Manuel de référence

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 (, version 3 or later, or the Creative Commons Attribution License (, version 3.0 or later.

Toutes les marques apparaissant dans ce document appartiennent à leurs propriétaires respectifs.


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


Marc Berlioux <[email protected]>, 2015-2016


Merci de signaler vos corrections de bugs, suggestions ou nouvelles versions ici :

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:

  • La vérification des règles électriques ou ERC (Electrical Rules Check), pour le contrôle des connexions manquantes ou incorrectes.

  • L’exportation de fichiers de tracé en plusieurs formats (Postscript, PDF, HPGL, SVG)

  • Bill of Materials generation (via Python or XSLT scripts, which allow many flexible formats).

Aperçu technique

The Schematic Editor is limited only by the available memory. There is thus no real limitation to the number of components, component pins, connections or sheets. In the case of multi-sheet schematics, the representation is hierarchical.

The Schematic Editor can use multi-sheet schematics in a few ways:

  • Schémas à hiérarchie simple (chaque schéma n’est utilisé qu’une fois).

  • Schémas à hiérarchie complexe (certains schémas sont utilisés plus d’une fois, en plusieurs instances).

  • Schémas à hiérarchie plate (les schémas ne font pas explicitement partie d’un schéma maître).

Configuration Initiale

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.

Generic Schematic Editor commands

Commands can be executed by:

  • En cliquant sur les menus, en haut de la fenêtre.

  • En cliquant sur les boutons de la barre d’outil principale, au sommet de la fenêtre, sous les menus.

  • En cliquant sur les boutons de la barre d’outils à droite de la fenêtre (outils de placement d’éléments).

  • En cliquant sur les boutons de la barre d’outils à gauche de la fenêtre (options d’affichage).

  • En utilisant la souris (commandes complémentaires importantes), notamment au moyen du clic droit sur un élément du schéma, qui affiche un menu contextuel (options de zoom, de dimension de grille et d’édition des éléments).

  • Function keys (F1, F2, F3, F4, Insert and Space). Specifically: Escape cancels the command in progress. Insert allows the duplication of the last element created.

  • Pressing hotkeys. For a list of hotkeys, see the Help→List Hotkeys menu entry or press Ctrl+F1. Many hotkeys select a tool but do not perform the tool’s action until the canvas is clicked. This behavior can be changed by unchecking First hotkey selects tool in the Common Preferences pane. With this option unchecked, pressing a hotkey will select the tool and immediately perform the tool’s action at the current cursor location.

Commands overview

Commandes à la souris

Commandes de base

Bouton gauche

  • Single click: Selects the item under the cursor and displays the item’s characteristics in the status bar.

  • Double click: edits the item if it is editable.

  • Long click (click and hold): opens a pop-up menu to clarify the selection.

Bouton droit

  • Opens a pop-up menu. If an item is selected, the items in the menu are related to the selected item. If an item is under the cursor when the right mouse button is clicked, the item is selected.

Selection operations

Schematic editor items can be selected by clicking on them. Multiple items can be selected at once. Add items to the selection with Shift + click, and remove items from the selection with Ctrl+Shift + click.

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

left mouse button

Select item.

Shift + left mouse button

Add item to selection.

Ctrl+Shift + left mouse button

Remove item from selection.

long click

Clarify selection from a pop-up menu.

Ctrl + left mouse button

Highlight net.

Items can also be selected by drawing a box around them using the left mouse button.

Dragging from left to right includes all items fully enclosed by the box. Dragging from right to left includes all items touched by the box, even if they are not fully enclosed.

The Shift and Ctrl+Shift modifiers also work with drag selections to add and remove items from the selection, respectively.

Raccourcis clavier

  • The Ctrl+F1 displays the current hotkey list.

  • All hotkeys can be redefined using the hotkey editor (PreferencesPreferences…​Hotkeys).

The default hotkey list is below. Many additional actions do not have hotkeys by default, but hotkeys can be assigned to them with the hotkey editor.

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.

Action Default Hotkey Description



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


Reset Grid Origin


Grid Origin


Set the grid origin point



Create a new document in the editor



Open existing document

Pan Down


Pan Left


Pan Right


Pan Up





Reset Local Coordinates




Save changes

Save As…


Save current document to another location

Always Show Cursor


Display crosshairs even in selection tool

Switch units


Switch between imperial and metric units

Update PCB from Schematic…


Update PCB with changes made to schematic




Zoom to Objects


Zoom to Objects

Zoom to Fit


Zoom to Fit

Zoom In at Cursor


Zoom In at Cursor

Zoom Out at Cursor


Zoom Out at Cursor




Zoom to Selection


Zoom to Selection

Change Edit Method


Change edit method constraints



Copy selected item(s) to clipboard



Cut selected item(s) to clipboard



Deletes selected item(s)



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



Redo last edit

Select All


Select all items on screen



Undo last edit

List Hotkeys…​


Displays current hotkeys table and corresponding commands



Show preferences for all open tools

Clear Net Highlighting


Clear any existing net highlighting

Edit Library Symbol…​


Open the library symbol in the Symbol Editor

Edit with Symbol Editor


Open the selected symbol in the Symbol Editor

Highlight Net


Highlight net under cursor

Show Datasheet


Opens the datasheet in a browser

Add Sheet


Add a hierarchical sheet

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 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 Bus


Add a bus

Add Lines


Add connected graphic lines

Add Wire


Add a wire

Finish Wire or Bus


Complete drawing at current segment

Unfold from Bus


Break a wire out of a bus

Autoplace Fields


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

Edit Footprint…


Displays footprint field dialog

Edit Reference Designator…​


Displays reference designator dialog

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



Displays item properties dialog

Repeat Last Item


Duplicates the last drawn item

Rotate Counterclockwise


Rotates selected item(s) counter-clockwise



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

Leave Sheet


Display the parent sheet in the schematic editor

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

It is possible to import hotkey settings from a user.hotkeys file using menu PreferencesPreferences…​HotkeysImport Hotkeys…​.


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 preferred grid to place symbols and wires in a schematic, and to place 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 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.

One can also work with a smaller grid from 25 mil to 10 mil. This is only intended for designing the symbol body or placing text and comments 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.

Sélection du Zoom

Pour changer le niveau du zoom :

  • Cliquez du bouton droit pour ouvrir le menu contextuel et choisissez la valeur de zoom désirée.

  • Or use hotkeys:

    • F1: Zoom in

    • F2: Zoom out

    • F4: Center the view around the cursor pointer position

    • Home: Zoom and center the view to fit the entire schematic sheet

    • Ctrl+Home: Zoom and center the view to fit all of the objects in the schematic

    • Ctrl+F5: Activate the Zoom to Selection tool

  • Zoom fenêtre :

    • Mouse wheel: Zoom in/out

    • Shift+Mouse wheel: Pan up/down

    • Ctrl+Mouse wheel: Pan left/right

Mouse scroll gestures are configurable in the Mouse and Touchpad page of the Preferences dialog.

Affichage des coordonnées du curseur

The display units are in inches, mils, or millimeters.

Les informations suivantes sont affichées en bas et à droite de la fenêtre :

  • Le facteur de Zoom

  • La position absolue du curseur (X Y)

  • La position relative du curseur (dx dy)

  • The grid size

  • The active unit system

  • The active tool

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

Barre d’état

Barre de menu

The top menu bar allows the opening and saving of schematics, program configuration and viewing the documentation.


Barre d’outils supérieure

This toolbar gives access to the main functions of the Schematic Editor.

If the Schematic Editor is run in standalone mode, this is the available tool set:


Note that when KiCad runs in project mode, the first two icons are not available as they work with individual files.

New schematic icon

Create a new schematic (only in standalone mode).

Open schematic icon

Open a schematic (only in standalone mode).

Save schematic icon

Save complete schematic project.

Schematic Setup icon

Set the schematic-specific options.

Page Settings icon

Select the sheet size and edit the title block.

Print icon

Open print dialog.

Plot icon

Open plot dialog.

paste icon

Paste a copied/cut item or block to the current sheet.

undo icon

Undo: Revert the last change.

redo icon

Redo: Revert the last undo operation.

search icon

Show the dialog to search symbols and texts in the schematic.

search replace icon

Show the dialog to search and replace texts in the schematic.

refresh icon

Refresh screen.

zoom in icon

Zoom in.

zoom out icon

Zoom out.

zoom to fit icon

Zoom to fit the entire schematic sheet.

zoom fit to objects icon

Zoom to fit all objects in the schematic.

zoom fit to selection icon

Zoom to fit selected items.

hierarchy navigator icon

View and navigate the hierarchy tree.

leave sheet icon

Leave the current sheet and go up in the hierarchy.

rotate counter-clockwise icon

Rotate selected items counter-clockwise.

rotate clockwise icon

Rotate selected items clockwise.

mirror vertical icon

Mirror selected items vertically.

mirror horizontal icon

Mirror selected items horizontally.

symbol editor icon

Call the symbol library editor to view and modify libraries and symbols.

symbol library browser icon

Browse symbol libraries.

footprint editor icon

Open the footprint library editor to view and modify libraries and footprints.

annotate icon

Annotate symbols.

ERC icon

Electrical Rules Checker (ERC), automatically validate electrical connections.

run footprint assignment icon

Open the footprint assignment tool to assign footprints to symbols.

Symbol fields editor icon

Bulk edit symbol fields in a spreadsheet interface.

BOM icon

Generate the Bill of Materials (BOM).

pcb editor icon

Open the PCB editor.

python scripting console icon

Open the Python scripting console.

Barre d’outils latérale droite

Cette barre d’outils contient les outils pour :

  • Place symbols, wires, buses, junctions, labels, text, etc.

  • Create hierarchical subsheets and connection symbols.

Selection tool icon

Cancel the active command or tool and go into selection mode.

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.

New Symbol icon

Display the symbol selector dialog to select a new symbol to be placed.

Add Power icon

Display the power symbol selector dialog to select a power symbol to be placed.

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. It is done to notify the Electrical Rules Checker that lack of connection for a particular pin is intentional and should not be reported.

place junction icon

Place a junction. This connects two crossing wires or a wire and a pin, when it can be ambiguous (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 label connects items located in the same sheet. For connections between two different sheets, you have to 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 parent sheet that contains it.

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 a line. These are only graphical and 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.

Barre d’outils latérale gauche

Cette barre d’outils permet de gérer les options d’affichage :

grid visibility icon

Toggle grid visibility.

inch unit icon

Switch units to inches.

mil unit icon

Switch units to mils (0.001 inches).

millimeter unit icon

Switch units to millimeters.

cursor shape icon

Choose the cursor shape (full screen/small).

hidden pin icon

Toggle visibility of "invisible" pins.

free angle wire icon

Toggle free angle/90 degrees wires and buses placement.

Menus contextuels et édition rapide

Un clic droit ouvre un menu contextuel pour l’élément sélectionné ou survolé : ce menu permet d’ajuster :

  • Le facteur de Zoom.

  • La taille de grille.

  • Copy/Paste/Delete commands.

  • Add Wire/Bus.

  • Les paramètres couramment édités de l’élément sélectionné.

Barre de menus

Menu Fichiers

Menu Fichiers
New Close current schematic and start a new one (only in standalone mode).


Load a schematic project (only in standalone mode).

Open Recent

Open a schematic project from the list of recently opened files (only in standalone mode).


Save current sheet and all its subsheets.

Save As…​

Save the current sheet under a new name (only in standalone mode).

Save Current Sheet Copy As…​

Save a copy of the current sheet under a new name (only in project mode).

Insert Schematic Sheet Content…​

Insert the contents of another schematic sheet into the current sheet (only in standalone mode).


Import a non-KiCad schematic or a footprint assignment file.


Export a netlist or a drawing of the schematic to the clipboard.

Schematic Setup…​

Set up schematic formatting, electrical rules, net classes, and text variables.

Page Settings…​

Configure page dimensions and title block.


Print schematic project (See also chapter Plot and Print).


Export to PDF, PostScript, HPGL or SVG format (See chapter Plot and Print).


Terminate the application.

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.

Menu Préférences

Menu Préférences

Configure Paths…​

Set the default search paths.

Manage Symbol Library Tables…​

Add/remove symbol libraries.


Preferences (units, grid size, field names, etc.).

Set Language

Select interface language.

Manage Symbol Library Tables

Symbol Library Tables

This dialog is used to manage the tables of symbol libraries. Symbol library management is described later.


Common Preferences
TODO: write this section
Common settings
Mouse and Touchpad

Center and warp cursor on zoom

If checked, the pointed location is warped to the screen center when zooming in/out.

Use touchpad to pan

When enabled, view is panned using scroll wheels (or touchpad gestures) and to zoom one needs to hold Ctrl. Otherwise scroll wheels zoom in/out and Ctrl/Shift are the panning modifiers.

