the intermediate netlist file to the Orcad netlist format.

<?xml version="1.0" encoding="ISO-8859-1"?>
<!--XSL style sheet to Eeschema Generic Netlist Format to CADSTAR netlist format
    Copyright (C) 2010, SoftPLC Corporation.
    GPL v2.

    How to use:

<!DOCTYPE xsl:stylesheet [
  <!ENTITY nl  "&#xd;&#xa;"> <!--new line CR, LF -->

<xsl:stylesheet version="1.0" xmlns:xsl="http://www.w3.org/1999/XSL/Transform">
<xsl:output method="text" omit-xml-declaration="yes" indent="no"/>

    Netlist header
    Creates the entire netlist
    (can be seen as equivalent to main function in C
<xsl:template match="/export">
    <xsl:text>( { Eeschema Netlist Version 1.1  </xsl:text>
    <!-- Generate line .TIM <time> -->
<xsl:apply-templates select="design/date"/>
<!-- Generate line eeschema version ... -->
<xsl:apply-templates select="design/tool"/>

<!-- Generate the list of components -->
<xsl:apply-templates select="components/comp"/>  <!-- Generate list of components -->

<!-- end of file -->

    Generate id in header like "eeschema (2010-08-17 BZR 2450)-unstable"
<xsl:template match="tool">

    Generate date in header like "20/08/2010 10:45:33"
<xsl:template match="date">

    This template read each component
    (path = /export/components/comp)
    creates lines:
     ( 3EBF7DBD $noname U1 74LS125
      ... pin list ...
    and calls "create_pin_list" template to build the pin list
<xsl:template match="comp">
    <xsl:text> ( </xsl:text>
        <xsl:when test = "tstamp != '' ">
            <xsl:apply-templates select="tstamp"/>
    <xsl:text> </xsl:text>
        <xsl:when test = "footprint != '' ">
            <xsl:apply-templates select="footprint"/>
    <xsl:text> </xsl:text>
    <xsl:value-of select="@ref"/>
    <xsl:text> </xsl:text>
        <xsl:when test = "value != '' ">
            <xsl:apply-templates select="value"/>
    <xsl:call-template name="Search_pin_list" >
        <xsl:with-param name="cmplib_id" select="libsource/@part"/>
        <xsl:with-param name="cmp_ref" select="@ref"/>
    <xsl:text> )&nl;</xsl:text>

    This template search for a given lib component description in list
    lib component descriptions are in /export/libparts,
    and each description start at ./libpart
    We search here for the list of pins of the given component
    This template has 2 parameters:
        "cmplib_id" (reference in libparts)
        "cmp_ref"   (schematic reference of the given component)
<xsl:template name="Search_pin_list" >
    <xsl:param name="cmplib_id" select="0" />
    <xsl:param name="cmp_ref" select="0" />
        <xsl:for-each select="/export/libparts/libpart">
            <xsl:if test = "@part = $cmplib_id ">
                <xsl:apply-templates name="build_pin_list" select="pins/pin">
                    <xsl:with-param name="cmp_ref" select="$cmp_ref"/>

    This template writes the pin list of a component
    from the pin list of the library description
    The pin list from library description is something like
            <pin num="1" type="passive"/>
            <pin num="2" type="passive"/>
    Output pin list is ( <pin num> <net name> )
    something like
            ( 1 VCC )
            ( 2 GND )
<xsl:template name="build_pin_list" match="pin">
    <xsl:param name="cmp_ref" select="0" />

    <!-- write pin numner and separator -->
    <xsl:text>  ( </xsl:text>
    <xsl:value-of select="@num"/>
    <xsl:text> </xsl:text>

    <!-- search net name in nets section and write it: -->
    <xsl:variable name="pinNum" select="@num" />
    <xsl:for-each select="/export/nets/net">
        <!-- net name is output only if there is more than one pin in net
             else use "?" as net name, so count items in this net
        <xsl:variable name="pinCnt" select="count(node)" />
        <xsl:apply-templates name="Search_pin_netname" select="node">
            <xsl:with-param name="cmp_ref" select="$cmp_ref"/>
            <xsl:with-param name="pin_cnt_in_net" select="$pinCnt"/>
            <xsl:with-param name="pin_num"> <xsl:value-of select="$pinNum"/>

