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

==== Podgląd bieżącego footprintu

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/pl/footprint_view.png[scaledwidth="90%", alt="Podgląd footprintu"]

The top toolbar contains the following commands:

[width="90%", cols="10%,90%"]
|=======================================================================
|image:images/icons/refresh_24.png[]
|Refresh view
|image:images/icons/zoom_in_24.png[]
|Zoom in

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

|image:images/icons/zoom_fit_in_page_24.png[]
|Zoom to fit drawing in display area

|image:images/icons/shape_3d_24.png[]
|Show 3D viewer
|=======================================================================

The left toolbar contains the following commands:

[width="90%", cols="10%,90%"]
|=======================================================================
|image:images/icons/cursor_24.png[]
|Use the select tool

|image:images/icons/measurement_24.png[]
|Interactively measure between two points

|image:images/icons/grid_24.png[]
|Display grid dots or lines

|image:images/icons/polar_coord_24.png[]
|Switch between polar and cartesian coordinate systems

|image:images/icons/unit_inch_24.png[]
|Use inches

|image:images/icons/unit_mil_24.png[]
|Display coordinates in mils (1/1000 of an inch)

|image:images/icons/unit_mm_24.png[]
|Display coordinates in millimeters

|image:images/icons/cursor_shape_24.png[]
|Toggle display of full-window crosshairs

|image:images/icons/pad_number_24.png[]
|Toggle between drawing pads in sketch or normal mode

|image:images/icons/pad_sketch_24.png[]
|Toggle between drawing pads in normal mode or outline mode

|image:images/icons/text_sketch_24.png[]
|Toggle between drawing text in normal mode or outline mode

|image:images/icons/show_mod_edge_24.png[]
|Toggle between drawing graphic lines in normal mode or outline mode
|=======================================================================

===== Podgląd bieżącego modelu 3D
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/pl/3d_window.png[scaledwidth="90%", alt="Podgląd 3D"]

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


:experimental:

[[schematic-to-pcb]]
== Transferring designs between schematic and PCB

=== Update PCB from Schematic
Use the Update PCB from Schematic tool to sync design information from the Schematic Editor to the Board Editor. The tool can be accessed with **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.

[cols="1,2"]
|===
| Option | Description

| Re-link footprints to schematic symbols based on their reference designators
| Footprints are normally linked to schematic symbols via a unique identifier
created when the symbol is added to the schematic. A symbol's unique identifier
cannot be changed.

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

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

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

| Delete footprints with no symbols
| If checked, any footprint in the PCB without a corresponding symbol in the
schematic will be deleted from the PCB. Footprints with the "Not in schematic"
attribute will be unaffected.

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

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

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

=== Update Schematic from PCB

NOTE: TODO: write this section

==== Backannotation with CMP files

Select changes can also be synced from the PCB back to the schematic by exporting a CMP file from the PCB editor (**File** -> **Export** -> **Footprint Association (.cmp) File...**) and importing it in the Schematic Editor (**File** -> **Import** -> **Footprint Assignments...**).

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

:experimental:

[[generating-outputs]]
== Generating Outputs

=== Printing

KiCad can print the schematic to a standard printer using **File**->**Print...**.

image::images/eeschema_print.png["Print dialog"]

==== Printing options

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

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

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

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

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

**Preview:** Opens a print preview dialog.

**Close:** Closes the dialog without printing.

**Print:** Opens the system print dialog.

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

=== Plotting

KiCad can plot schematics to a file using **File** -> **Plot...**.

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


image::images/eeschema_plot.png["Plot dialog"]

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

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

==== Plotting options

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

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

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

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

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

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

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

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

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

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

[[bom-export]]
=== Generating a Bill of Materials

KiCad can generate a Bill of Materials using **Tools** -> **Generate BOM...** or the image:images/icons/post_bom_24.png[BOM icon] button on the top toolbar. The generated BOM lists all of the components in the design.

image::images/pl/dialog_bom.png[alt="Główne okno narzędzia BOM", scaledwidth="60%"]

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

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

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

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

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

==== BOM generator scripts

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

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

  ** Line item number
  ** Quantity
  ** Reference designator(s)
  ** Value
  ** Symbol library and symbol name
  ** Footprint
  ** Datasheet
  ** Any other symbol fields

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

  ** Reference designator(s)
  ** Quantity
  ** Value
  ** Symbol name
  ** Footprint
  ** Symbol description
  ** Vendor


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

[options="header", cols="30%,70%"]
|===
|Operating System |Location
|Windows |`C:\Program Files\KiCad\6.0\bin\scripting\plugins\`
|Linux |`/usr/share/kicad/plugins/`
|macOS |`/Applications/KiCad/KiCad.app/Contents/SharedSupport/plugins/`
|===

Additional scripts can be added to the list of BOM generator scripts by clicking the image:images/icons/small_plus_16.png[Plus icon] button. Scripts can be removed by clicking the image:images/icons/small_trash_16.png[Delete icon] button. The image:images/icons/small_edit_16.png[Edit icon] button opens the selected script in a text editor.

For more information on creating and using custom BOM generators, see the <<custom-netlist-and-bom-formats,advanced documentation>>.


[[netlist-export]]
=== Netlists

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

* A list of symbols and their pins.
* A list of connections (nets) between symbol pins.

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

KiCad supports several netlist formats:

* KiCad format, which can be imported by the KiCad PCB Editor. However, the <<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.

NOTE: Other software tools that use netlists may have restrictions on spaces and
      special characters in component names, pins, nets, and other fields. For
      compatibility, be aware of such restrictions in other tools you plan to
      use, and name components, nets, etc. accordingly.

[[netlist-formats]]
==== Format listy sieci

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

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

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

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

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

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

===== Spice Netlist Format

image::images/pl/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 <<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.

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.

[[netlist-examples]]
==== Przykłady list sieci

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:

In Spice format, the netlist is as follows:

:experimental:

[[managing-symbol-libraries]]
== Managing Symbol Libraries

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

=== Tabele Bibliotek Symboli

KiCad uses a table of symbol libraries to map symbol libraries to a library nickname. Kicad uses a global symbol library table as well as a table specific to each project. To edit either symbol library table, use **Preferences** -> **Manage Symbol Libraries...**.

image::images/pl/options_symbol_lib.png[scaledwidth="80%", alt="Okno ustawień bibliotek"]

The global symbol library table contains the list of libraries that are always available regardless of the currently loaded project. The table is saved in the file `sym-lib-table` in the KiCad configuration folder. xref:../kicad/kicad.adoc#config-file-location[The location of this folder] depends on the operating system being used.