Pan while moving object

If checked, automatically pans the window if the cursor leaves the window during drawing or moving.

Raccourcis clavier

Redefine hotkeys.

Hotkeys settings

Select a new hotkey by double clicking an action or right click on an action to show a popup menu:


Define a new hotkey for the action (same as double click).

Undo Changes

Reverts the recent hotkey changes for the action.

Clear Assigned Hotkey

Restore Default

Sets the action hotkey to its default value.

Display Options
Display options

Grid Size

Grid size selection.

It is recommended to work with normal grid (0.050 inches or 1,27 mm). Smaller grids are used for component building.

Bus thickness

Pen size used to draw buses.

Line thickness

Pen size used to draw objects that do not have a specified pen size.

Part ID notation

Style of suffix that is used to denote symbol units (U1A, U1.A, U1-1, etc.)

Icon scale

Adjust toolbar icons size.

Show Grid

Grid visibility setting.

Restrict buses and wires to H and V orientation

If checked, buses and wires are drawn only with vertical or horizontal lines. Otherwise buses and wires can be placed at any orientation.

Show hidden pins:

Display invisible (or hidden) pins, typically power pins.

Show page limits

If checked, shows the page boundaries on screen.

Footprint previews in symbol chooser

Displays a footprint preview frame and footprint selector when placing a new symbol.

Note: it may cause problems or delays, use at your own risk.

Editing Options
Editing settings

Measurement units

Select the display and the cursor coordinate units (inches or millimeters).

Horizontal pitch of repeated items

Increment on X axis during element duplication (default: 0) (after placing an item like a symbol, label or wire, a duplication is made by the Insert key)

Vertical pitch of repeated items

Increment on Y axis during element duplication (default: 0.100 inches or 2,54 mm).

Increment of repeated labels

Increment of label value during duplication of texts ending in a number, such as bus members (usual value 1 or -1).

Default text size

Text size used when creating new text items or labels.

Auto-save time interval

Time in minutes between saving backups.

Automatically place symbol fields

If checked, symbol fields (e.g. value and reference) in newly placed symbols might be moved to avoid collisions with other items.

Allow field autoplace to change justification

Extension of 'Automatically place symbol fields' option. Enable text justification adjustment for symbol fields when placing a new part.

Always align autoplaced fields to the 50 mil grid

Extension of 'Automatically place symbol fields' option. If checked, fields are autoplaced using 50 mils grid, otherwise they are placed freely.


Color scheme for various graphic elements. Click on any of the color swatches to select a new color for a particular element.

Couleurs dans Eeschema
Default Fields

Define additional custom fields and corresponding values that will appear in newly placed symbols.

Default Fields settings

Menu Aide

Access to on-line help (this document) for an extensive tutorial about KiCad.

Use the Report a Bug item to report a bug online. Full KiCad version and user system information is available via the Copy Version Info button in the About KiCad window.

Barre d’outils principale

Gestion des feuilles schématiques

The Sheet Settings icon (Sheet Settings icon) allows you to define the sheet size and the contents of the title block.

Réglage de la page

Le nombre de feuilles, numéro de feuille, sont mis à jour automatiquement. La date ne sera pas changée automatiquement, mais vous pouvez la fixer à aujourd’hui en cliquant sur le bouton "←".

Outil de recherche

The Find icon (Find icon) can be used to access the search tool.


You can search for a reference, a value or a text string in the current sheet or in the whole hierarchy. Once found, the cursor will be positioned on the found element in the relevant sub-sheet.

Outil de Netliste

The Netlist icon (Netlist icon) opens the netlist generation tool.

The tool creates a file which describe all connections in the entire hierarchy.

In a multisheet hierarchy, any local label is visible only inside the sheet to which it belongs. For example: the label LABEL1 of sheet 3 is different from the label LABEL1 of sheet 5 (if no connection has been intentionally introduced to connect them). This is due to the fact that the sheet name path is internally associated with the local label.

Even though there is no text length limit for labels in KiCad, please take into account that other programs reading the generated netlist may have such constraints.
Avoid spaces in labels, because they will appear as separated words in the generated file. It is not a limitation of KiCad, but of many netlist formats, which often assume that a label has no spaces.
La fenêtre de l’outil de Netlistes

Options :

Default Format

Check to select Pcbnew as the default format.

D’autres formats de netlistes peuvent être générés :

  • Orcad PCB2

  • CadStar

  • Spice (simulators)

External plugins can be added to extend the netlist formats list (PadsPcb Plugin was added in the picture above).

There is more information about creating netlists in Create a Netlist chapter.

Outil d’annotation

The icon Annotate icon launches the annotation tool. This tool assigns references to components.

Pour des composants multi-unités (comme par exemple le 7400 qui contient 4 portes), un suffixe d’unité sera attribué (ainsi notre 7400 désigné par la référence U3 sera divisé en quatre unités référencées U3A, U3B, U3C et U3D).

You can unconditionally annotate all the components or only the new components, i.e. those which were not previously annotated.



Use the entire schematic All sheets are re-annotated (default).

Use the current page only

Only the current sheet is re-annotated (this option is to be used only in special cases, for example to evaluate the amount of resistors in the current sheet.).

Keep existing annotation

Conditional annotation, only the new components will be re-annotated (default).

Reset existing annotation

Unconditional annotation, all the components will be re-annotated (this option is to be used when there are duplicated references).

Reset, but do not swap any annotated multi-unit parts

Keeps all groups of multiple units (e.g. U2A, U2B) together when reannotating.

Ordre d’annotation

Selects the order in which components will be numbered (either horizontally or vertically).

Choix de l’annotation

Selects the assigned reference format.

Outil de vérification des règles électriques

The icon ERC icon launches the electrical rules check (ERC) tool.

This tool performs a design verification and is able to detect forgotten connections, and inconsistencies.

Once you have run the ERC, KiCad places markers to highlight problems. The error description is displayed after left clicking on the marker. An error report file can also be generated.

Fenêtre principale de l’ERC

La fenêtre de l’ERC.

Errors are displayed in the Electrical Rules Checker dialog:

  • Total : nombre total d’erreurs et avertissements.

  • Erreurs : nombre d’erreurs.

  • Warnings : nombre d’avertissements.

Options :

Create ERC file report

Check this option to generate an ERC report file.

Commandes :

Delete Markers

Remove all ERC error/warnings markers.


Start an Electrical Rules Check.


Close the dialog.

  • En cliquant sur une erreur, vous êtes emmenés au marqueur correspondant sur le schéma.

Options de l’ERC

Onglet 'Options'

This tab allows you to define the connectivity rules between pins; you can choose between 3 options for each case:

  • Pas d’erreur (Vert)

  • Avertissement (W jaune)

  • Erreur (E rouge)

Chaque carré de la matrice peut être modifié en cliquant une ou plusieurs fois dessus.

Options :

Test similar labels

Report labels that differ only by letter case (e.g. label/Label/LaBeL). Net names are case-sensitive therefore such labels are treated as separate nets.

Test unique global labels

Report global lables that occur only once for a particular net. Normally it is required to have at least two make a connection.

Commandes :

Initialize to Default

Restores the original settings.

Footprint Assignment Tool

The footprint assignment tool icon button launches the Footprint Assignment Tool, which can be used to associate PCB footprints with symbols in the schematic. The footprint assignment process is described later in the manual.

Outil de Liste de Matériel

The icon BOM icon launches the bill of materials (BOM) generator. This tool generates a file listing the components and/or hierarchical connections (global labels).

Fenêtre du générateur de BOM

The Schematic Editor’s BOM generator makes use of external plugins, either as XSLT or Python scripts. There are a few examples installed inside the KiCad program files directory.

Quelques champs de composants utiles à utiliser pour le BOM :

  • Valeur : nom unique pour chaque composant utilisé.

  • Empreinte : entrée soit manuellement, soit par rétro-annotation (voir ci-dessous).

  • Champ 1 : nom du fabricant.

  • Champ 2 : référence fabricant.

  • Champ 3 : référence distributeur.

Exemple :

Fenêtre des propriétés du composant

On MS Windows, BOM generator dialog has a special option (pointed by red arrow) that controls visibility of external plugin window. + By default, BOM generator command is executed console window hidden and output is redirected to Plugin info field. Set this option to show the window of the running command. It may be necessary if plugin has provides a graphical user interface.

BOM dialog extra option on MS Windows

Edit Fields tool

The icon Edit Fields icon opens a spreadsheet to view and modify field values for all symbols.

Symbol Dialog

Once you modify field values, you need to either accept changes by clicking on 'Apply' button or undo them by clicking on 'Revert' button.

Tricks to simplify fields filling

There are several special copy/paste methods in spreadsheet. They may be useful when entering field values that are repeated in a few components.

These methods are illustrated below.

Copy (Ctrl+C) Selection Paste (Ctrl+V)
















These techniques are also available in other dialogs with a grid control element.

Import tool for footprint assignment

Accès :

The icon Import Footprint Names icon launches the back-annotate tool.

This tool allows footprint changes made in the PCB Editor to be imported back into the footprint fields in the Schematic Editor.

Managing Symbol Libraries

Symbol libraries hold collections of symbols used when creating schematics. Each symbol in a schematic is uniquely identified by a full name that is composed of a library nickname and a symbol name. An example is Audio:AD1853.

Symbol Library Table

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…​.

sym lib table dlg

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

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

Configuration Initiale

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.

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.

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.

Substitution d’une Variable d’Environnement

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.

Scénarios d’Utilisation

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

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

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

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

Migrating 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.

Legacy Project Remapping

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

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

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

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

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

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

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

Création et édition de schémas


Un schéma peut être représenté sur une seule feuille, mais, s’il est assez grand, il lui faudra plusieurs feuilles.

A schematic represented by several sheets is hierarchical, and all its sheets (each one represented by its own file) constitute a complete KiCad schematic. The manipulation of hierarchical schematics will be described in the Hierarchical Schematics chapter.


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:

A schematic mainly consists of symbols, wires, labels, junctions, buses and power ports. For clarity in the schematic, you can place purely graphical elements like bus entries, comments, and polylines.

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.

Symbol placement and editing

Find and place a symbol

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.

Fenêtre de sélection de composant

The Choose Symbols dialog will filter symbols by name, keywords, and description according to what you type into the search field. Advanced filters can be used just by typing them:

  • Wildcards: use the characters ? and * respectively to mean "any character" and "any number of characters".

  • Relational: 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 expression: 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.

Here is a symbol during placement:

composant en cours de placement

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.

Symbol Editing and Modification (already placed component)

There are two ways to edit a symbol:

  • Modification of the symbol itself: position, orientation, unit selection on a multi-unit symbol.

  • Modification of one of the fields of the symbol: reference, value, footprint, etc.

When a symbol has just been placed, you may have to modify its value (particularly for resistors, capacitors, etc.), but it is useless to assign to it a reference number right away, or to select the unit (except for components with locked units, which you have to assign manually). This can be done automatically by the annotation function.

Symbol modification

To modify some feature of a symbol, position the cursor on the symbol, and then either:

  • Double-click on the symbol to open the full editing dialog.

  • Faites un clic droit pour ouvrir le menu contextuel et choisissez l’une des commandes : Déplacer, Orienter, Éditer, Supprimer, etc…​

  • Use a hotkey to perform an action on the symbol (E to open the properties dialog, R to rotate, etc.). Note that hotkeys act on the selected symbol; if no symbol is selected hotkeys act on the symbol under the cursor.

Symbols can also be selected by clicking on them or drag-selecting them. Selected symbols can be modified by clicking relevant buttons in the top toolbar or using a hotkey.

Édition des champs du composant

Vous pouvez modifier la référence, la valeur, la position, l’orientation, la taille du texte et la visibilité des champs :

  • Double-cliquez sur le champ à modifier.

  • Faites un clic droit pour ouvrir le menu contextuel et choisissez l’une des commandes : Déplacer, Orienter, Éditer, Supprimer, etc…​

  • Position the cursor over the field (if nothing is selected) or select the field and press E to edit the field.

  • Position the cursor over the symbol (if nothing is selected) or select the symbol and press V, U, or F hotkeys to directly edit the symbol’s value, reference designator, or footprint fields, respectively.

For more options, or in order to create fields, double-click on the symbol to open the Symbol Properties dialog.

Fenêtre des propriétés du composant

Each field can be visible or hidden, and displayed horizontally or vertically. The displayed position is always indicated for a normally displayed symbol (no rotation or mirroring) and is relative to the anchor point of the symbol.

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.

Symbol Fields Table

TODO: Write this section.

Electrical Connections


There are a number of elements that can be added to a schematic to electrically connect components. All of these elements can be placed with the buttons on the vertical right toolbar or using hotkeys.

Ces éléments peuvent être des :

  • Wires: direct connection between pins.