    <!-- close line -->
    <xsl:text> )&nl;</xsl:text>

    This template writes the pin netname of a given pin of a given component
    from the nets list
    The nets list description is something like
        <net code="1" name="GND">
          <node ref="J1" pin="20"/>
              <node ref="C2" pin="2"/>
        <net code="2" name="">
          <node ref="U2" pin="11"/>
    This template has 2 parameters:
        "cmp_ref"   (schematic reference of the given component)
        "pin_num"   (pin number)

<xsl:template name="Search_pin_netname" match="node">
    <xsl:param name="cmp_ref" select="0" />
    <xsl:param name="pin_num" select="0" />
    <xsl:param name="pin_cnt_in_net" select="0" />

    <xsl:if test = "@ref = $cmp_ref ">
        <xsl:if test = "@pin = $pin_num">
        <!-- net name is output only if there is more than one pin in net
             else use "?" as net name
            <xsl:if test = "$pin_cnt_in_net>1">
                    <!-- if a net has a name, use it,
                        else build a name from its net code
                    <xsl:when test = "../@name != '' ">
                        <xsl:value-of select="../@name"/>
                        <xsl:text>$N-0</xsl:text><xsl:value-of select="../@code"/>
            <xsl:if test = "$pin_cnt_in_net &lt;2">



Poniżej znajduje się plik wyjściowy programu OrcadPCB2.

( { Eeschema Netlist Version 1.1  29/08/2010 21:07:51
eeschema (2010-08-28 BZR 2458)-unstable}
 ( 4C6E2141 $noname P1 CONN_4
  (  1 VCC )
  (  2 /SIG_OUT )
  (  3 /CLOCK_IN )
  (  4 GND )
 ( 4C6E20BA $noname U2 74LS74
  (  1 VCC )
  (  2 /SIG_OUT )
  (  3 N-04 )
  (  4 VCC )
  (  5 /SIG_OUT )
  (  6 ? )
  (  7 GND )
  (  14 VCC )
 ( 4C6E20A6 $noname U1 74LS04
  (  1 /CLOCK_IN )
  (  2 N-04 )
  (  7 GND )
  (  14 VCC )
 ( 4C6E2094 $noname C1 CP
  (  1 /CLOCK_IN )
  (  2 GND )
 ( 4C6E208A $noname R1 R
  (  1 VCC )
  (  2 /CLOCK_IN )

Actions reference

Below is a list of every available action in the KiCad Schematic Editor: a command that can be assigned to a hotkey.

Schematic Editor

The actions below are available in the Schematic Editor. Hotkeys can be assigned to any of these actions in the Hotkeys section of the preferences.