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

==== Konfiguracja początkowa

The first time the KiCad Schematic Editor is run and the global symbol table file `sym-lib-table` is not found in the KiCad configuration folder, KiCad will guide the user through setting up a new symbol library table. This process is described <<initial-configuration,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 image:images/icons/small_folder_16.png[Folder icon] button and selecting a library or clicking the image:images/icons/small_plus_16.png[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 image:images/icons/small_trash_16.png[Delete icon] button.

The image:images/icons/small_up_16.png[Up icon] and image:images/icons/small_down_16.png[Down icon] buttons move the selected library up and down in the library table. This does not affect the display order of libraries in the Symbol Library Browser, Symbol Editor, or Add Symbol tool.

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

A range of libraries can be selected by clicking the first library in the range and then kbd:[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,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-libraries,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.

[[environment-variable-substitution]]
==== Substytucja zmiennych środowiskowych

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

By default, KiCad defines several environment variables:

* `${KIPROJMOD}` points to the current project directory and cannot be modified.
* `${KICAD6_FOOTPRINT_DIR}` points to the default location of KiCad's standard footprint libraries.
* `${KICAD6_SYMBOL_DIR}` points to the default location of KiCad's standard symbol libraries.
* `${KICAD6_3DMODEL_DIR}` points to the default location of KiCad's standard 3D model libraries.
* `${KICAD6_TEMPLATE_DIR}` points to the default location of KiCad's standard template library.

`${KIPROJMOD}` cannot be redefined, but the other environment variables can be redefined and new environment variables added in the **Preferences** -> **Configure Paths...** dialog.

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

`${KIPROJMOD}` allows libraries to be stored in the project folder without having to use an absolute path in the project library table. This makes it possible to relocate projects without breaking their project library tables. One of the most powerful features of the symbol library table is environment variable substitution. This allows for definition of custom paths to where symbol libraries are stored in environment variables. Environment variable substitution is supported by using the syntax `${ENV_VAR_NAME}` in the library path.

==== Zakres stosowania

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

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

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

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

[[migrating-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 kbd:[Ctrl]-clicking or kbd:[shift]-clicking.

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

==== Remapowanie projektów z poprzednich wersji

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

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

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

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

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

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

[NOTE]
====
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.
====

:experimental:

[[symbol-editor]]
== Symbol Editor

[[general-information-about-symbol-libraries]]
=== Podstawowe informacje na temat bibliotek

A symbol is a schematic element which contains a graphical representation, electrical connections, and text fields describing the symbol. Symbols used in a schematic are stored in symbol libraries. KiCad provides a symbol editing tool that allows you to create libraries, add, delete or transfer symbols between libraries, export symbols to files, and import symbols from files. The symbol editing tool provides a simple way to manage symbols and symbol libraries.

[[symbol-library-overview]]
=== Biblioteki symboli - Przegląd

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

Symbol znajdujący się w bibliotece jest złożony z:

* Graphical items (lines, circles, arcs, text, etc.) that determine how symbol looks in a schematic.
* Pins which have both graphic properties (line, clock, inverted, low level active, etc.) and electrical properties (input, output, bidirectional, etc.) used by the Electrical Rules Check (ERC) tool.
* Pól (tekstowych) takich jak oznaczenie, wartość, nazwa footprintu potrzebna do wstawienia go na płytkę.

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

Do poprawnego tworzenia symboli wymagane jest:

* Zdefiniowanie ogólnych właściwości: czy posiada wiele części składowych.
* Defining if the symbol has an alternate body style (also known as a De Morgan representation).
* Projektowanie wyglądu (z wyjątkiem pinów) z użyciem linii, prostokątów, okręgów, wielokątów i tekstów.
* Dodanie wyprowadzeń, dokładnie określając ich projekt graficzny, nazwę oraz numer pinu, a także ich właściwości elektryczne (wejście, wyjście, trzy-stanowe, port zasilania, itp.).
* Determining if the symbol should be derived from another symbol with the same graphical design and pin definition.
* Dodanie pól w razie potrzeby (jest to opcjonalne, nazwa modułu jest wykorzystywany przez oprogramowanie PCB) i/lub określenie ich widoczności.
* Dokumentowanie składnika np. poprzez dodanie słów kluczowych i adresu dokumentacji w sieci lub na lokalnym nośniku.
* Zapisanie go do wybranej biblioteki.

[[symbol-library-editor-overview]]
=== Edytor bibliotek symboli - Przegląd

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

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

[[main-toolbar]]
==== Główny pasek menu

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

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_area_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.

|=======================================================================

[[element-toolbar]]
==== Pasek narzędzi edycji symbolu

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

[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
cursor.

|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.
|=======================================================================

[[options-toolbar]]
==== Pasek opcji

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

[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.
|=======================================================================

[[library-selection-and-maintenance]]
=== Wybór bibliotek i zarządzanie nimi

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]]
==== Wybór i zapis symbolu

[[symbol-selection]]
===== Wybór symbolu

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.

[NOTE]
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]]
===== Zapisywanie symbolu

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

To save the modified symbol in the current library, click the 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]]
=== Tworzenie symboli biblliotecznych

[[create-a-new-symbol]]
==== Tworzenie nowego symbolu

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%"]

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

image::images/pl/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]]
==== Tworzenie nowego symbolu na podstawie innego

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

* Załadować symbol który będzie użyty jako wzorcowy.
* Save a new copy of the symbol using **File** -> **Save As...**. The Save As dialog will prompt for a name for the new symbol and the library to save it in.
* Wykonać niezbędne edycje.
* Save the modified symbol.

[[symbol-properties]]
==== Właściwości symbolu

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

image::images/pl/eeschema_properties_for_symbol.png[alt="Właściwości symbolu", 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.

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

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

[[symbol-name-description-and-keywords]]
===== 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]]
===== 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/pl/eeschema_libedit_footprint.png[alt="Footprint filters", scaledwidth="70%"]

[[symbols-with-alternate-symbolic-representation]]
==== Symbole wieloczęściowe i podwójna reprezentacja

If the symbol has an alternate body style defined, one body style must be selected for editing at a time. To edit the normal representation, click the 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/pl/eeschema_libedit_select_unit.png[alt="Selecting a symbol unit", scaledwidth="80%"]

[[graphical-elements]]
=== Elementy graficzne symbolu

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

* Linie i linie łamane są definiowane poprzez punkty startowe i końcowe.
* Prostokąty są definiowane przez punkty dwóch przeciwległych narożników.
* Okręgi są definiowane przez punkt centralny i promień.
* Łuki są definiowane przez punkt początkowy i końcowy łuku oraz ich punkt centralny. Kąt rozwarcia łuku może zawierać się w przedziale 0° to 180°.