  • Buses: connections for a group of signals.

  • Bus entries: connections between wires and buses.

  • No-connection flags: terminations for pins or wires that are intentionally unconnected. These flags prevent ERC violations for unconnected pins.

  • Junctions: connections between crossing wires or buses.

  • Net labels: local name for a signal. Signals within a sheet that have the same net label are connected.

  • Global labels: global name for a signal. Signals with the same global label are connected even if they are not in the same sheet.

  • Hierarchical labels: a label for a signal in a subsheet that enables the signal to be accessed in a parent sheet. See the Hierarchical Schematics section for more information about hierarchical labels, sheets, and pins.

  • Hierarchical sheets: an instantiation of a subsheet within a parent sheet. The parent sheet can connect to the subsheet through the subsheet’s hierarchical pins.

  • Hierarchical pins: connection points between a parent sheet and a subsheet. Hierarchical pins appear at the parent sheet’s level and correspond to hierarchical labels in the subsheet.

Several other types of items can be placed on the schematic but do not affect connectivity:

  • Graphical lines: graphical lines for presentation.

  • Text: textual comments and annotations.

  • Bitmap images: raster graphics from an external file.

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).

Connexions (Fils et Labels)

Il y a deux moyens d’établir des connexions :

  • Fils de pin à pin.

  • Labels.

La figure ci-dessous montre les deux méthodes :

Labels de fils
Label Connections

The point of "contact" of a label is the small square in the corner of the label. The square disappears when the label is connected. The position of the connection point relative to the label text can be changed by choosing a different label orientation in the label properties, or by mirroring/rotating the label.

The label’s connection point must be in contact with a wire or the end of a pin for the label to be connected.

Wire Connections

Pour établir une connexion, un segment de fil doit être connecté par ses extrémités à un autre segment ou à une pin de composant.

Si il y a chevauchement (si un fil survole une pin sans être connecté à son extrémité), il n’y a pas de connexion.

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.
Wire Junctions

Wires that cross are not implicitly connected. It is necessary to join them with a junction dot if a connection is desired. Junction dots will be automatically added to wires that start or end on top of an existing wire.

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

Nets with Multiple Names

A signal 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.

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 automatically be connected to the global VCC net.

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, the use of invisible power pins in symbols is not recommended outside of power port symbols, and is only supported for compatibility with legacy designs and symbols.
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 (options) 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.

It is not recommended to use labels for power connection. These only have a "local" connection scope, and will not connect to invisible power pins.


To begin connecting elements, you may either use the 'Wire' or 'Bus' tools from the right-hand toolbar, or you can auto-start a new wire from any existing pin or unconnected wire.

The wire drag action will drag the entire wire if you start dragging from the middle of the wire. Alternatively, it will drag just one corner if you start the drag action over a corner where two wires connect

Connexions (Bus)

Dans le schéma ci-dessous, de nombreuses pins sont connectées à des bus.

Exemple de schéma avec des bus :
Membres d’un bus

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, and are named using labels the same way signal wires are. There are two types of bus in KiCad 6.0 and later: vector buses and group buses.

A vector bus is a collection of signals that start with a common prefix and end with a number. Vector buses are named <PREFIX>[M..N] where PREFIX is any valid signal name, M is the first suffix number, and N is the last suffix number. For example, the bus DATA[0..7] contains the signals DATA0, DATA1, and so on up to DATA7. It doesn’t matter which order M and N are specified in, but both must be non-negative.

A group bus is a collection of one or more signals and/or vector buses. Group buses can be used to bundle together related signals even when they have different names. Group buses use a special label syntax:


The members of the group are listed inside curly braces ({}) separated by space characters. An optional name for the group goes before the opening curly brace. If the group bus is unnamed, the resulting nets on the PCB will just be the signal names inside the group. If the group bus has a name, the resulting nets will have the name as a prefix, with a period (.) separating the prefix from the signal name.

For example, the bus {SCL SDA} has two signal members, and in the netlist these signals will be SCL and SDA. The bus USB1{DP DM} will generate nets called USB1.DP and USB1.DM. For designs with larger buses that are repeated across several similar circuits, using this technique can save time.

Group buses can also contain vector buses. For example, the bus MEMORY{A[7..0] D[7..0] OE WE} contains both vector buses and plain signals, and will result in nets such as MEMORY.A7 and MEMORY.OE on the 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.

Connexions entre membres de bus

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.

Dans l’exemple ci-dessus, les connexions sont faites par des labels placés sur les fils connectés aux pins. Les entrées de bus (segments de fil à 45 degrés) sont purement décoratifs, et ne sont pas nécessaires pour établir des connexions logiques.

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.

  • Dessinez le fil sous le premier label. Ensuite, utilisez la commande de répétition pour placer les autres fils sous les autres labels.

  • Au besoin, placez les entrées de bus de la même façon (placez la première entrée, puis utilisez la commande de répétition).

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.).

Bus unfolding

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.

After selecting the bus member, the next click will place the bus member label at the desired location. The tool automatically generates a bus entry and wire leading up to the label location. After placing the label, you can continue placing additional wire segments (for example, to connect to a component pin) and complete the wire in any of the normal ways.

Bus aliases

Bus aliases are shortcuts that allow you to work with large group buses more efficiently. They allow you to define a group bus and give it a short name that can then be used instead of the full group name across the schematic.

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

Bus Definitions Dialog

An alias may be named any valid signal name. Using the dialog, you can add signals or vector buses to the alias. As a shortcut, you can type or paste in a list of signals and/or buses separated by spaces, and they will all be added to the alias definition. In this example, we define an alias called USB with members DP, DM, and VBUS.

After defining an alias, it can be used in a group bus label by putting the alias name inside the curly braces of the group bus: {USB}. This has the same effect as labeling the bus {DP DM VBUS}. You can also add a prefix name to the group, such as USB1{USB}, which results in nets such as USB1.DP as described above. For complicated buses, using aliases can make the labels on your schematic much shorter. Keep in mind that the aliases are just a shortcut, and the name of the alias is not included in the netlist.

Bus aliases are saved in the schematic file. Any aliases created in a given schematic sheet are available to use in any other schematic sheet that is in the same hierarchical design.

Buses with more than one label

KiCad 5.0 and earlier allowed the connection of bus wires with different labels together, and would join the members of these buses during netlisting. This behavior has been removed in KiCad 6.0 because it is incompatible with group buses, and also leads to confusing netlists because the name that a given signal will receive is not easily predicted.

If you open a design that made use of this feature in a modern version of KiCad, you will see the Migrate Buses dialog which guides you through updating the schematic so that only one label exists on any given set of bus wires.

Bus Migration Dialog

For each set of bus wires that has more than one label, you must choose the label to keep. The drop-down name box lets you choose between the labels that exist in the design, or you can choose a different name by manually entering it into the new name field.

Power Ports

Power port symbols are conventionally used to connect pins to power nets. Power port symbols have a single pin which is invisible and marked as a power input. As described in the hidden power pins section, any wire connected to the pin of a power port is therefore automatically connected to the power net with the same name as the port’s pin.

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 hidden pin marked as a power input. Name the pin according to the desired power net.

La figure ci-dessous montre un exemple de connexion de sources d’alimentation.

Exemples de sources d’alimentations

In this example, power ports symbols are used to connect the positive and negative terminals of the capacitors to the VCC and GND nets, respectively.

Power port symbols are found in the power symbol library. They can also be created by drawing a symbol with a hidden "power input" pin that has the name of the desired power net.


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.

Compléments Graphiques

Text comments 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.

Cadre et exemple de texte de commentaire.


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

Fenêtre des Options de la page

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.

A drawing sheet template file can also be selected.

Bloc Titre

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

Rescuing cached symbols

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:

Fenêtre de résolution des conflits

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.

If you would prefer not to see this dialog, you can press "Never Show Again". The default will be to do nothing and allow the new components to be loaded. This option can be changed back in the Libraries preferences.

Schématiques hiérarchiques


Une représentation hiérarchique est généralement une bonne solution pour des projets dépassant quelques feuilles. Si vous voulez gérer ce type de projet, il vous faudra :

  • Utiliser de grande feuilles, ce qui pourrait conduire à des problèmes d’impression ou de manipulation.

  • Utiliser plusieurs feuilles, ce qui vous amène à une structure hiérarchique.

La schématique complète consiste alors en une feuille principale, appelée feuille racine, et des sous-feuilles constituant la hiérarchie. En outre, une habile subdivision du schéma en plusieurs feuilles augmentera souvent sa lisibilité.

From the root sheet, you must be able to find all sub-sheets. Hierarchical schematics management is very easy with KiCad, thanks to an integrated "hierarchy navigator" accessible via the icon Hierarchy navigator icon of the top toolbar.

There are two types of hierarchy that can exist simultaneously: the first one has just been evoked and is of general use. The second consists in creating symbols in the library that appear like traditional symbols in the schematic, but which actually correspond to a schematic which describes their internal structure.

Le second type est utilisé pour concevoir des circuits intégrés, car dans ce cas vous devez utiliser des librairies de fonctions dans le schéma que vous êtes en train de dessiner.

KiCad currently doesn’t treat this second case.

Une hiérarchie peut être :

  • simple : une feuille donnée n’est utilisée qu’une seule fois.

  • complexe : une feuille donnée sera utilisée plusieurs fois (instances multiples).

  • à plat : c’est un hiérarchie simple, mais les liaisons entre feuilles ne sont pas dessinées.

KiCad can deal with all these hierarchies.

La création d’une schématique hiérarchique est facile, la hiérarchie étant manipulée à partir de la feuille racine, comme si vous n’aviez qu’un seul schéma.

Les deux étapes importantes à comprendre sont :

  • Comment créer une sous-feuille.

  • How to build electrical connections between sub-sheets.

Navigation among sub-sheets is achieved by using the navigator tool accessible via the button Hierarchy navigator icon on the top toolbar.


Each sheet is reachable by clicking on its name. For quick access, right click on a sheet name, and choose to Enter Sheet or double click within the bounds of the sheet.

In order to exit the current sheet to the parent sheet, right click anywhere in the schematic where there is no object and select "Leave Sheet" in the context menu or press Alt+Backspace.

Labels locaux, hiérarchiques et globaux


Local labels, tool Local label icon, are connecting signals only within a sheet. Hierarchical labels (tool Hierarchical label icon) are connecting signals only within a sheet and to a hierarchical pin placed in the parent sheet.

Global labels (tool Global label icon) are connecting signals across all the hierarchy. Power pins (type power in and power out) invisible are like global labels because they are seen as connected between them across all the hierarchy.

À l’intérieur d’une hiérarchie, on peut utiliser à la fois des labels globaux ou hiérarchiques.

Summary of hierarchy creation

Vous devez :

  • Placer dans la feuille racine un symbole appelé "Feuille hiérarchique".

  • Accéder à cette nouvelle feuille schématique (sous-feuille) par le navigateur, et la dessiner, comme n’importe quel schéma.

  • Draw the electric connections between the two schematics by placing Global Labels (HLabels) in the new schematic (sub-sheet), and labels having the same name in the root sheet, known as SheetLabels. These SheetLabels will be connected to the sheet symbol of the root sheet to the other elements of the schematic like standard symbol pins.

Symbole de feuille hiérarchique

Tracez un rectangle symbolisant la sous-feuille, en plaçant deux points sur une diagonale.

La taille de ce rectangle vous permettra d’ajouter plus tard des labels particuliers, des pins de hiérarchie, correspondant aux labels globaux (Hlabels) de la sous-feuille.

These labels are similar to usual symbol pins. Select the tool Add hierarchical subsheet icon.

Cliquez pour placer le coin supérieur gauche du rectangle. Cliquez à nouveau pour positionner le coin inférieur droit, afin d’avoir un rectangle suffisamment grand.

On vous demandera alors de donner un nom de fichier et un nom de feuille pour cette sous-feuille, pour vous permettre de l’atteindre par le navigateur de hiérarchie.


Vous devez au moins spécifier un nom de fichier. En l’absence de nom de feuille, c’est le nom de fichier qui sera utilisé comme nom de feuille (c’est la méthode habituelle).

Connexions - Pins hiérarchiques

Vous allez maintenant créer des points de connexion (pins hiérarchiques) pour le symbole de feuille qui vient d’être créé.

These points of connection are similar to normal symbol pins, with however the possibility to connect a complete bus with only one point of connection.

Importing Hierarchical Sheet Pins

  • Select the tool Import hierarchical pin icon.

  • Click on the hierarchical sheet from where you want to import the pins corresponding to hierarchical labels placed in the corresponding schematic. A hierarchical pin appears, if a new hierarchical label exists, i.e. not corresponding to an already placed pin.

  • Cliquez où vous souhaiter placer la pin.

All necessary pins can thus be placed quickly and without error. Their aspect is in accordance with corresponding hierarchical labels.