Action Default Hotkey Description

Align Elements to Grid

Annotate Schematic…​

Fill in schematic symbol reference designators

Assign Footprints…​

Run footprint assignment tool

Clear Net Highlighting


Clear any existing net highlighting

Export Drawing to Clipboard

Export drawing of current sheet to clipboard

Edit Library Symbol…​


Open the library symbol in the Symbol Editor

Edit Sheet Page Number…​

Edit the page number of the current or selected sheet

Edit Symbol Fields…​

Bulk-edit fields of all symbols in schematic

Edit Symbol Library Links…​

Edit links between schematic and library symbols

Edit with Symbol Editor


Open the selected symbol in the Symbol Editor

Highlight on PCB

Highlight corresponding items in PCB editor

Export Netlist…​

Export file containing netlist in one of several formats

Force H/V Wires and Buses

Switch H & V only mode for new wires and buses

Generate BOM…​

Generate a bill of materials for the current schematic

Highlight Net


Highlight net under cursor

Highlight Nets

Highlight wires and pins of a net

Import Footprint Assignments…​

Import symbol footprint assignments from .cmp file created by Pcbnew

Remap Legacy Library Symbols…​

Remap library symbol references in legacy schematics to the symbol library table

Repair Schematic

Run various diagnostics and attempt to repair schematic

Rescue Symbols…​

Find old symbols in project and rename/rescue them


Simulate circuit in SPICE

Save Current Sheet Copy As…​

Save a copy of the current sheet to another location or name

Schematic Setup…​

Edit schematic setup including annotation styles and electrical rules

Bus Definitions…​

Manage bus definitions

Show Hidden Fields

Toggle display of hidden text fields

Show Hidden Pins

Toggle display of hidden pins

Switch to PCB Editor

Open PCB in board editor

Scripting Console

Show the Python scripting console

Symbol Checker

Show the symbol checker window

Electrical Rules Checker

Perform electrical rules check

Show Datasheet


Opens the datasheet in a browser

Add Sheet


Add a hierarchical sheet

Finish Sheet

Finish drawing sheet

Import Sheet Pin

Import a hierarchical sheet pin

Import Sheet Pin

Import a hierarchical sheet pin

Add Wire to Bus Entry


Add a wire entry to a bus

Add Global Label


Add a global label

Add Hierarchical Label


Add a hierarchical label

Add Image

Add bitmap image

Add Junction


Add a junction

Add Label


Add a net label

Add No Connect Flag


Add a no-connection flag

Add Power


Add a power port

Add Text


Add text

Add Symbol


Add a symbol

Add Junctions to Selection where needed

Add Bus


Add a bus

Add Lines


Add connected graphic lines

Add Wire


Add a wire

Finish Wire or Bus


Complete drawing at current segment

Finish Bus

Complete bus with current segment

Finish Lines

Complete connected lines with current segment

Finish Wire

Complete wire with current segment

Unfold from Bus


Break a wire out of a bus

Assign Netclass…​

Assign a netclass to the net of the selected wire

Autoplace Fields


Runs the automatic placement algorithm on the symbol or sheet’s fields

Break Bus

Divide a bus into segments which can be dragged independently

Break Wire

Divide a wire into segments which can be dragged independently

Change Symbol…​

Assign a different symbol from the library

Change Symbols…​

Assign different symbols from the library

Cleanup Sheet Pins

Delete unreferenced sheet pins

Edit Footprint…


Displays footprint field dialog

Edit Reference Designator…​


Displays reference designator dialog

Edit Text & Graphics Properties…​

Edit text and graphics properties globally across schematic

Edit Value…


Displays value field dialog

Mirror Horizontally


Flips selected item(s) from left to right

Mirror Vertically


Flips selected item(s) from top to bottom

Pin Table…​

Displays pin table for bulk editing of pins



Displays item properties dialog

Repeat Last Item


Duplicates the last drawn item

Rotate Counterclockwise


Rotates selected item(s) counter-clockwise

Rotate Clockwise

Rotates selected item(s) clockwise

De Morgan Alternate

Switch to alternate De Morgan representation

De Morgan Standard

Switch to standard De Morgan representation

Symbol Properties…​

Displays symbol properties dialog

Change to Global Label

Change existing item to a global label

Change to Hierarchical Label

Change existing item to a hierarchical label

Change to Label

Change existing item to a label

Change to Text

Change existing item to a text comment

De Morgan Conversion

Switch between De Morgan representations

Update Symbol…​

Update symbol to include any changes from the library

Update Symbols from Library…​

Update symbols to include any changes from the library

Move Activate



Drags the selected item(s)



Moves the selected item(s)

Select Connection


Select a complete connection

Select Node


Select a connection item under the cursor

Enter Sheet

Display the selected sheet’s contents in the schematic editor

Navigate to page

Navigate to page

Leave Sheet


Display the parent sheet in the schematic editor

Hierarchy Navigator

Show schematic sheet hierarchy

Push Pin Length

Copy pin length to other pins in symbol

Push Pin Name Size

Copy pin name size to other pins in symbol

Push Pin Number Size

Copy pin number size to other pins in symbol

Create Corner

Create a corner

Remove Corner

Remove corner

Add a simulator probe

Select a value to be tuned

Add Arc

Add an arc

Add Circle

Add a circle

Add Lines

Add connected graphic lines

Add Rectangle

Add a rectangle

Finish Drawing

Finish drawing shape

Move Symbol Anchor

Specify a new location for the symbol anchor

Add Pin


Add a pin

Add Text

Add a text item

Add Symbol to Schematic

Add Symbol to Schematic



Delete Symbol

Remove the selected symbol from its library

Duplicate Symbol

Make a copy of the selected symbol

Edit Symbol

Show selected symbol on editor canvas


Export a symbol to a new library file

Export Symbol as SVG…

Create SVG file from the current symbol

Export View as PNG…

Create PNG file from the current view

Hide Symbol Tree

Import Symbol…​

Import a symbol to the current library

New Symbol…​


Create a new symbol

Paste Symbol

Save Library As…​


Save the current library to a new file.