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

[[graphical-element-membership]]
==== Przynależność elementów graficznych

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

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

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

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

Głównymi właściwościami dla elementów graficznych są:

* "Line width" defines the width of the element's line in the current drawing units.
* "Fill Style" determines if the shape defined by the graphical element is to be drawn unfilled, background filled, or foreground filled.
* "Common to all units in symbol" determines if the graphical element is drawn for each unit in symbol with more than one unit per package or if the graphical element is only drawn for the current unit.
* "Common to all body styles (De Morgan)" determines if the graphical element is drawn for each symbolic representation in symbols with an alternate body style or if the graphical element is only drawn for the current body style.

[[graphical-text-elements]]
==== Tekst jako grafika w symbolu

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]]
=== Symbole wieloczęściowe, podwójna reprezentacja symboli

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

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

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

[[example-of-a-symbol-with-multiple-noninterchangeable-units]]
==== 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/pl/eeschema_libedit_not_interchangeable.png[alt="Uncheck all units are interchangeable", scaledwidth="60%"]

===== Unit A

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

===== Unit B

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

===== Unit C

image::images/pl/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.

[[graphical-symbolic-elements]]
===== Elementy geometryczne w symbolach

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

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

[[pin-creation-and-editing]]
=== Tworzenie i edycja wyprowadzeń (pinów)

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.

[[pin-overview]]
==== Wyprowadzenia - Informacje podstawowe

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

Ważne uwagi:

* Symbol pins are matched to footprint pads by number. The pin number in the symbol must match the corresponding pad number in the footprint.
* Do not use spaces in pin names and numbers. Spaces will be automatically replaced with underscores (`_`).
* To define a pin name with an inverted signal (overline) use the `~` (tilde) character followed by the text to invert in braces. For example `~{FO}O` would display [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.

[[pin-properties]]
==== Właściwości wyprowadzeń

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

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

* The pin name and text size.
* The pin number and text size.
* The pin length.
* The pin electrical type and graphical style.
* Przynależność do części i alternatywnej reprezentacji.
* Pin visibility.
* <<alternate-pin-definitions,Alternate pin definitions>>.

[[pin-graphic-styles]]
==== 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/pl/eeschema_libedit_pin_properties_style.png[alt="Pin graphic styles", scaledwidth="95%"]

[[pin-electrical-types]]
==== Typy elektryczne

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

[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
concerns.
| 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
output.
| 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]]
==== 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/pl/eeschema_libedit_pin_context_menu.png[alt="Pin context menu", scaledwidth="60%"]

[[defining-pins-for-multiple-units-and-alternate-symbolic-representations]]
==== Określanie pinów w symbolach wieloczęściowych i podwójna reprezentacja

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

The symbol library editor allows the simultaneous creation of pins. By default, changes made to a pin are made for all units of a multiple unit symbol and to both representations for symbols with an alternate symbolic representation. The only exception to this is the pin's graphical type and name, which remain unlinked between symbol units and body styles. This dependency was established to allow for easier pin creation and editing in most cases. This dependency can be disabled by toggling the 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]]
==== 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]]
==== 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]]
=== Pola symboli

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

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

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]]
==== Edycja pól symboli

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

image::images/pl/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.

Ważne uwagi:

* Modifying the `Value` field changes the name of the symbol. The symbol's name in the library will change when the symbol is saved.
* The Symbol Properties dialog must be used to edit a field that is empty or has the invisible attribute enabled because such fields cannot be clicked on.
* The footprint is defined as an absolute footprint using the `LIBNAME:FOOTPRINTNAME` format where `LIBNAME` is the name of the footprint library defined in the footprint library table (see the "Footprint Library Table" section in the PCB Editor manual) and `FOOTPRINTNAME` is the name of the footprint in the library `LIBNAME`.

[[creating-power-ports]]
=== Creating Power Port Symbols

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

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


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

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

Power port symbols consist of a pin of type "Power input" that is marked invisible. <<hidden-power-pins,Invisible power input pins>> have a special property of making implicit connections based on the pin name. 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%"]

By utworzyć port zasilania, należy wykonać następujące kroki:

* Add a pin of type "Power input", with "Visible" unchecked, and the pin named according to the desired net. Make the pin number `1`, the length `0`, and set the graphic style to "Line". The pin name establishes the connection to the net; in this case the pin will automatically connect to the net `GND`. The pin number, length, and line style do not matter electrically.
* Place the pin on the symbol anchor.
* Use the shape tools to draw the symbol graphics.
* Set the symbol value. The symbol value does not matter electrically, but it is displayed in the schematic. To eliminate confusion, it should match the pin name (which determines the connected net name).
* Check the "Define as power symbol" box in Symbol Properties window. This makes the symbol appear in the "Add Power Port" dialog, makes the `Value` field read-only in the schematic, prevents the symbol from being assigned a footprint, and excludes the symbol from the board, BOM, and netlists.
* Set the symbol reference and uncheck the "Show" box. The reference text is not important except for the first character, which should be `\#`. For the power port shown above, the reference could be `#GND`. Symbols with references that begin with `#` are not added to the PCB, are not included in Bill of Materials exports or netlists, and they cannot be assigned a footprint in the footprint assignment tool. If a power port's reference does not begin with `#`, the character will be inserted automatically when the annotation or footprint assignment tools are run.

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

NOTE: The connected net name is determined by the power port's *pin name*, not
      the name of the symbol. When modifying an existing power port symbol, make
      sure to rename the pin so that the new symbol connects to the appropriate
      power net.

:experimental:

[[viewlib]]
== Przeglądanie bibliotek symboli

=== Wprowadzenie

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/pl/eeschema_viewlib_choose.png[alt="Okno przeglądarki", scaledwidth="60%"]

[[viewlib---main-screen]]
=== Ekran główny

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

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

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

[[viewlib-top-toolbar]]
=== Pasek narzędzi Przeglądarki Bibliotek Symboli

Podstawowy pasek narzędzi wygląda następująco.

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

Dostępne polecenia to:

[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
list.

|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.

|image:images/toolbar_viewlib_part.png[alt="images/toolbar_viewlib_part.png",width="70%"]
|Selection of the unit for symbols that contain multiple units.

|image:images/icons/datasheet_24.png[icons/datasheet_png]
|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.
|=======================================================================

:experimental:

[[simulator]]
== Symulator ==

KiCad provides an embedded electrical circuit simulator using http://ngspice.sourceforge.net[ngspice] as the simulation engine.

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

Istnieje również kilka projektów demonstracyjnych ilustrujących możliwości symulatora. Znajdziesz je w katalogu _demos/simulation_.

=== Przypisywanie modeli

Przed uruchomieniem symulacji komponenty muszą mieć przypisany modele Spice.