Connexions - Labels hiérarchiques

Each pin of the sheet symbol just created, must correspond to a label called hierarchical Label in the sub-sheet. Hierarchical labels are similar to labels, but they provide connections between sub-sheet and root sheet. The graphical representation of the two complementary labels (pin and hierarchical labels) is similar. Hierarchical labels are made with the tool Add hierarchical label icon.

Ci-dessous un exemple de feuille racine :


Remarquez la pin hiérarchique VCC-PIC, reliée au connecteur JP1.

Voici les connexions correspondantes dans la sous-feuille :


Nous retrouvons les deux labels hiérarchiques correspondants, qui établissent la connexion entre les deux feuilles hiérarchiques.

Vous pouvez utiliser des pins et des labels hiérarchiques pour relier deux bus, en utilisant la syntaxe décrite précédemment (Bus [N..m]).

Labels, labels hiérarchiques, labels globaux et pins d’alimentation invisibles

Quelques remarques sur les différentes façons d’établir des connexions autrement qu’avec des fils.

Labels simples

Les labels simples n’ont qu’une portée locale de connexion, limitée à la feuille de schéma dans laquelle ils sont placés. Ceci est du au fait que :

  • Chaque feuille a un numéro de feuille.

  • Ce numéro de feuille est associé à l’étiquette.

Ainsi, quand vous placez un label "TOTO" dans la feuille n°3, le vrai nom de ce label est "TOTO_3". Si vous avez aussi un label "TOTO" dans la feuille n°1 (feuille racine), c’est en fait un label "TOTO_1" différent de "TOTO_3". Ceci est toujours vrai, même si vous n’avez qu’une seule feuille.

Labels hiérarchiques

Ce que nous avons dit pour les labels simple est vrai aussi pour les labels hiérarchiques.

Thus in the same sheet, a hierarchical label "TOTO" is considered to be connected to a local label "TOTO", but not connected to a hierarchical label or label called "TOTO" in another sheet.

A hierarchical label is considered to be connected to the corresponding sheet pin symbol in the hierarchical symbol placed in the parent sheet.

Pins d’alimentations invisibles

It was seen that invisible power pins were connected together if they have the same name. Thus all the power pins declared "Invisible Power Pins" and named VCC are connected all symbol invisible power pins named VCC only within the sheet they are placed.

En revanche, si vous placez un label VCC dans une sous-feuille, il ne sera pas relié aux pins VCC, parce que ce label est en fait VCC_n, où n est le numéro de la feuille.

If you want this label VCC to be really connected to the VCC for the entire schematic, it will have to be explicitly connected to an invisible power pin via a VCC power symbol.

Labels globaux

Les labels globaux qui portent le même nom sont connectés à travers toute la hiérarchie.

(les labels d’alimentation comme vcc …​ sont des labels globaux)

Hiérarchie complexe

Here is an example. The same schematic is used twice (two instances). The two sheets share the same schematic because the file name is the same for the two sheets (``other_sheet.sch''). The sheet names must be unique.


Hiérarchie à plat

You can create a project using many sheets without creating connections between these sheets (flat hierarchy) if the following rules are observed:

  • Create a root sheet containing the other sheets which acts as a link between others sheets.

  • Aucune connexion explicite n’est nécessaire.

  • Use global labels instead of hierarchical labels in all sheets.

Voici un exemple de feuille racine :


Voici les deux feuilles, connectées par des labels globaux.

Voici la feuille pic_programmer.sch.


Voici la feuille pic_sockets.sch.


Regardez les labels globaux.


Symbol Annotation Tool


The annotation tool allows you to automatically assign a designator to symbols in your schematic. Annotation of symbols with multiple units will assign a unique suffix to minimize the number of these symbols. The annotation tool is accessible via the icon Annotate icon. Here you find its main window.


Available annotation schemes:

  • Annotate all the symbols (reset existing annotation option)

  • Annotate all the symbols, but do not swap any previously annotated multi-unit parts.

  • Annotate only symbols that are currently not annotated. Symbols that are not annotated will have a designator which ends with a '?' character.

  • Annoter toute la hiérarchie (Utiliser la schématique entière).

  • Annoter seulement le schéma en cours (Utiliser la feuille active uniquement).

The Reset, but do not swap any annotated multi-unit parts option keeps all existing associations between symbols with multiple units. For example, U2A and U2B may be reannotated to U1A and U1B respectively but they will never be reannotated to U1A and U2A, nor to U2B and U2A. This is useful if you want to ensure that pin groupings are maintained.

Le choix de l’ordre de l’annotation fixe la méthode utilisée pour affecter les numéros de référence sur chaque feuille de la hiérarchie.

Sauf exception, l’annotation automatique s’applique au projet entier (toutes les feuilles) et aux nouveaux composants, si on ne veut pas modifier les annotations précédentes.

The Annotation Choice gives the method used to calculate reference:

  • Use first free number in schematic: components are annotated from 1 (for each reference prefix). If a previous annotation exists, only unused numbers will be used.

  • Démarrer à numéro de feuille *100 et utiliser le premier nombre libre : l’annotation commence par 101 sur la feuille numéro 1, par 201 sur la feuille numéro 2, etc…​ S’il y a plus de 99 éléments avec le même préfixe de référence (U, R) sur la feuille 1, l’outil d’annotation utilisera le numéro 200 et suivants, et l’annotation de la feuille 2 commencera au prochain numéro libre.

  • Démarrer à numéro de feuille *1000 et utiliser le premier nombre libre : l’annotation commence par 1001 sur la feuille numéro 1, par 2001 sur la feuille numéro 2, etc…​

Quelques exemples

Ordre d’annotation

Cet exemple montre 5 composants, non encore annotés.


Après l’exécution de l’annotation automatique, on obtient le résultat suivant.

Composants triés par position X.


Composants triés par position Y.


Vous pouvez voir que quatre portes 74LS00 ont été réparties dans le boitier U1, et que la cinquième porte 74LS00 a été assignée au suivant, U2.

Choix de l’annotation

Voici une annotation de la feuille 2 avec l’option 'Utiliser le premier nombre libre de la schématique'.


L’option 'Démarrer à numéro de feuille *100 et utiliser le premier nombre libre' donne le résultat suivant.


L’option 'Démarrer à numéro de feuille *1000 et utiliser le premier nombre libre' donne le résultat suivant.


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:

  • Symbol Properties

    • 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.

Filtrage de la Liste d’Empreintes

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 des Fichiers d’Équivalences

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'

Voici un exemple de fichier d’équivalences :

#regulators 'LP2985LV' 'Package_TO_SOT_SMD:SOT-23-5_HandSoldering' ```

==== Visualiser l'Empreinte Courante

The Footprint Assignment Tool contains a footprint viewer. Clicking the image:images/icons/icon_footprint_browser_24.png[footprint viewer icon] button in the top toolbar launches the footprint viewer and shows the selected footprint.

image::images/en/footprint_view.png[scaledwidth="90%", alt="Viewing a footprint"]

The top toolbar contains the following commands:

[width="90%", cols="10%,90%"]
|Refresh view
|Zoom in

|Zoom out

|Zoom to fit drawing in display area

|Show 3D viewer

The left toolbar contains the following commands:

[width="90%", cols="10%,90%"]
|Use the select tool

|Interactively measure between two points

|Display grid dots or lines

|Switch between polar and cartesian coordinate systems

|Use inches

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

|Display coordinates in millimeters

|Toggle display of full-window crosshairs

|Toggle between drawing pads in sketch or normal mode

|Toggle between drawing pads in normal mode or outline mode

|Toggle between drawing text in normal mode or outline mode

|Toggle between drawing graphic lines in normal mode or outline mode

===== Visualisation du Modèle 3D Courant
Clicking the image:images/icons/shape_3d_24.png[3D Viewer icon] button opens the footprint in the 3D model viewer.

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

image::images/en/3d_window.png[scaledwidth="90%", alt="3D-Model view"]

The 3D Viewer is described in the xref:../pcbnew/pcbnew_inspecting.adoc#threed-viewer[PCB Editor manual].


== Vérification des règles électriques (ERC)

=== Introduction

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.

image::images/fr/dialog_erc.png[alt="La fenêtre de l'ERC.", scaledwidth="70%"]

=== Utilisation de l'ERC

ERC can be started by clicking on the icon image:images/icons/erc_24.png[ERC icon].

Des avertissements, sous forme de petites flèches de marquage, seront placés sur les éléments schématiques générant une erreur ERC (pins ou labels).

* Dans cette boite de dialogue, en cliquant sur un message d'erreur, vous allez au marqueur d'erreur correspondant dans le schéma.
* Dans le schéma, faites un clic droit sur un marqueur pour accéder au message de diagnostic correspondant.

You can also delete error markers from the dialog and set specific ERC messages to be suppressed by using the right-click context menu.

image::images/erc_ignore_warning.png[alt="Ignore ERC warning", scaledwidth="70%"]

=== Exemple d'ERC

image::images/erc_pointers.png[alt="Marqueurs d'ERC", scaledwidth="70%"]

Ici, vous pouvez voir quatre erreurs :

* Deux sorties logiques ont été reliées ensemble (flèche rouge).
* Deux entrées ne sont pas connectées (flèches vertes du bas).
* Une erreur sur une source d'alimentation invisible, dont il manque le symbole d'alimentation (flèche verte du haut).

=== Affichage du diagnostic

Un clic droit sur un marqueur vous affiche le menu contextuel permettant d'accéder à la fenêtre d'informations de diagnostic de l'ERC.

image::images/en/erc_pointers_info.png[alt="Infos des marqueurs de L'ERC", scaledwidth="70%"]

et en cliquant sur un marqueur, vous obtenez une description de l'erreur.

image::images/erc_pointers_message.png[alt="ERC pointers message", scaledwidth="80%"]

=== Pins d'alimentation et symboles d'alimentation (Power Flag)

It is common to have an error or a warning on power pins, as shown in the example above, even though all seems normal. This happens in designs where the power is provided through connectors or other components that are not marked as power sources (unlike a regulator output, which is represented by a Power Out pin). Therefore ERC won't detect any Power Out pin connected to the net and will determine it is not driven by a power source.

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.

image::images/eeschema_power_pins_and_flags.png[alt="Power pins and flags", scaledwidth="70%"]

Et ainsi le marqueur disparaît.

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.

=== 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

image::images/fr/dialog_erc_opts.png[alt="Schematic ERC Pin Conflicts Map", scaledwidth="70%"]

Les règles sont modifiées en cliquant plusieurs fois sur le bouton carré dans le tableau pour faire défiler les différents choix : normal [vert], avertissement [W jaune], erreur [E rouge].

image::images/eeschema_erc_severity.png[alt="Schematic ERC severity settings", scaledwidth="70%"]
The _Violation Severity_ panel in Schematic Setup lets you configure what types of ERC messages should be reported as Errors, Warnings or ignored.

=== Fichier de rapport d'ERC

An ERC report file can be generated and saved by checking the option Write ERC report. The file extension for ERC report files is .erc. Here is an example ERC report file.

ERC control (4/1/1997-14:16:4)

ERC: Warning Pin input Unconnected @ 8.450, 2.350
ERC: Warning passive Pin Unconnected @ 8.450, 1.950
ERC: Warning: BiDir Pin connected to power Pin (Net 6) @ 10.100, 3.300
ERC: Warning: Power Pin connected to BiDir Pin (Net 6) @ 4.950, 1.400

>> Errors ERC: 4


== Transfer Schematic to PCB

=== Généralités
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 **Tools** -> **Update PCB from Schematic** (kbd:[F8]) in both the schematic and board editors. You can also use the image:images/icons/update_pcb_from_sch_24.png[Update PCB from Schematic icon] icon in the top toolbar of the Board Editor.

NOTE: 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.

image::images/update_pcb_from_schematic.png[alt="Update PCB from schematic", scaledwidth="70%"]

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.

=== Options

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

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.


== Tracer / Imprimer

=== Introduction

Les commandes 'Imprimer' et 'Tracer' sont accessibles par le menu 'Fichiers'.

image::images/fr/menu_path_plot.png[alt="eeschema_file_menu_plot_png", scaledwidth="60%"]

The supported output formats are Postscript, PDF, SVG, DXF and HPGL. You can also directly print to your printer.

=== Commandes de tracé communes

Tracer Page Courante:: génère un fichier pour la feuille courante seulement.

Tracer Toutes les Pages:: vous permet de tracer toute la hiérarchie (un fichier est généré pour chaque feuille).