Save As…

Save the current symbol to a different library.

Show Pin Electrical Types

Annotate pins with their electrical types

Show Symbol Tree

Synchronized Pins Edit Mode

Synchronized Pins Edit Mode When enabled propagates all changes (except pin numbers) to other units. Enabled by default for multiunit parts with interchangeable units.

Update Symbol Fields…​

Update symbol to match changes made in parent symbol

Symbol Move Activate


The actions below are available across KiCad, including in the Schematic Editor. Hotkeys can be assigned to any of these actions in the Hotkeys section of the preferences.

Action Default Hotkey Description

Exclude Marker

Mark current violation in Checker window as an exclusion

Next Marker

Go to next marker in Checker window

Previous Marker

Go to previous marker in Checker window

Add Library…

Add an existing library folder



Performs left mouse button click



Performs left mouse button double-click

Cursor Down


Cursor Down Fast


Cursor Left


Cursor Left Fast


Cursor Right


Cursor Right Fast


Cursor Up


Cursor Up Fast


Switch to Fast Grid 1


Switch to Fast Grid 2


Switch to Next Grid


Switch to Previous Grid


Grid Properties…​

Set grid dimensions

Reset Grid Origin


Grid Origin


Set the grid origin point

Inactive Layer View Mode

Toggle inactive layers between normal and dimmed

Inactive Layer View Mode (3-state)


Cycle inactive layers between normal, dimmed, and hidden


Use inches


Use millimeters


Use mils



Create a new document in the editor

New Library…

Create a new library folder



Open existing document

Page Settings…​

Settings for paper size and title block info

Pan Down


Pan Left


Pan Right


Pan Up


Pin Library

Keep the library at the top of the list







Close the current editor

Reset Local Coordinates



Throw away changes



Save changes

Save All

Save all changes

Save As…


Save current document to another location

Save Copy As…​

Save a copy of the current document to another location

3D Viewer


Show 3D viewer window

Show Context Menu

Perform the right-mouse-button action

Footprint Library Browser

Browse footprint libraries

Footprint Editor

Create, delete and edit footprints

Symbol Library Browser

Browse symbol libraries

Symbol Editor

Create, delete and edit symbols

Always Show Cursor


Display crosshairs even in selection tool

Full-Window Crosshairs

Switch display of full-window crosshairs

Show Grid

Display grid dots or lines in the edit window

Polar Coordinates

Switch between polar and cartesian coordinate systems

Switch units


Switch between imperial and metric units

Unpin Library

No longer keep the library at the top of the list

Update PCB from Schematic…


Update PCB with changes made to schematic

Update Schematic from PCB…​

Update schematic with changes made to PCB




Zoom to Objects


Zoom to Objects

Zoom to Fit


Zoom to Fit

Zoom In at Cursor


Zoom In at Cursor

Zoom In

Zoom In

Zoom Out at Cursor


Zoom Out at Cursor

Zoom Out

Zoom Out




Zoom to Selection


Zoom to Selection


Cancel current tool

Change Edit Method


Change edit method constraints



Copy selected item(s) to clipboard



Cut selected item(s) to clipboard



Deletes selected item(s)

Interactive Delete Tool

Delete clicked items



Duplicates the selected item(s)



Find text

Find and Replace


Find and replace text

Find Next


Find next match

Find Next Marker




Paste item(s) from clipboard

Paste Special…​

Paste item(s) from clipboard with options



Redo last edit

Replace All

Replace all matches

Replace and Find Next

Replace current match and find next

Select All


Select all items on screen



Undo last edit

Measure Tool


Interactively measure distance between points

Select item(s)

Select item(s)

Configure Paths…

Edit path configuration environment variables


Open "Donate to KiCad" in a web browser

Get Involved

Open "Contribute to KiCad" in a web browser

Getting Started with KiCad

Open “Getting Started in KiCad” guide for beginners


Open product documentation in a web browser

List Hotkeys…​


Displays current hotkeys table and corresponding commands



Show preferences for all open tools

Report Bug

Report a problem with KiCad

Manage Footprint Libraries…​

Edit the global and project footprint library lists

Manage Symbol Libraries…

Edit the global and project symbol library lists

Table of Contents