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

[[sim-passive-models]] Komponenty pasywne z referencją pasującą do typu urządzenia w zapisie Spice (_R*_ dla rezystorów, _C*_ dla kondensatorów, _L*_ dla cewek indukcyjnych) będą miały przypisane modele niejawnie i będą używać pola _Wartość_ do określania ich właściwości.

[NOTE]
Należy pamiętać, że w Spice zapis 'M' oznacza mili, a 'Meg' odpowiada Mega. Jeśli wolisz użyć 'M' do wskazania prefiksu Mega, możesz o tym zdecydować w <<sim-settings,ustawieniach symulatora>>.

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

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

[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.
|====

==== Pasywne

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

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

image::images/pl/sim_model_passive.png[alt="Zakładka edytora modelu pasywnego"]

[width="90%", cols="30%a,70%a"]
|====
|Typ
|Wybór typu elementu (rezystor, kondensator lub cewka).
|Wartość
|Definiuje właściwości komponentu (rezystancja, pojemność lub indukcyjność). Wartość
może używać popularnych przedrostków jednostek Spice (wymienionych poniżej pola
wprowadzania tekstu) i powinien używać kropki jako separatora dziesiętnego. Zauważ,
że interpreter Spice nie działa poprawnie gdy przedrostki przeplatają się w wartości (np. 1k5).
|====

==== Model

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

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

image::images/pl/sim_model_subckt.png[alt="Zakładka edytora modelu półprzewodnikowego lub złożonego"]

[width="90%", cols="30%a,70%a"]
|====================
|Plik
|Ścieżka do pliku bibliotecznego Spice. Ten plik będzie używany przez symulator,
tak jak jest dodawany za pomocą dyrektywy _.include_.
|Model
|Wybrany model komponentu. Po wybraniu pliku lista jest wypełniana modelami
do wyboru.
|Typ
|Wybór typu modelu (inny układ, BJT, MOSFET lub dioda). Zwykle jest ustawiony
automatycznie po wybraniu modelu.
|====================

==== Źródła

Zakładka _Źródło_ służy do przypisania modelu źródła zasilania lub sygnału. Dostępne są dwie sekcje: _Analiza DC/AC_ oraz _Analiza czasowa_. Każdy definiuje parametry źródłowe dla odpowiedniego typu symulacji.

Opcja _Typ źródła_ jest aktywna dla wszystkich typów symulacji.

image::images/pl/sim_model_source.png[alt="Zakładka edytora modeli źródeł"]

Więcej na temat źródeł w http://ngspice.sourceforge.net/docs/ngspice-27-manual.pdf[dokumentacji ngspice], rodział 4 (Voltage and Current Sources).

[[sim-directives]]
=== Dyrektywy Spice

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

=== Symulacja

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

image::images/pl/sim_main_dialog.png[alt="Główne okno symulacji"]

Okno dialogowe posiada kilka sekcji:

* <<sim-toolbar,Pasek narzędzi>>
* <<sim-plot-panel,Panel wykresu>>
* <<sim-output-console,Konsola>>
* <<sim-signals-list,Lista sygnałów>>
* <<sim-cursors-list,Lista znaczników kursora>>
* <<sim-tune-panel,Panel strojenia>>

==== Menu

[[sim-menu-file]]
===== Menu Plik
[width="90%", cols="30%,70%"]
|====
|Nowy wykres |Tworzy nową kartę w panelu wykresów.
|Otwórz skoroszyt |Otwiera listę kreślonych sygnałów.
|Zapisz skoroszyt |Zapisuje listę kreślonych sygnałów.
|Zapisz jako obraz |Eksportuje aktywny wykres do pliku `.png`.
|Zapisz jako plik `.csv` |Eksportuje aktywne punkty danych surowych wykresu do pliku `.csv`.
|Wyjdź z symulacji |Zamyka okno dialogowe.
|====

[[sim-menu-simulation]]
===== Symulacja
[width="90%", cols="30%,70%"]
|====
|Uruchom symulację | Wykonuje symulację przy użyciu bieżących ustawień.
|Dodaj sygnały... | Otwiera okno dialogowe wyboru sygnałów do kreślenia.
|Sondy ze schematu | Uruchamia <<sim-probe-tool, narzędzie typu Sonda>>.
|Dostrój wartość komponentu | Uruchom narzędzie <<sim-tuner-tool,Tuner>>.
|Pokaż listę sieci SPICE... | Otwiera okno dialogowe pokazujące wygenerowaną
listę sieci symulowanego obwodu.
|Ustawienia... | Otwiera <<sim-settings, okno dialogowe ustawień symulacji>>.
|====

[[sim-menu-view]]
===== Menu Widok
[width="90%", cols="30%,70%"]
|====
|Powiększ | Powiększa aktywny wykres.
|Pomniejsz | Zmniejsza aktywny wykres.
|Dopasuj do ekranu | Dostosuj ustawienie powiększenia, aby wyświetlić wszystkie wykresy.
|Pokaż siatkę | Włącza widoczność siatki.
|Pokaż legendę | Przełącz widoczność legendy wykresu.
|====

[[sim-toolbar]]
==== Pasek narzędziowy
image::images/pl/sim_main_toolbar.png[alt="Pasek narzędziowy symulatora"]
Ten pasek umożliwia dostęp do głównych funkcji symulatora.

[width="90%", cols="30%,70%"]
|====
|Uruchom/Zatrzymaj symulację | Uruchamia lub zatrzymuje symulację.
|Dodaj sygnały | Otwiera okno dialogowe wyboru sygnałów do wykreślenia.
|Sonda | Uruchamia <<sim-probe-tool,narzędzie Sonda>>.
|Dostrajanie | Uruchamia narzędzie <<sim-tuner-tool,do dostrajania>>.
|Ustawienia | Otwiera <<sim-settings,okno dialogowe ustawień symulacji>>.
|====

[[sim-plot-panel]]
==== Panel wykresu
Pokazuje wyniki symulacji w formie wykresów. W oddzielnych zakładkach można otworzyć wiele wykresów, ale tylko aktywny jest aktualizowany podczas przeprowadzania symulacji. W ten sposób można porównać wyniki symulacji dla różnych przebiegów.

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

Interakcje w panelu wykresu:

* kółko myszy służy do przybliżania/oddalania
* kliknięcie prawym przyciskiem myszy otwiera menu kontekstowe w celu dostosowania widoku
* zaznaczenie prostokątnego wyboru pozwala powiększyć wybrany obszar
* przeciągnięcie kursora zmienia jego położenie

[[sim-output-console]]
==== Konsola wyjściowa
Konsola wyjścia wyświetla komunikaty z symulatora. Zaleca się sprawdzanie konsoli, aby mieć pewność że nie ma błędów ani ostrzeżeń.