=== Tracer en Postscript

Cette commande vous permet de générer des fichiers au format PostScript.

image::images/fr/eeschema_plot_ps.png[alt="eeschema_plot_postscript_png", scaledwidth="70%"]

Le nom du fichier généré est le nom de la feuille avec l'extension .ps. Vous pouvez désactiver l'option "Tracer cartouche et encadrement". Ceci est utile quand vous voulez créer un fichier PostScript pour l'encapsulation (format .eps), utilisé pour insérer une figure dans un logiciel de traitement de texte. La fenêtre de message affiche le chemin et le nom des fichiers créés.

=== Tracer en PDF

image::images/fr/eeschema_plot_pdf.png[alt="eeschema_plot_pdf.png", scaledwidth="70%"]

Vous permet de générer un tracé au format PDF. Le nom du fichier généré est le nom de la feuille avec l'extension .pdf.

=== Tracer en SVG

image::images/fr/eeschema_plot_svg.png[alt="eeschema_plot_svg_png", scaledwidth="70%"]

Vous permet de générer un tracé au format vectoriel SVG. Le nom du fichier généré est le nom de la feuille avec l'extension .svg.

=== Tracer en DXF

image::images/fr/eeschema_plot_dxf.png[alt="eeschema_plot_dxf_png", scaledwidth="70%"]

Vous permet de générer un tracé au format DXF. Le nom du fichier généré est le nom de la feuille avec l'extension .dxf.

=== Tracer en HPGL

Vous permet de générer un tracé au format HPGL. Pour ce format, vous pouvez définir :

* La taille de page.
* L'origine.
* La taille du pinceau (en mm).

La fenêtre de configuration du tracé ressemble à ceci :

image::images/fr/eeschema_plot_hpgl.png[alt="eeschema_plot_hpgl_png", scaledwidth="70%"]

Le nom du fichier généré sera le nom de la feuille avec l'extension .plt.

==== Sélection de la taille de la feuille schématique

La case 'Taille Shématique' est normalement cochée. Dans ce cas, la taille de la feuille définie dans les options de la page sera utilisée, et l'échelle choisie sera de 1. Si une autre taille de feuille est sélectionnée (de A4 à A0, de A à E, etc..), l'échelle sera automatiquement ajustée pour remplir la page.

==== Ajustement des décalages

Pour toutes les dimensions standards, vous pouvez ajuster les décalages pour centrer le dessin aussi précisément que possible. Certains traceurs ayant un point d'origine au centre, et d'autres au coin inférieur droit, il est nécessaire de pouvoir introduire un décalage pour tracer correctement.

Généralement :

* Pour des traceurs ayant leur point d'origine au centre de la feuille, le décalage doit être négatif et fixé à la moitié de la dimension de la feuille.
* Pour des traceurs ayant leur point d'origine dans le coin inférieur gauche de la feuille, le décalage doit être réglé à 0.

Pour fixer un décalage :

* Sélectionnez la taille de la feuille.
* Fixez les décalages X et Y.
* Cliquez sur accepter les décalages.

=== Imprimer sur papier

This command, available via the icon image:images/icons/print_button_24.png[Print icon], allows you to visualize and generate design files for the standard printer.

image::images/fr/print_dialog.png[alt="print_dialog_png", scaledwidth="50%"]

L'option "Imprimer cartouche" active ou désactive l'impression du cartouche.

L'option "Imprimer en noir et blanc seulement" force l'impression en monochrome. Cette option est généralement nécessaire si vous avez une imprimante laser noir et blanc, parce que les couleurs, imprimées en demi-tons, ne sont souvent pas très lisibles.


== Symbol Editor

=== General Information About Symbol Libraries

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.

=== Symbol Library Overview

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

A symbol is composed of:

* Graphical items (lines, circles, arcs, text, etc.) that determine how symbol looks in a schematic.
* Pins which have both graphic properties (line, clock, inverted, low level active, etc.) and electrical properties (input, output, bidirectional, etc.) used by the Electrical Rules Check (ERC) tool.
* Des champs : référence, valeur, empreintes correspondantes pour le dessin du circuit imprimé, etc...

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.

Proper symbol designing requires:

* Defining if the symbol is made up of one or more units.
* Defining if the symbol has an alternate body style (also known as a De Morgan representation).
* De dessiner sa représentation symbolique, au moyen de lignes, rectangles, cercles, polygones, et de texte.
* D'ajouter des pins, en définissant leurs éléments graphiques, leurs noms, leurs numéros et leurs propriétés électriques (entrées, sorties, trois-états, alimentations, etc..).
* Determining if the symbol should be derived from another symbol with the same graphical design and pin definition.
* D'ajouter des champs supplémentaires, comme le nom de l'empreinte utilisée par le logiciel de dessin du circuit imprimé, et de définir leur visibilité.
* Documenting the symbol by adding a description string and links to data sheets, etc.
* De le sauvegarder dans la librairie désirée.

=== Symbol Library Editor Overview

The symbol library editor main window is shown below. It consists of three tool bars for quick access to common features and a symbol viewing/editing area. Not all commands are available on the tool bars but can be accessed using the menus.

image::images/libedit_main_window.png[alt="Symbol Editor main window", scaledwidth="95%"]

==== Barre d'outils principale

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.

image::images/toolbar_libedit.png[alt="Symbol Editor toolbar", scaledwidth="95%"]

[width="100%", cols="20%,80%"]
|image:images/icons/new_component_24.png[New symbol icon]
|Create a new symbol in the selected library.

|image:images/icons/save_24.png[Save icon]
|Save the currently selected library. All modified symbols in the library will
be saved.

|image:images/icons/undo_24.png[Undo icon]
|Undo last edit.

|image:images/icons/redo_24.png[Redo icon]
|Redo last undo.

|image:images/icons/refresh_24.png[Refresh icon]|Refresh display.

|image:images/icons/zoom_in_24.png[Zoom in icon]|Zoom in.

|image:images/icons/zoom_out_24.png[Zoom out icon]|Zoom out.

|image:images/icons/zoom_fit_in_page_24.png[Zoom to fit page icon]|Zoom to fit symbol in display.

|image:images/icons/zoom_selection_24.png[Zoom to selection icon]|Zoom to fit selection.

|image:images/icons/rotate_ccw_24.png[Rotate counterclockwise icon]|Rotate counter-clockwise.

|image:images/icons/rotate_cw_24.png[Rotate clockwise icon]|Rotate clockwise.

|image:images/icons/mirror_h_24.png[Mirror horizontally icon]|Mirror horizontally.

|image:images/icons/mirror_v_24.png[Mirror vertically icon]|Mirror vertically.

|image:images/icons/part_properties_24.png[Symbol properties icon]
|Edit the current symbol properties.

|image:images/icons/pin_table_24.png[Pin table icon]
|Edit the symbol's pins in a tablular interface.

|image:images/icons/datasheet_24.png[Datasheet icon]
|Open the symbol's datasheet. The button will be disabled if no datasheet is
defined for the current symbol.

|image:images/icons/erc_24.png[ERC icon]
|Test the current symbol for design errors.

|image:images/icons/morgan1_24.png[Normal body style icon]
|Select the normal body style. The button is disabled if the current
symbol does not have an alternate body style.

|image:images/icons/morgan2_24.png[Alternate body style icon]
|Select the alternate body style. The button is disabled if the current
symbol does not have an alternate body style.

|image:images/toolbar_libedit_part.png[alt="Unit dropdown",width="80%"]
|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.

|image:images/icons/pin2pin_24.png[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.

|image:images/icons/add_symbol_to_schematic_24.png[Add symbol to schematic icon]
Insert current symbol into schematic.


==== Barre d'outils des éléments

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.

[width="100%", cols="10%,90%"]
|image:images/icons/cursor_24.png[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

|image:images/icons/pin_24.png[Pin icon]
|Pin tool. Left-click to add a new pin.

|image:images/icons/text_24.png[Text icon]
|Graphical text tool. Left-click to add a new graphical text item.

|image:images/icons/add_rectangle_24.png[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.

|image:images/icons/add_circle_24.png[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.

|image:images/icons/add_arc_24.png[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.

|image:images/icons/add_line_24.png[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.

|image:images/icons/anchor_24.png[Anchor icon]
|Anchor tool. Left-click to set the anchor position of the symbol.

|image:images/icons/delete_cursor_24.png[Delete icon]
|Delete tool. Left-click to delete an object from the current symbol.

==== Barre d'outils des options

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

[width="100%", cols="10%,90%"]
|image:images/icons/grid_24.png[Grid icon]
|Toggle grid visibility on and off.

|image:images/icons/unit_inch_24.png[Inch unit icon]
|Set units to inches.

|image:images/icons/unit_mil_24.png[Millimeter unit icon]
|Set units to mils (0.001 inch).

|image:images/icons/unit_mm_24.png[Millimeter unit icon]
|Set units to millimeters.

|image:images/icons/cursor_shape_24.png[Cursor shape icon]
|Toggle full screen cursor on and off.

|image:images/icons/pin_show_etype_24.png[Show pintype icon]
|Toggle display of pin electrical types.

|image:images/icons/search_tree_24.png[Symbol tree icon]
|Toggle display of libraries and symbols.

=== Sélection et gestion des librairies

The selection of the current library is possible via the image:images/icons/search_tree_24.png[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.

==== Select and Save a Symbol

===== Symbol Selection

Clicking the image:images/icons/search_tree_24.png[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.

===== Save a Symbol

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

To save the modified symbol in the current library, click the image:images/icons/save_24.png[Save icon] icon. The modifications will be written to the existing symbol.

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

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

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

=== Creating Library Symbols

==== Create a New Symbol

A new symbol can be created by clicking the image:images/icons/new_component_24.png[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, Symbol Properties window>>.

image::images/eeschema_new_symbol_properties.png[alt="New symbol properties", scaledwidth="50%"]

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

image::images/eeschema_libedit_new.png[alt="Newly created symbol", scaledwidth="95%"]

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 image:images/icons/anchor_24.png[Anchor icon] icon and clicking on the new desired anchor position.

==== Create a Symbol from Another Symbol

Often, the symbol that you want to make is similar to one already in a symbol library. In this case it is easy to load and modify an existing symbol.

* Load the symbol which will be used as a starting point.
* Save a new copy of the symbol using **File** -> **Save As...**. The Save As dialog will prompt for a name for the new symbol and the library to save it in.
* Edit the new symbol as required.
* Save the modified symbol.

==== Symbol Properties

Symbol properties are set when the symbol is created but they can be modified at any point. To change the symbol properties, click on the image:images/icons/part_properties_24.png[Symbol properties icon] icon to show the dialog below.

image::images/eeschema_properties_for_symbol.png[alt="Symbol Properties", scaledwidth="60%"]

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.

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

image::images/eeschema_uncheck_pin_name_inside.png[alt="Place pin name inside unchecked", scaledwidth="95%"]

===== 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.

image::images/eeschema_add_symbol_search_description.png[alt="Searching for a symbol in the add a symbol dialog", scaledwidth="65%"]

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`.

image::images/eeschema_libedit_footprint.png[alt="Footprint filters", scaledwidth="70%"]

==== Symbols with Alternate Symbolic Representation

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 image:images/icons/morgan1_24.png[Normal representation icon] icon.

To edit the alternate representation, click on the image:images/icons/morgan2_24.png[Alternate representation icon] icon. Use the image:images/toolbar_libedit_alias.png[images/toolbar_libedit_part.png] dropdown shown below to select the unit you wish to edit.

image::images/eeschema_libedit_select_unit.png[alt="Selecting a symbol unit", scaledwidth="80%"]

=== Éléments graphiques

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

* Lignes et polygones définis par des points d'origine et des points de fin.
* Rectangles définis par leurs deux coins opposés sur la diagonale.
* Cercles définis par leur centre et leur rayon.
* Arcs de cercles définis par leur centre et leurs points de départ et de fin. Un arc peut aller de 0 à 180°.

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

==== Appartenance des éléments graphiques

Chaque élément graphique, (ligne, arc, cercle, etc...), peut être défini comme commun à toutes les unités et/ou représentations, ou spécifique à une unité donnée et/ou une représentation. Les options des éléments sont accessibles rapidement par le menu contextuel : clic droit sur l'élément à modifier. Ci-dessous, le menu contextuel pour un élément de type ligne.

image::images/eeschema_libedit_context_menu.png[alt="Graphic line context menu", scaledwidth="80%"]

Vous pouvez aussi double-cliquer sur un élément et modifier ses propriétés. Ci-dessous, la fenêtre des propriétés pour un élément de type polygone.

image::images/eeschema_libedit_polyline_properties.png[alt="Graphic line properties", scaledwidth="50%"]

Les propriétés d'un élément graphique sont :

* "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.

==== Éléments Graphiques Textes

The image:images/icons/text_24.png[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.