[[sim-signals-list]]
==== Lista sygnałów
Pokazuje listę sygnałów pokazywanych w aktywnym wykresie.

Interakcje na liście sygnałów:

* kliknięcie prawym przyciskiem myszy otwiera menu kontekstowe w celu ukrycia sygnału lub przełączenia krusora
* podwójne kliknięcie ukrywa sygnał

[[sim-cursors-list]]
==== Lista kursorów
Wyświetla listę kursorów i ich współrzędne. Każdy sygnał może mieć wyświetlany jeden kursor. Widoczność kursorów ustawiana jest za pomocą listy <<sim-signals-list,sygnałów>>.

[[sim-tune-panel]]
==== Panel dostrajania
Wyświetla komponenty pobrane za pomocą narzędzia <<sim-tuner-tool,Dostrajanie>>. Panel dostrajania pozwala użytkownikowi szybko modyfikować wartości komponentów i obserwować ich wpływ na wyniki symulacji - za każdym razem, gdy wartość składnika jest zmieniana, symulacja jest ponownie uruchamiana, a wykresy są aktualizowane.

Z każdym komponentem jest powiązane kilka kontrolek:

* Górne pole tekstowe określa maksymalną wartość komponentu.
* Środkowe pole tekstowe określa aktualną wartość komponentu.
* Dolne pole tekstowe określa minimalną wartość komponentu.
* Suwak pozwala użytkownikowi modyfikować wartość komponentu w sposób płynny.
* Przycisk _Zapisz_ modyfikuje wartość komponentu na schemacie do tej wybranej za pomocą suwaka.
* Przycisk _X_ usuwa komponent z panelu Dostrajanie i przywraca jego oryginalną wartość.

Trzy pola tekstowe rozpoznają przedrostki jednostek używanych przez Spice.

[[sim-tuner-tool]]
==== Narzędzie Dostrajanie
Narzędzie dostrajania pozwala użytkownikowi na wybór komponentu, którego wartość chce dostroić.

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

[[sim-probe-tool]]
==== Narzędzie Sonda
Narzędzie Sonda zapewnia przyjazny dla użytkownika sposób wyboru sygnałów w celu umieszczenia ich na wykresie.

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

[[sim-settings]]
==== Ustawienia symulacji

image::images/pl/sim_settings.png[alt="Okno dialogowe ustawień symulatora"]

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

* AC
* Przenoszenie DC
* Analiza czasowa
* Własne

Pierwsze trzy zakładki zawierają formularze w których można określić parametry symulacji. Ostatnia zakładka umożliwia użytkownikowi wpisanie również niestandardowych dyrektyw Spice. Więcej informacji o typach i parametrach symulacji można znaleźć w http://ngspice.sourceforge.net/docs/ngspice-27-manual.pdf[dokumentacji ngspice], rozdział 1.2.

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

Istnieją dwie opcje wspólne dla wszystkich typów symulacji:
[width="90%", cols="30%,70%"]
|====
|Dostosuj wartości symboli pasywnych | Zastąp wartości symboli pasywnych by dokonać
często wykonywanej konwersji wartości do ich notacji w Spice.
|Dodaj pełną ścieżkę do dyrektyw _.include_ wprowadzające nowe biblioteki | Łączy nazwy
plików bibliotek modeli Spice z pełną ścieżką dostępu. Normalnie, pełna ścieżka jest wymagana
przez ngspice by mógł uzyskać dostęp do pliku biblioteki.
|====

:experimental:

[[advanced]]
== Advanced Topics

[[color-settings]]
[[configuration-and-customization]]
=== Configuration and Customization

NOTE: TODO: write this section

[[text-variables]]
=== Text variables

NOTE: TODO: write this section


=== Database Libraries

A database library is a type of KiCad symbol library that holds data about parts in an external SQL database. Database libraries do not contain any symbol or footprint definitions by themselves. Instead, they **reference** symbols and footprints found in other KiCad libraries. Each database library entry maps a KiCad symbol (from another library) to a set of properties (fields) and usually a KiCad footprint (from a footprint library).

Using database libraries allows you to create fully-defined parts (sometimes called *atomic parts*) out of KiCad symbols and footprints without needing to store all the part properties in a symbol library. The external database can be linked to third-party tools for managing part data and lifecycles. Database library workflows are generally more complex than the standard KiCad library workflows, and so this type of library is typically only used in situations where it makes managing a large library of fully-defined parts more efficient (such as in organization or team settings).

KiCad does not provide a GUI for editing a SQL database or defining a database library. It is up to the user to find the most appropriate workflow and toolchain for creating and updating the database itself. Some users may want to directly edit the database through a third-party database client, and some may use other third-party software such as a part lifecycle management (PLM) tool to create and edit data.

In a database library, there are one or more **tables** that generally represent a single type of part (such as Resistors or Capacitors). Each table can have an independent schema, meaning that different types of parts can have different properties that are translated into symbol fields in KiCad. Each table must have a unique ID column which is used as the identifier for a symbol placed from that table. This unique ID will typically be a part number (either a manufacturer's part number, or an internal organization part number). Each table must also have a column that contains a mapping to a KiCad symbol, in the form `LibraryNickname:SymbolName`. The `LibraryNickname` must match a symbol library that is present in the KiCad library tables. Tables may also contain a column containing a KiCad footprint, in the form `LibraryNickname:FootprintName`. If this column is present, symbols placed from the table will include a footprint mapping.

Tables may also contain arbitrary additional columns that may optionally be mapped to symbol fields in KiCad. The KiCad database library configuration file controls how these fields should be named, whether or not to make the fields visible, and whether or not to include the fields in the data displayed in the Symbol Chooser.

==== Database Library Configuration Files

To create a database library, you must create a configuration file that contains the necessary information for KiCad to connect to your database and retrieve data from tables. Copy the template below into a new file and save it with a `kicad_dbl` extension. You can then add this file to your global symbol library table using the Configure Symbol Libraries dialog.

```json
{
    "meta": {
        "version": 0
    },
    "name": "My Database Library",
    "description": "A database of components",
    "source": {
        "type": "odbc",
        "dsn": "",
        "username": "",
        "password": "",
        "timeout_seconds": 2,
        "connection_string": ""
    },
    "libraries": [
        {
            "name": "Resistors",
            "table": "Resistors",
            "key": "Part ID",
            "symbols": "Symbols",
            "footprints": "Footprints",
            "fields": [
                {
                    "column": "MPN",
                    "name": "MPN",
                    "visible_on_add": false,
                    "visible_in_chooser": true,
                    "show_name": true,
                    "inherit_properties": true
                },
                {
                    "column": "Value",
                    "name": "Value",
                    "visible_on_add": true,
                    "visible_in_chooser": true,
                    "show_name": false
                }
            ],
            "properties": {
                "description": "Description",
                "footprint_filters": "Footprint Filters",
                "keywords": "Keywords",
                "exclude_from_bom": "No BOM",
                "exclude_from_board": "Schematic Only"
            }
        }
    ]
}

 ...  ```">[[the-header-section]]
===== Sekcja nagłówka

The header has the delimiter `<design>`

```xml <design> <source>F:\kicad_aux\netlist_test\netlist_test.sch</source> <date>21/08/2010 08:12:08</date> <tool>eeschema (2010-08-09 BZR 2439)-unstable</tool> </design> ```

Sekcja ta może być widoczna jako komentarze.

[[the-components-section]]
===== Sekcja komponentów

The component section has the delimiter `<components>`

```xml <components> <comp ref="P1"> <value>CONN_4</value> <libsource lib="conn" part="CONN_4"/> <sheetpath names="/" tstamps="/"/> <tstamps>4C6E2141</tstamps> </comp> </components> ``` This section contains the list of components in your schematic. Each component is described like this:

```xml <comp ref="P1"> <value>CONN_4</value> <libsource lib="conn" part="CONN_4"/> <sheetpath names="/" tstamps="/"/> <tstamps>4C6E2141</tstamps> </comp> ```

[width="100%", cols="37%,63%"]
|=======================================================================
|Element name |Element description

|`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` |timestamp of the component.
|=======================================================================

[[note-about-time-stamps-for-components]]
====== Note about time stamps for components

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

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

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

[[the-libparts-section]]
===== Sekcja elementów bibliotecznych

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

```xml
<libparts>
<libpart lib="device" part="CP">
  <description>Condensateur polarise</description>
  <footprints>
    <fp>CP*</fp>
    <fp>SM*</fp>
  </footprints>
  <fields>
    <field name="Reference">C</field>
    <field name="Valeur">CP</field>
  </fields>
  <pins>
    <pin num="1" name="1" type="passive"/>
    <pin num="2" name="2" type="passive"/>
  </pins>
</libpart>
</libparts>

<libraries>
  <library logical="device">
    <uri>F:\kicad\share\library\device.lib</uri>
  </library>
  <library logical="conn">
    <uri>F:\kicad\share\library\conn.lib</uri>
  </library>
</libraries>

<nets>
  <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>
  <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>
</nets>

<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>

<?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:
        https://lists.launchpad.net/kicad-developers/msg05157.html
-->

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

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

<xsl:template match="/export">
    <xsl:text>*PADS-PCB*&nl;*PART*&nl;</xsl:text>
    <xsl:apply-templates select="components/comp"/>
    <xsl:text>&nl;*NET*&nl;</xsl:text>
    <xsl:apply-templates select="nets/net"/>
    <xsl:text>*END*&nl;</xsl:text>
</xsl:template>

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

<!-- 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:choose>
            <xsl:when test = "@name != '' ">
                <xsl:value-of select="@name"/>
            </xsl:when>
            <xsl:otherwise>
                <xsl:text>N-</xsl:text>
                <xsl:value-of select="@code"/>
            </xsl:otherwise>
        </xsl:choose>
        <xsl:text>&nl;</xsl:text>
        <xsl:apply-templates select="node"/>
    </xsl:if>
</xsl:template>

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

</xsl:stylesheet> ```

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

``` *PADS-PCB* *PART* P1 unknown U2 unknown U1 unknown C1 unknown R1 unknown *NET* *SIGNAL* GND U1.7 C1.2 U2.7 P1.4 *SIGNAL* VCC R1.1 U1.14 U2.4 U2.1 U2.14 P1.1 *SIGNAL* N-4 U1.2 U2.3 *SIGNAL* /SIG_OUT P1.2 U2.5 U2.2 *SIGNAL* /CLOCK_IN R1.2 C1.1 U1.1 P1.3

*END*

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

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

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

<!-- Netlist header -->
<xsl:template match="/export">
    <xsl:text>.HEA&nl;</xsl:text>
    <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:text>&nl;&nl;</xsl:text>
    <xsl:apply-templates select="nets/net"/>          <!-- Generate list of nets and connections -->
    <xsl:text>&nl;.END&nl;</xsl:text>
</xsl:template>

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

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

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

<!-- 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:text>"</xsl:text>
        <xsl:choose>
            <xsl:when test = "@name != '' ">
                <xsl:value-of select="@name"/>
            </xsl:when>
            <xsl:otherwise>
                <xsl:text>N-</xsl:text>
                <xsl:value-of select="@code"/>
        </xsl:otherwise>
        </xsl:choose>
        <xsl:text>"&nl;</xsl:text>
        </xsl:variable>
        <xsl:apply-templates select="node" mode="first"/>
        <xsl:value-of select="$netname"/>
        <xsl:apply-templates select="node" mode="others"/>
    </xsl:if>
</xsl:template>

<!-- 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:text>.</xsl:text>
    <xsl:value-of select="@pin"/>
    <xsl:text> </xsl:text>
    </xsl:if>
</xsl:template>

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

</xsl:stylesheet> ```

Poniżej znajduje się plik wyjściowy dla programu Cadstar.