=== Multiple Units per Symbol and Alternate Body Styles

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.

image::images/eeschema_libedit_not_interchangeable.png[alt="Uncheck all units are interchangeable", scaledwidth="60%"]

===== Unit A

image::images/eeschema_libedit_unit1.png[alt="Relay unit A", scaledwidth="45%"]

===== Unit B

image::images/eeschema_libedit_unit2.png[alt="Relay unit B", scaledwidth="45%"]

===== Unit C

image::images/eeschema_libedit_unit3.png[alt="Relay unit C", scaledwidth="45%"]

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

NOTE: "Synchronized Pins Edit Mode" can be enabled by clicking the image:images/icons/pin2pin_24.png[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.

===== Éléments graphiques symboliques

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.

image::images/eeschema_libedit_disable_common.png[alt="Disable common to all units in symbol", scaledwidth="70%"]

=== Création et édition de pins

You can click on the image:images/icons/pin_24.png[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.

==== Généralités sur les pins

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.

Notes importantes :

* 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 [overline]#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.

==== Propriétés des pins

image::images/eeschema_libedit_pin_properties.png[alt="Pin properties", scaledwidth="95%"]

La fenêtre des propriétés des pins vous permet de modifier toutes les caractéristiques d'une pin. Cette fenêtre apparaît automatiquement à la création de la pin ou quand vous double-cliquez sur une pin existante. Vous pouvez modifier :

* The pin name and text size.
* The pin number and text size.
* The pin length.
* The pin electrical type and graphical style.
* Son appartenance aux unités et aux représentations alternatives.
* Pin visibility.
* <<alternate-pin-definitions,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.

image::images/eeschema_libedit_pin_properties_style.png[alt="Pin graphic styles", scaledwidth="95%"]

==== Types électriques des pins

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.

[width="100%", cols="25%,75%"]
| Pin Type | Description
| Input | A pin which is exclusively an input.
| Output | A pin which is exclusively an output.
| Bidirectional | A pin that can be either an input or an output, such as a
microcontroller data bus pin.
| Tri-state | A three state output pin (high, low, or high impedance)
| Passive | A passive symbol pin: resistors, connectors, etc.
| Free | A pin that can be freely connected to any other pin without electrical
| Unspecified | 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 <<creating-power-ports, Power Ports section>> for more information.
| Power output | A pin that provides power to other pins, such as a regulator
| Open collector | An open collector logic output.
| Open emitter | An open emitter logic output.
| Unconnected | 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.

image::images/eeschema_libedit_pin_context_menu.png[alt="Pin context menu", scaledwidth="60%"]

==== Définitions de pins pour unités multiples et représentations alternatives

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 image:images/icons/pin2pin_24.png[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 image:images/icons/morgan2_24.png[Alternate representation icon] button on the tool bar. To edit the pin number for each unit, select the appropriate unit using the image:images/toolbar_libedit_alias.png[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 image:images/icons/pin_table_24.png[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 image:images/icons/small_plus_16.png[Plus icon] and image:images/icons/small_trash_16.png[Trash icon] icons, respectively.

NOTE: 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.

image::images/eeschema_libedit_pin_table.png[alt="Pin table", scaledwidth="95%"]

==== 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.

image::images/eeschema_libedit_alternate_pin_definitions.png[alt="Alternate pin definitions", scaledwidth="60%"]

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.

image::images/eeschema_alternate_pin_assignment_selection.png[alt="Selecting an alternate pin definition", scaledwidth="60%"]

=== Symbol Fields

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.

NOTE: 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.

==== Editing Symbol Fields

To edit an existing symbol field, right-click on the field text to show the field context menu shown below.

image::images/eeschema_libedit_field_context_menu.png[alt="Symbol field context menu", scaledwidth="35%"]

To add new fields, delete optional fields, or edit existing fields, use the image:images/icons/part_properties_24.png[Component properties icon] icon on the main tool bar to open the <<symbol-properties,Symbol Properties dialog>>.

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

Notes importantes :

* 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`.

=== Power Ports

Power ports, or power symbols, are conventionally used to label a wire as part of a power net, like `VCC`, `+5V`, or `GND`. In the schematic below, the `+3.3V` and `GND` symbols are power ports. In addition to acting as a visual indicator that a net is a power rail, a power port will determine the name of the net it is attached to. This is true even if there is another net label attached to the net; the net name determined by the power symbol overrides any other net names.

image::images/eeschema_power_port_example.png[alt="Power port example", scaledwidth="60%"]

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.

Power symbols are handled and created the same way as normal symbols, but there are several additional considerations described below. They consist of a graphical symbol and a pin of the type "Power input" that is marked hidden.

Below is an example of a `GND` power symbol.

image::images/eeschema_libedit_power_symbol.png[alt="Editing a power symbol", scaledwidth="95%"]

==== Creating a Power Port Symbol

Power Port symbols consist of a pin of type "Power input" that is marked invisible. Invisible power input pins have a special property of automatically connecting to a net with the same name as the pin name. A net that is wired to an invisible power input pin will therefore be named after the pin, even if there are other net labels on the net. This connection is global.

NOTE: 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.

image::images/eeschema_libedit_power_symbol_pin.png[alt="Power symbol pin", scaledwidth="60%"]

Pour créer un symbole d'alimentation, utilisez les étapes suivantes :

* 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, <<creating-a-symbol-from-another-symbol,as described earlier>>.

NOTE: When modifying an existing power port symbol, make sure to rename the pin name so that the new symbol connects to the appropriate power net.


== Symbol Library Browser

=== Introduction

The Symbol Library Browser allows you to quickly examine the content of symbol libraries. The Symbol Library Viewer can be accessed by clicking image:images/icons/library_browser_24.png[Library viewer icon] icon on the main toolbar, **View** -> **Symbol Library Browser...**, or clicking **Select With Browser** in the "Choose Symbol" window.

image::images/eeschema_viewlib_choose.png[alt="eeschema_viewlib_choose_png", scaledwidth="60%"]

=== Viewlib - fenêtre principale

image::images/eeschema_viewlib_select_library.png[alt="eeschema_viewlib_select_library_png", scaledwidth="95%"]

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

image::images/eeschema_viewlib_select_component.png[alt="eeschema_viewlib_select_component_png", scaledwidth="95%"]

=== Symbol Library Browser Top Toolbar

The top tool bar in Symbol Library Brower is shown below.

image::images/toolbar_viewlib.png[alt="images/toolbar_viewlib.png", scaledwidth="95%"]

The available commands are:

[width="100%", cols="20%,80%"]
|image:images/icons/library_browser_24.png[Symbol selection icon]
|Selection of the symbol which can be also selected in the displayed

|image:images/icons/lib_previous_24.png[Previous symbol icon]
|Display previous symbol.

|image:images/icons/lib_next_24.png[Next symbol icon]
|Display next symbol.

|image:images/icons/refresh_24.png[] image:images/icons/zoom_in_24.png[]
image:images/icons/zoom_out_24.png[] image:images/icons/zoom_fit_in_page_24.png[]
|Zoom tools.

|image:images/icons/morgan1_24.png[] image:images/icons/morgan2_24.png[]
|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.

|image:images/icons/add_symbol_to_schematic_24.png[Add symbol to schematic icon]
|Close the browser and place the selected symbol in the schematic.


== Création d'une Netliste

=== Généralités

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.
* Schematic and electrical signal simulators.
* Programmable logic (FPGA, CPLD, etc.) compilers.

KiCad supports several netlist formats:

* KiCad format, which can be imported by the KiCad PCB Editor. However, the <<eeschema_schematic_to_pcb.adoc#schematic-to-pcb,"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.

NOTE: 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 <<eeschema_schematic_to_pcb.adoc#schematic-to-pcb,"Update PCB from Schematic">> tool.

=== Formats de Netliste

Netlists are exported with the Export Netlist dialog (**File**->**Export**->**Netlist...**).

Several netlist formats are available, and are selectable with the tabs at the top of the window. Some netlist formats have 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 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 <<adding-new-netlist-generators,the section on adding custom netlist generators>>.

==== KiCad Netlist Format

image::images/eeschema_netlist_dialog_kicad.png[alt="KiCad netlist export", scaledwidth="70%"]

The KiCad netlist exporter does not have any options.

NOTE: 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 <<eeschema_schematic_to_pcb.adoc#schematic-to-pcb,"Update PCB from Schematic">> tool.

==== OrCAD PCB2 Netlist Format

image::images/eeschema_netlist_dialog_orcad.png[alt="OrCAD netlist export", scaledwidth="70%"]

The OrCAD netlist exporter does not have any options.

==== CADSTAR Netlist Format

image::images/eeschema_netlist_dialog_cadstar.png[alt="CADSTAR netlist export", scaledwidth="70%"]

The CADSTAR netlist exporter does not have any options.

==== Spice Netlist Format

image::images/eeschema_netlist_dialog_spice.png[alt="Spice netlist export", scaledwidth="70%"]

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:

* `&mu;` and `M` as unit prefixes are replaced with `u` and `Meg`, respectively
* Units are removed (e.g. `4.7k&ohm;` 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 <<eeschema_simulator.adoc#simulator,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.

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

For more information on the contents of Spice netlists, see the <<spice-netlists,Spice netlist section>>.

=== Exemples de netlistes

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

image::images/eeschema_netlist_schematic.png[alt="sallen_key demo schematic", scaledwidth="95%"]

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

=== Notes sur les netlistes

==== Précautions pour les noms de netlistes

Many software tools that use netlists do not accept spaces in component names, pins, nets, or other fields. Avoid using spaces in pins, labels, names, and value fields of components to ensure maximum compatibility.

In the same way, special characters other than letters and numbers can cause problems. Note that this limitation is not related to KiCad, but to the netlist formats that can then become untranslatable by other software that reads those netlist files.

==== Spice netlists

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.

=== Autres formats

KiCad supports custom netlist generators for exporting netlists in other formats. Some examples of netlist generators are given in the <<eeschema_creating_customized_netlists_and_bom_files.adoc#creating-customized-netlists-and-bom-files,custom netlist generators section>>.

A netlist generator is a script or program that converts the intermediate netlist file created by KiCad into the desired netlist format. The intermediate netlist file contains all of the netlist information required to create an arbitrary netlist for the schematic. Python and XSLT are commonly used tools to create custom netlist generators.

==== Adding new netlist generators

New netlist generators are added by clicking the **Add Generator...** button.

image::images/eeschema_netlist_dialog_add_plugin.png[alt="Custom Netlist Generator", scaledwidth="40%"]

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 `%I` argument represents the input intermediate netlist filename and the `%O` argument represents the output netlist filename. The exact netlist command will depend on the generator script used.

==== Format de la ligne de commande

Consider the following example which uses `xsltproc` to generate a netlist in PADS ASC format. `xsltproc` converts the intermediate netlist using the `netlist_form_pads-pcb.asc.xsl` stylesheet to define the output format:

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

The purpose of each part of the command is as follows:

[width="100%", cols="58%,42%"]
|`xsltproc` |A tool to convert an XML file (the intermediate netlist) according
to an XSLT stylesheet.

|`-o` |Output filename. `%O` is replaced with the name of the
intermediate netlist file, which is `<schematic name>.xml`. Therefore in this
example the complete output filename is `<schematic name>`. An arbitrary
output filename can be specified if desired with `-o <filename>`.

|`/usr/share/kicad/plugins/netlist_form_pads-pcb.asc.xsl` |XSLT stylesheet which
determines how the output is formatted. This particular stylesheet is included
with KiCad, but custom stylesheets can also be created.

|`%I` |Input (intermediate netlist) filename. `%I` is replaced with the name of
the intermediate netlist file, which is `<schematic name>.xml`.

For netlist generators that do not use `xsltproc`, the generator command will differ.

==== Format du fichier intermédiaire de Netliste

See the <<eeschema_creating_customized_netlists_and_bom_files.adoc#creating-customized-netlists-and-bom-files,custom netlist generators section>> for more information about netlist generators, a description of the intermediate netlist format, and some examples of netlist generators.


== Création de Netlistes et BOM personnalisés

=== Fichier intermédiaire de Netliste

BOM files and netlist files can be converted from an Intermediate netlist file created by KiCad.

Ce fichier utilise une syntaxe XML, et est appelé "netliste intermédiaire". Cette netliste intermédiaire inclue une grande quantité de données relatives au circuit, et, pour cette raison, il peut être utilisé par un post-traitement pour créer une liste de composants ou d'autres rapports.

Suivant le fichier de sortie (BOM ou netliste), différentes portions de la netliste intermédiaire seront utilisées dans le post-traitement.