===== OrcadPCB2 netlist example using XSLT

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

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

```xml
<?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:
        https://lists.launchpad.net/kicad-developers/msg05157.html
-->

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

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

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

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

<!-- end of file --> <xsl:text>)&nl;*&nl;</xsl:text> </xsl:template>

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

<!--
    Generate date in header like "20/08/2010 10:45:33"
-->
<xsl:template match="date">
    <xsl:apply-templates/>
    <xsl:text>&nl;</xsl:text>
</xsl:template>

<!--
    This template read each component
    (path = /export/components/comp)
    creates lines:
     ( 3EBF7DBD $noname U1 74LS125
      ... pin list ...
)
and calls "create_pin_list" template to build the pin list
-->
<xsl:template match="comp">
    <xsl:text> ( </xsl:text>
    <xsl:choose>
        <xsl:when test = "tstamp != '' ">
            <xsl:apply-templates select="tstamp"/>
        </xsl:when>
        <xsl:otherwise>
            <xsl:text>00000000</xsl:text>
        </xsl:otherwise>
    </xsl:choose>
    <xsl:text> </xsl:text>
    <xsl:choose>
        <xsl:when test = "footprint != '' ">
            <xsl:apply-templates select="footprint"/>
        </xsl:when>
        <xsl:otherwise>
            <xsl:text>$noname</xsl:text>
        </xsl:otherwise>
    </xsl:choose>
    <xsl:text> </xsl:text>
    <xsl:value-of select="@ref"/>
    <xsl:text> </xsl:text>
    <xsl:choose>
        <xsl:when test = "value != '' ">
            <xsl:apply-templates select="value"/>
        </xsl:when>
        <xsl:otherwise>
            <xsl:text>"~"</xsl:text>
        </xsl:otherwise>
    </xsl:choose>
    <xsl:text>&nl;</xsl:text>
    <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:call-template>
    <xsl:text> )&nl;</xsl:text>
</xsl:template>

<!--
    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"/>
                </xsl:apply-templates>
            </xsl:if>
        </xsl:for-each>
</xsl:template>


<!--
    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
          <pins>
            <pin num="1" type="passive"/>
            <pin num="2" type="passive"/>
          </pins>
    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"/>
            </xsl:with-param>
        </xsl:apply-templates>
    </xsl:for-each>

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

<!--
    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
      <nets>
        <net code="1" name="GND">
          <node ref="J1" pin="20"/>
              <node ref="C2" pin="2"/>
        </net>
        <net code="2" name="">
          <node ref="U2" pin="11"/>
        </net>
    </nets>
    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">
                <xsl:choose>
                    <!-- 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:when>
                    <xsl:otherwise>
                        <xsl:text>$N-0</xsl:text><xsl:value-of select="../@code"/>
                    </xsl:otherwise>
                </xsl:choose>
            </xsl:if>
            <xsl:if test = "$pin_cnt_in_net &lt;2">
                <xsl:text>?</xsl:text>
            </xsl:if>
        </xsl:if>
    </xsl:if>

</xsl:template>

</xsl:stylesheet> ```

Poniżej znajduje się plik wyjściowy programu OrcadPCB2.

:experimental:

[[eeschema-actions-reference]]
== Actions reference
Below is a list of every available *action* in the KiCad Schematic Editor: a command that can be assigned to a hotkey.


=== Schematic Editor

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

[width="100%", options="header", cols="20%,15%,65%"]
|===
| Action | Default Hotkey | Description
| Align Elements to Grid
  |
  |
| Annotate Schematic...
  |
  | Fill in schematic symbol reference designators
| Assign Footprints...
  |
  | Run footprint assignment tool
| Clear Net Highlighting
  | kbd:[~]
  | Clear any existing net highlighting
| Export Drawing to Clipboard
  |
  | Export drawing of current sheet to clipboard
| Edit Library Symbol...
  | kbd:[Ctrl+Shift+E]
  | Open the library symbol in the Symbol Editor
| Edit Sheet Page Number...
  |
  | Edit the page number of the current or selected sheet
| Edit Symbol Fields...
  |
  | Bulk-edit fields of all symbols in schematic
| Edit Symbol Library Links...
  |
  | Edit links between schematic and library symbols
| Edit with Symbol Editor
  | kbd:[Ctrl+E]
  | Open the selected symbol in the Symbol Editor
| Highlight on PCB
  |
  | Highlight corresponding items in PCB editor
| Export Netlist...
  |
  | Export file containing netlist in one of several formats
| Force H/V Wires and Buses
  |
  | Switch H & V only mode for new wires and buses
| Generate BOM...
  |
  | Generate a bill of materials for the current schematic
| Highlight Net
  | kbd:[`]
  | Highlight net under cursor
| Highlight Nets
  |
  | Highlight wires and pins of a net
| Import Footprint Assignments...
  |
  | Import symbol footprint assignments from .cmp file created by Pcbnew
| Remap Legacy Library Symbols...
  |
  | Remap library symbol references in legacy schematics to the symbol library table
| Repair Schematic
  |
  | Run various diagnostics and attempt to repair schematic
| Rescue Symbols...
  |
  | Find old symbols in project and rename/rescue them
| Simulator...
  |
  | Simulate circuit in SPICE
| Save Current Sheet Copy As...
  |
  | Save a copy of the current sheet to another location or name
| Schematic Setup...
  |
  | Edit schematic setup including annotation styles and electrical rules
| Bus Definitions...
  |
  | Manage bus definitions
| Show Hidden Fields
  |
  | Toggle display of hidden text fields
| Show Hidden Pins
  |
  | Toggle display of hidden pins
| Switch to PCB Editor
  |
  | Open PCB in board editor
| Scripting Console
  |
  | Show the Python scripting console
| Symbol Checker
  |
  | Show the symbol checker window
| Electrical Rules Checker
  |
  | Perform electrical rules check
| Show Datasheet
  | kbd:[D]
  | Opens the datasheet in a browser
| Add Sheet
  | kbd:[S]
  | Add a hierarchical sheet
| Finish Sheet
  |
  | Finish drawing sheet
| Import Sheet Pin
  |
  | Import a hierarchical sheet pin
| Import Sheet Pin
  |
  | Import a hierarchical sheet pin
| Add Wire to Bus Entry
  | kbd:[Z]
  | Add a wire entry to a bus
| Add Global Label
  | kbd:[Ctrl+L]
  | Add a global label
| Add Hierarchical Label
  | kbd:[H]
  | Add a hierarchical label
| Add Image
  |
  | Add bitmap image
| Add Junction
  | kbd:[J]
  | Add a junction
| Add Label
  | kbd:[L]
  | Add a net label
| Add No Connect Flag
  | kbd:[Q]