==== Exemple de schéma

image::images/schematic-sample.png[alt="Exemple de schéma", scaledwidth="95%"]

==== Exemple de fichier netliste intermédiaire

Le fichier netliste intermédiaire (utilisant une syntaxe XML) correspondant au schéma ci-dessus :

<?xml version="1.0" encoding="utf-8"?>
<export version="D">
    <date>29/08/2010 20:35:21</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="/"/>
    <libpart lib="device" part="C">
      <description>Condensateur non polarise</description>
        <field name="Reference">C</field>
        <field name="Value">C</field>
        <pin num="1" name="~" type="passive"/>
        <pin num="2" name="~" type="passive"/>
    <libpart lib="device" part="R">
        <field name="Reference">R</field>
        <field name="Value">R</field>
        <pin num="1" name="~" type="passive"/>
        <pin num="2" name="~" type="passive"/>
    <libpart lib="conn" part="CONN_4">
      <description>Symbole general de connecteur</description>
        <field name="Reference">P</field>
        <field name="Value">CONN_4</field>
        <pin num="1" name="P1" type="passive"/>
        <pin num="2" name="P2" type="passive"/>
        <pin num="3" name="P3" type="passive"/>
        <pin num="4" name="P4" type="passive"/>
    <libpart lib="74xx" part="74LS04">
      <description>Hex Inverseur</description>
        <field name="Reference">U</field>
        <field name="Value">74LS04</field>
        <pin num="1" name="~" type="input"/>
        <pin num="2" name="~" type="output"/>
        <pin num="3" name="~" type="input"/>
        <pin num="4" name="~" type="output"/>
        <pin num="5" name="~" type="input"/>
        <pin num="6" name="~" type="output"/>
        <pin num="7" name="GND" type="power_in"/>
        <pin num="8" name="~" type="output"/>
        <pin num="9" name="~" type="input"/>
        <pin num="10" name="~" type="output"/>
        <pin num="11" name="~" type="input"/>
        <pin num="12" name="~" type="output"/>
        <pin num="13" name="~" type="input"/>
        <pin num="14" name="VCC" type="power_in"/>
    <libpart lib="74xx" part="74LS74">
      <description>Dual D FlipFlop, Set &amp; Reset</description>
        <field name="Reference">U</field>
        <field name="Value">74LS74</field>
        <pin num="1" name="Cd" type="input"/>
        <pin num="2" name="D" type="input"/>
        <pin num="3" name="Cp" type="input"/>
        <pin num="4" name="Sd" type="input"/>
        <pin num="5" name="Q" type="output"/>
        <pin num="6" name="~Q" type="output"/>
        <pin num="7" name="GND" type="power_in"/>
        <pin num="8" name="~Q" type="output"/>
        <pin num="9" name="Q" type="output"/>
        <pin num="10" name="Sd" type="input"/>
        <pin num="11" name="Cp" type="input"/>
        <pin num="12" name="D" type="input"/>
        <pin num="13" name="Cd" type="input"/>
        <pin num="14" name="VCC" type="power_in"/>
    <library logical="device">
    <library logical="conn">
    <library logical="74xx">
    <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"/>

=== Conversion dans un nouveau format de netliste

En appliquant un filtre de post-traitement au fichier netliste Intermédiaire, vous pouvez générer des formats inconnus de netliste, ou de BOM. Parce que cette conversion est une transformation de texte en texte, ce filtre de post-traitement pourra être écrit en Python, XSLT, ou tout autre outil capable de prendre du XML en entrée.

XSLT itself is an XML language very suitable for XML transformations. There is a free program called _xsltproc_ that you can download and install. 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.

=== L'approche XSLT

Vous trouverez la documentation qui décrit les transformations XSL (XSLT) ici :


==== Créer un fichier Netliste Pads-Pcb

Le format pads-pcb contient deux sections.

* La liste des empreintes.

* La Netliste : qui regroupe les références des broches par équipotentielles.

Ci-dessous, une feuille de style qui convertit le fichier netliste intermédiaire au format de netliste pads-pcb

<?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="">
<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"/>


Voici le fichier de sortie pads-pcb après traitement par xsltproc :

P1 unknown
U2 unknown
U1 unknown
C1 unknown
R1 unknown


La ligne de commande utilisée pour effectuer cette conversion :

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

==== Créer un fichier de netliste Cadstar

Le format Cadstar contient deux sections.

* La liste des empreintes.

* La Netliste : qui regroupe les références des broches par équipotentielles.

Ci-dessous, la feuille de style pour effectuer cette conversion spécifique :

<?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="">
<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"/>


Le fichier de sortie au format 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


==== Create an OrcadPCB2 netlist file

Ce format a une seule section, qui est la liste des empreintes. Chaque empreinte inclue sa liste de broches avec leurs références d'équipotentielles.

Ci-dessous, la feuille de style pour cette conversion spécifique :

<?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="">
<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">



Le fichier de sortie au format 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 )

==== Netlist plugins interface

Intermediate Netlist converters can be automatically launched within the Schematic Editor.

===== Ouvrez la fenêtre de configuration

Vous pouvez ajouter un nouveau plugin par le bouton "Ajouter Plugin".

image::images/eeschema_plugin_add_plugin.png[alt="eeschema_plugin_add_plugin_png", scaledwidth="50%"]

Voici l'onglet de configuration du plugin pour Pads-Pcb :

image::images/eeschema_plugin_padspcb.png[alt="eeschema_plugin_padspcb_png", scaledwidth="80%"]

===== Configuration des paramètres du plugin

The netlist plug-in configuration dialog requires the following information:

* Un titre : pour l’onglet, comme le nom du format de Netliste.

* La ligne de commande pour lancer la conversion.

Quand vous cliquez sur le bouton netliste :

1.  KiCad creates an intermediate netlist file *.xml, for instance test.xml.

2.  KiCad runs the plug-in by reading test.xml and creates

===== Génération de fichiers netlistes en ligne de commande

Partant du fait que nous utilisons le programme _xsltproc.exe_ pour appliquer la feuille de style au fichier intermédiaire, _xsltproc.exe_ sera exécuté avec la commande suivante :

_xsltproc.exe -o <fichier de sortie> <fichier feuille de style> <fichier XML d'entrée à convertir>_

Sous Windows, la ligne de commande sera la suivante :

_f:/kicad/bin/xsltproc.exe -o "%O" f:/kicad/bin/plugins/netlist_form_pads-pcb.xsl "%I"_

Sous Linux, la ligne de commande sera la suivante :

_xsltproc -o "%O" /usr/local/kicad/bin/plugins/netlist_form_pads-pcb.xsl "%I"_

Where _netlist_form_pads-pcb.xsl_ is the style-sheet that you are applying. Do not forget the double quotes around the file names, this allows them to have spaces after the substitution by KiCad.

Le format de la ligne de commande accepte des paramètres de substitution pour les noms de fichiers :

Les paramètres autorisés sont.

* %B => nom et chemin du fichier de sortie, sans le point et l'extension.

* %I => nom et chemin complets du fichier d'entrée (le fichier intermédiaire de netliste).

* %O => nom et chemin complets du fichier de sortie.

_%I_ sera remplacé par le nom de fichier intermédiaire de netliste.

_%O_ sera remplacé par le nom de fichier de sortie.

===== Format de ligne de commande : exemple pour xsltproc

Le format de ligne de commande de xsltproc est le suivant :

<chemin vers xsltproc> xsltproc <paramètres de xsltproc >

Sous Windows

*f:/kicad/bin/xsltproc.exe -o "%O" f:/kicad/bin/plugins/netlist_form_pads-pcb.xsl "%I"*

Sous Linux

*xsltproc -o "%O" /usr/local/kicad/bin/plugins/netlist_form_pads-pcb.xsl "%I"*

Les exemples ci-dessus supposent que xsltproc est installé sur votre PC sous Windows et que tous les fichiers sont situés dans F:\kicad\bin.

==== Génération de listes de composants (BOM)

Puisque le fichier netliste intermédiaire contient toutes les informations sur les composants utilisés, une liste de composants peut en être extraite. Voici la fenêtre de configuration du plugin (sous Linux) permettant de créer un fichier de BOM (Bill Of Materials) personnalisé :

image::images/en/bom-netlist-tab.png[alt="bom-netlist-tab_png", scaledwidth="80%"]

Le chemin vers la feuille de style bom2csv.xsl dépend de votre système. Actuellement, la meilleure feuille de style XSLT pour la génération du BOM est nommée __bom2csv.xsl__. Vous êtes libre de la modifier en fonction de vos besoins, et si vous développez un autre modèle utile à tous, vous pouvez demander qu'il fasse partie du projet KiCad.

=== Exemples de lignes de commandes pour les scripts Python

Le format d'une ligne de commande pour python ressemble à ceci :

python <fichier script> <fichier d'entrée> <fichier de sortie>

Sous Windows

*python *.exe f:/kicad/python/ "%I" "%O"*

Sous Linux

*python /usr/local/kicad/python/ "%I" "%O"*

Partant du fait que Python est effectivement installé sur votre PC..

=== Structure du fichier de netliste intermédiaire

L'exemple qui suit donne une idée du format du fichier de netliste intermédiaire.

<?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"/>

==== Structure générale

Le fichier de netliste intermédiaire contient cinq sections.

* La section Entête.
* The components section.
* La section Composants en librairie.
* La section Librairies.
* La section Équipotentielles

Le contenu du fichier a pour balises de délimitations <export>

<export version="D">

==== Section Entête (Header)

L'entête a pour balises de délimitations <design>

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

Cette section peut être considérée comme une section de commentaires.

==== Section Composants

La section composants a pour balises de délimitations <components>

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

Cette section contient la liste des composants de votre schéma. Chaque composant est décrit comme ceci :

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

[width="100%", cols="37%,63%"]
|*libsource* |name of the lib where this component was found.

|*part* |component name inside this library.

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

|*tstamps (time stamps)* |time stamp of the schematic file.

|*tstamp (time stamp)* |time stamp of the component.

===== Note à propos de l'horodatage des composants

Pour identifier un composant dans une netliste, et par voie de conséquence sur le circuit, l'horodatage est utilisé comme référence unique pour chaque composant. Toutefois, Kicad fournit un autre moyen pour identifier un composant, qui est son empreinte correspondante sur le circuit. Ceci permet la ré-annotation de composants dans un projet de schéma sans perdre le lien entre le composant et son empreinte.

Un horodatage (timestamp) est un identifiant unique pour chaque composant, ou chaque feuille d'un projet schématique. Cependant, dans des hiérarchies complexes, la même feuille étant utilisée plus d'une fois, cette feuille contiendra des composants avec le même horodatage.

Une feuille donnée à l'intérieur d'une hiérarchie complexe dispose d'un identifiant unique : son chemin de feuille (sheetpath). Un composant donné (à l'intérieur d'une hiérarchie complexe) a donc un identifiant unique : le sheetpath + son timestamp.

==== Section Composants en librairie (libparts)

La section libparts a pour délimiteur <libparts>, et le contenu de cette section est celui défini dans les librairies schématiques. La section libparts contient :

* The allowed footprints names (names use wildcards) delimiter <fp>.
* Les champs définis en librairie, avec pour délimiteur <fields>.
* La liste des pins, avec pour délimiteur <pins>.

<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"/>

Les lignes <pin num="1" type="passive"/> donnent aussi le type électrique de la pin. Les types électriques possibles sont :

[width="94%", cols="25%,75%"]
|Input |Entrée
|Output |Sortie
|Bidirectional |Entrée ou Sortie
|Tri-state |Trois-états
|Passive |Extrémités de composants passifs
|Unspecified |Non-Spécifié
|Power input |Entrée d'alimentation d'un composant
|Power output |Sortie d'alimentation, comme celle des régulateurs
|Open collector |Collecteur ouvert
|Open emitter |Émetteur ouvert
|Not connected |Non-connecté, sera laissé en l'air dans le schéma

====  Section Librairies

La section librairies a pour délimiteur <libraries>. Cette section contient la liste des librairies utilisées dans le projet.

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

==== Section Équipotentielles (nets)

La section nets a pour délimiteur <nets>. Cette section contient la liste des équipotentielles, la "connectivité" du schéma.

  <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"/>

Cette section recense toutes les équipotentielles du schéma.

Une entrée net peut contenir :

<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"/>

[width="77%", cols="20%,80%"]
|net code |Identifiant interne pour ce net
|name |Nom de ce net
|node |Référence une pin de composant connectée à ce net

=== Complément sur xsltproc

Réfère à la page : _

==== Introduction

xsltproc est un outil en ligne de commande pour appliquer des feuilles de styles XSLT à des documents XML. Bien qu'il ait été développé au sein du projet GNOME, il peut opérer indépendamment du bureau GNOME.

xsltproc est invoqué à partir de la ligne de commande, avec le nom de la feuille de style à utiliser, suivi du nom du ou des fichiers auxquels la feuille de style doit être appliquée. Il utilisera l'entrée standard si le nom de fichier d'entrée fournit est - .

Si une feuille de style est incluse dans un document XML, au moyen d'une instruction de traitement de feuille de style, il n'est pas nécessaire de spécifier la feuille de style sur la ligne de commande. xsltproc détectera automatiquement la feuille de style incluse et l'utilisera. Par défaut, la sortie est la sortie standard. Vous pouvez préciser un fichier de sortie en utilisant l'option -o.

==== Synoptique

xsltproc [[-V] | [-v] | [-o *file* ] | [--timing] | [--repeat] |
[--debug] | [--novalid] | [--noout] | [--maxdepth *val* ] | [--html] |
[--param *name* *value* ] | [--stringparam *name* *value* ] | [--nonet] |
[--path *paths* ] | [--load-trace] | [--catalogs] | [--xinclude] |
[--profile] | [--dumpextensions] | [--nowrite] | [--nomkdir] |
[--writesubtree] | [--nodtdattr]] [ *stylesheet* ] [ *file1* ] [ *file2* ]
[ *....* ]

==== Options de la ligne de commande

_-V_ ou _--version_

Affiche les versions de libxml et libxslt qui sont utilisées.

_-v_ ou _--verbose_

Affiche chaque étape de xsltproc lors du traitement du la feuille de style et du document.

_-o_ ou _--output fichier_

Redirige la sortie vers le fichier nommé __fichier__. Pour des sorties multiples, que l'on appelle également ``chunking'', -o répertoire/ redirige les fichiers de sortie vers un répertoire donné. Le répertoire doit déjà exister.


Affiche le temps qu'il a fallu pour traiter la feuille de style, traiter le document, appliquer la feuille de style et enregistrer le résultat. Il est affiché en millisecondes.


Lance la transformation 20 fois de suite. Utile pour des tests de vitesse.


Affiche un arbre XML du document transformé afin de déboguer.


Évite le chargement de la DTD du document.


N'affiche pas le résultat.

_--maxdepth valeur_

Ajuste la profondeur maximale de la pile avant que libxslt ne conclue qu'il y ait une boucle infinie. La valeur par défaut est 500.


Le document en entrée est un fichier HTML.

_--param nom valeur_

Passe un paramètre de nom _nom_ et de valeur _valeur_ à la feuille de style. Vous pouvez passer plusieurs paires nom/valeur, jusqu'à 32 valeurs. Si la valeur qui est spécifiée est une chaîne de caractères au lieu du nom d'identification d'un noeud, vous devez utiliser --stringparam à la place.

_--stringparam nom valeur_

Passe un paramètre de nom _nom_ et de valeur _valeur_ où valeur est une chaîne de caractères plutôt qu'un identifiant de noeud. (Note : La chaîne doit être en utf-8.)


Ne pas utiliser Internet pour récupérer les DTD ou les entités.

_--path chemins_

Use the list (separated by space or column) of filesystem paths specified by _paths_ to load DTDs, entities or documents.


Affiche sur la sortie d'erreurs standard (stderr) tous les documents chargés pendant le traitement.


Utilise les catalogues SGML pour résoudre l'emplacement des entités externes. Par défaut xsltproc utilise les catalogues XML installés dans /etc/xml/catalog.


Traite le document en entrée en utilisant les spécifications Xinclude. Vous pouvez obtenir plus de détails dans les spécifications de Xinclude :[].

_--profile --norman_

Donne des informations détaillant le temps passé pour chaque partie de la feuille de style. C'est utile pour optimiser les performances de la feuille de style.


Affiche la liste de toutes les extensions enregistrées sur la sortie standard (stdout).


N'écrit sur aucun fichier ni ressource.


Ne crée aucun répertoire.

_--writesubtree chemin_

Autorise l'écriture de fichiers seulement sur le sous-répertoire _chemin_.


N'applique pas les attributs par défaut de la DTD du document.

==== Valeurs de retour de xsltproc

xsltproc renvoie un code fournissant des informations qui peuvent être très utiles lorsqu'on l'utilise dans des scripts.

0 : normal

1 : pas d'argument

2 : trop de paramètres

3 : option inconnue

4 : le traitement de la feuille de style a échoué

5 : erreur dans la feuille de style

6 : erreur dans un des documents

7 : méthode de sortie xsl (xsl:output) non-supportée

8 : la chaîne de paramètres contient à la fois des guillemets simples et doubles

9 : erreur interne de traitement

10 : le traitement a été stoppé par un signal d'achèvement

11: Impossible d'écrire le résultat dans le fichier de sortie

==== Plus d'infos sur xsltproc

Page web de la libxml :[]

Page XSLT sur le W3C :[]


== Simulator ==

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

When working with the simulator, you may find the official _pspice_ library useful. It contains common symbols used for simulation like voltage/current sources or transistors with pins numbered to match the ngspice node order specification.

There are also a few demo projects to illustrate the simulator capabilities. You will find them in _demos/simulation_ directory.

=== Assigning models

Before a simulation is launched, components need to have Spice model assigned.

Each component can have only one model assigned, even if component consists of multiple units. In such case, the first unit should have the model specified.

[[sim-passive-models]] Passive components with reference matching a device type in Spice notation (_R*_ for resistors, _C*_ for capacitors, _L*_ for inductors) will have models assigned implicitly and use the value field to determine their properties.

Keep in mind that in Spice notation 'M' stands for milli and 'Meg' corresponds to mega. If you prefer to use 'M' to indicate mega prefix, you may request doing so in the <<sim-settings, simulation settings dialog>>.

Spice model information is stored as text in symbol fields, therefore you may either define it in symbol editor or schematics editor. Open symbol properties dialog and click on _Edit Spice Model_ button to open Spice Model Editor dialog.

Spice Model Editor dialog has three tabs corresponding to different model types. There are two options common to all model types:

[width="90%", cols="30%a,70%a"]
|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.

'Example:' +
`* 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`

image::images/opamp_symbol.png[alt="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{nbsp}3{nbsp}5{nbsp}2{nbsp}4". It is a list of pin numbers corresponding to the Spice model nodes order.

==== Passive

_Passive_ tab allows the user to assign a passive device model (resistor, capacitor or inductor) to a component. It is a rarely used option, as normally passive components have models assigned <<sim-passive-models,implicitly>>, unless component reference does not match the actual device type.

Explicitly defined passive device models have priority over the ones assigned implicitly. It means that once a passive device model is assigned, the reference and value fields are not taken into account during simulation. It may lead to a confusing situation when assigned model value does not match the one displayed on a schematic sheet.

image::images/sim_model_passive.png[alt="Passive device model editor tab"]

[width="90%", cols="30%a,70%a"]
|Selects the device type (resistor, capacitor or inductor).
|Defines the device property (resistance, capacitance or inductance). The value
may use common Spice unit prefixes (as listed below the text input field) and
should use point as the decimal separator. Note that Spice does not correctly
interpret prefixes intertwined in the value (e.g. 1k5).

==== Model

_Model_ tab is used to assign a semiconductor or a complex model defined in an external library file. Spice model libraries are often offered by device manufacturers.

The main text widget displays the selected library file contents. It is a common practice to put models description inside library files, including the node order.

image::images/sim_model_subckt.png[alt="Semiconductor device model editor tab"]

[width="90%", cols="30%a,70%a"]
|Path to a Spice library file. This file is going to be used by the simulator,
as it is added using _.include_ directive.
|Selected device model. When a file is selected, the list is filled with available
models to choose from.
|Selects model type (subcircuit, BJT, MOSFET or diode). Normally it is set
automatically when a model is selected.

==== Source

_Source_ tab is used to assign a power or signal source model. There are two sections: _DC/AC analysis_ and _Transient analysis_. Each defines source parameters for the corresponding simulation type.

_Source type_ option applies to all simulation types.

image::images/sim_model_source.png[alt="Source model editor tab"]

Refer to the[ngspice documentation], chapter 4 (Voltage and Current Sources) for more details about sources.

=== Spice directives

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.

=== Simulation

To launch a simulation, open _Spice Simulator_ dialog by selecting menu _Tools->Simulator_ in the schematics editor window.

image::images/sim_main_dialog.png[alt="Main simulation dialog"]

The dialog is divided into several sections:

* <<sim-toolbar,Toolbar>>
* <<sim-plot-panel,Plot panel>>
* <<sim-output-console,Output console>>
* <<sim-signals-list,Signals list>>
* <<sim-cursors-list,Cursors list>>
* <<sim-tune-panel,Tune panel>>

==== Menu

===== File
[width="90%", cols="30%,70%"]
|New Plot | Create a new tab in the plot panel.
|Open Workbook | Open a list of plotted signals.
|Save Workbook | Save a list of plotted signals.
|Save as image | Export the active plot to a .png file.
|Save as .csv file | Export the active plot raw data points to a .csv file.
|Exit Simulation | Close the dialog.

===== Simulation
[width="90%", cols="30%,70%"]
|Run Simulation | Perform a simulation using the current settings.
|Add signals... | Open a dialog to select signals to be plotted.
|Probe from schematics | Start the schematics <<sim-probe-tool,Probe>> tool.
|Tune component value | Start the <<sim-tuner-tool,Tuner>> tool.
|Show SPICE Netlist... | Open a dialog showing the generated netlist for the
simulated circuit.
|Settings... | Open the <<sim-settings,simulation settings dialog>>.

===== View
[width="90%", cols="30%,70%"]
|Zoom In | Zoom in the active plot.
|Zoom Out | Zoom out the active plot.
|Fit on Screen | Adjust the zoom setting to display all plots.
|Show grid | Toggle grid visibility.
|Show legend | Toggle plot legend visibility.

==== Toolbar
image::images/sim_main_toolbar.png[alt="Simulation dialog top toolbar"]
The top toolbar provides access to the most frequently performed actions.

[width="90%", cols="30%,70%"]
|Run/Stop Simulation | Start or stop the simulation.
|Add Signals | Open a dialog to select signals to be plotted.
|Probe | Start the schematics <<sim-probe-tool,Probe>> tool.
|Tune | Start the <<sim-tuner-tool,Tuner>> tool.
|Settings | Open the <<sim-settings,simulation settings dialog>>.

==== Plot panel
Visualizes the simulation results as plots. One can have multiple plots opened in separate tabs, but only the active one is updated when a simulation is executed. This way it is possible to compare simulation results for different runs.

Plots might be customized by toggling grid and legend visibility using <<sim-menu-view,View>> menu. When a legend is visible, it can be dragged to change its position.

Plot panel interaction:

* scroll mouse wheel to zoom in/out
* right click to open a context menu to adjust the view
* draw a selection rectangle to zoom in the selected area
* drag a cursor to change its coordinates

==== Output console
Output console displays messages from the simulator. It is advised to check the console output to verify there are no errors or warnings.

==== Signals list
Shows the list of signals displayed in the active plot.

Signals list interaction:

* right click to open a context menu to hide signal or toggle cursor
* double click to hide signal

==== Cursors list
Shows the list of cursors and their coordinates. Each signal may have one cursor displayed. Cursors visibility is set using the <<sim-signals-list,Signals>> list.

==== Tune panel
Displays components picked with the <<sim-tuner-tool,Tuner>> tool. Tune panel allows the user to quickly modify component values and observe their influence on the simulation results - every time a component value is changed, the simulation is rerun and plots are updated.

For each component there a few controls associated:

* The top text field sets the maximum component value.
* The middle text field sets the actual component value.
* The bottom text field sets the minimum component value.
* Slider allows the user to modify the component value in a smooth way.
* _Save_ button modifies component value on the schematics to the one selected with the slider.
* _X_ button removes component from the Tune panel and restores its original value.

The three text fields recognize Spice unit prefixes.

==== Tuner tool
Tuner tool lets the user pick components for tuning.

To select a component for tuning, click on one in the schematics editor when the tool is active. Selected components will appear in the <<sim-tune-panel,Tune>> panel. Only passive components might be tuned.

==== Probe tool
Probe tool provides an user-friendly way of selecting signals for plotting.

To add a signal to plot, click on a corresponding wire in the schematics editor when the tool is active.

==== Simulation settings

image::images/sim_settings.png[alt="Simulation settings dialog"]

Simulation settings dialog lets the user set the simulation type and parameters. There are four tabs:

* AC
* DC Transfer
* Transient
* Custom

The first three tabs provide forms where simulation parameters might be specified. The last tab allows the user to type in custom Spice directives to set up a simulation. You can find more information about simulation types and parameters in the[ngspice documentation], chapter 1.2.

An alternative way to configure a simulation is to type <<sim-directives,Spice directives>> into text fields on schematics. Any text field directives related to simulation type are overridden by the settings selected in the dialog. It means that once you start using the simulation dialog, the dialog overriddes the schematics directives until the simulator is reopened.

There are two options common to all simulation types:
[width="90%", cols="30%,70%"]
|Adjust passive symbol values | Replace passive symbol values to convert common
component values notation to Spice notation.
|Add full path for .include library directives | Prepend Spice model library
file names with full path. Normally full path is required by ngspice to access
a library file.