  | Add a no-connection flag
| Add Power
  | kbd:[P]
  | Add a power port
| Add Text
  | kbd:[T]
  | Add text
| Add Symbol
  | kbd:[A]
  | Add a symbol
| Add Junctions to Selection where needed
  |
  |
| Add Bus
  | kbd:[B]
  | Add a bus
| Add Lines
  | kbd:[I]
  | Add connected graphic lines
| Add Wire
  | kbd:[W]
  | Add a wire
| Finish Wire or Bus
  | kbd:[K]
  | Complete drawing at current segment
| Finish Bus
  |
  | Complete bus with current segment
| Finish Lines
  |
  | Complete connected lines with current segment
| Finish Wire
  |
  | Complete wire with current segment
| Unfold from Bus
  | kbd:[C]
  | Break a wire out of a bus
| Assign Netclass...
  |
  | Assign a netclass to the net of the selected wire
| Autoplace Fields
  | kbd:[O]
  | Runs the automatic placement algorithm on the symbol or sheet's fields
| Break Bus
  |
  | Divide a bus into segments which can be dragged independently
| Break Wire
  |
  | Divide a wire into segments which can be dragged independently
| Change Symbol...
  |
  | Assign a different symbol from the library
| Change Symbols...
  |
  | Assign different symbols from the library
| Cleanup Sheet Pins
  |
  | Delete unreferenced sheet pins
| Edit Footprint…
  | kbd:[F]
  | Displays footprint field dialog
| Edit Reference Designator...
  | kbd:[U]
  | Displays reference designator dialog
| Edit Text & Graphics Properties...
  |
  | Edit text and graphics properties globally across schematic
| Edit Value…
  | kbd:[V]
  | Displays value field dialog
| Mirror Horizontally
  | kbd:[X]
  | Flips selected item(s) from left to right
| Mirror Vertically
  | kbd:[Y]
  | Flips selected item(s) from top to bottom
| Pin Table...
  |
  | Displays pin table for bulk editing of pins
| Properties…
  | kbd:[E]
  | Displays item properties dialog
| Repeat Last Item
  | kbd:[Ins]
  | Duplicates the last drawn item
| Rotate Counterclockwise
  | kbd:[R]
  | Rotates selected item(s) counter-clockwise
| Rotate Clockwise
  |
  | Rotates selected item(s) clockwise
| De Morgan Alternate
  |
  | Switch to alternate De Morgan representation
| De Morgan Standard
  |
  | Switch to standard De Morgan representation
| Symbol Properties...
  |
  | Displays symbol properties dialog
| Change to Global Label
  |
  | Change existing item to a global label
| Change to Hierarchical Label
  |
  | Change existing item to a hierarchical label
| Change to Label
  |
  | Change existing item to a label
| Change to Text
  |
  | Change existing item to a text comment
| De Morgan Conversion
  |
  | Switch between De Morgan representations
| Update Symbol...
  |
  | Update symbol to include any changes from the library
| Update Symbols from Library...
  |
  | Update symbols to include any changes from the library
| Move Activate
  |
  |
| Drag
  | kbd:[G]
  | Drags the selected item(s)
| Move
  | kbd:[M]
  | Moves the selected item(s)
| Select Connection
  | kbd:[Alt+4]
  | Select a complete connection
| Select Node
  | kbd:[Alt+3]
  | Select a connection item under the cursor
| Enter Sheet
  |
  | Display the selected sheet's contents in the schematic editor
| Navigate to page
  |
  | Navigate to page
| Leave Sheet
  | kbd:[Alt+Back]
  | Display the parent sheet in the schematic editor
| Hierarchy Navigator
  |
  | Show schematic sheet hierarchy
| Push Pin Length
  |
  | Copy pin length to other pins in symbol
| Push Pin Name Size
  |
  | Copy pin name size to other pins in symbol
| Push Pin Number Size
  |
  | Copy pin number size to other pins in symbol
| Create Corner
  |
  | Create a corner
| Remove Corner
  |
  | Remove corner
| Add a simulator probe
  |
  |
| Select a value to be tuned
  |
  |
| Add Arc
  |
  | Add an arc
| Add Circle
  |
  | Add a circle
| Add Lines
  |
  | Add connected graphic lines
| Add Rectangle
  |
  | Add a rectangle
| Finish Drawing
  |
  | Finish drawing shape
| Move Symbol Anchor
  |
  | Specify a new location for the symbol anchor
| Add Pin
  | kbd:[P]
  | Add a pin
| Add Text
  |
  | Add a text item
| Add Symbol to Schematic
  |
  | Add Symbol to Schematic
| Copy
  |
  |
| Cut
  |
  |
| Delete Symbol
  |
  | Remove the selected symbol from its library
| Duplicate Symbol
  |
  | Make a copy of the selected symbol
| Edit Symbol
  |
  | Show selected symbol on editor canvas
| Export…
  |
  | Export a symbol to a new library file
| Export Symbol as SVG…
  |
  | Create SVG file from the current symbol
| Export View as PNG…
  |
  | Create PNG file from the current view
| Hide Symbol Tree
  |
  |
| Import Symbol...
  |
  | Import a symbol to the current library
| New Symbol...
  | kbd:[N]
  | Create a new symbol
| Paste Symbol
  |
  |
| Save Library As...
  | kbd:[Ctrl+Shift+S]
  | Save the current library to a new file.
| Save As…
  |
  | Save the current symbol to a different library.
| Show Pin Electrical Types
  |
  | Annotate pins with their electrical types
| Show Symbol Tree
  |
  |
| Synchronized Pins Edit Mode
  |
  | Synchronized Pins Edit Mode
When enabled propagates all changes (except pin numbers) to other units.
Enabled by default for multiunit parts with interchangeable units.
| Update Symbol Fields...
  |
  | Update symbol to match changes made in parent symbol
| Symbol Move Activate
  |
  |
|===

=== Common

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

[width="100%", options="header", cols="20%,15%,65%"]
|===
| Action | Default Hotkey | Description
| Exclude Marker
  |
  | Mark current violation in Checker window as an exclusion
| Next Marker
  |
  | Go to next marker in Checker window
| Previous Marker
  |
  | Go to previous marker in Checker window
| Add Library…
  |
  | Add an existing library folder
| Click
  | kbd:[Return]
  | Performs left mouse button click
| Double-click
  | kbd:[End]
  | Performs left mouse button double-click
| Cursor Down
  | kbd:[Down]
  |
| Cursor Down Fast
  | kbd:[Ctrl+Down]
  |
| Cursor Left
  | kbd:[Left]
  |
| Cursor Left Fast
  | kbd:[Ctrl+Left]
  |
| Cursor Right
  | kbd:[Right]
  |
| Cursor Right Fast
  | kbd:[Ctrl+Right]
  |
| Cursor Up
  | kbd:[Up]
  |
| Cursor Up Fast
  | kbd:[Ctrl+Up]
  |
| Switch to Fast Grid 1
  | kbd:[Alt+1]
  |
| Switch to Fast Grid 2
  | kbd:[Alt+2]
  |
| Switch to Next Grid
  | kbd:[N]
  |
| Switch to Previous Grid
  | kbd:[Shift+N]
  |
| Grid Properties...
  |
  | Set grid dimensions
| Reset Grid Origin
  | kbd:[Z]
  |
| Grid Origin
  | kbd:[S]
  | Set the grid origin point
| Inactive Layer View Mode
  |
  | Toggle inactive layers between normal and dimmed
| Inactive Layer View Mode (3-state)
  | kbd:[H]
  | Cycle inactive layers between normal, dimmed, and hidden
| Inches
  |
  | Use inches
| Millimeters
  |
  | Use millimeters
| Mils
  |
  | Use mils
| New...
  | kbd:[Ctrl+N]
  | Create a new document in the editor
| New Library…
  |
  | Create a new library folder
| Open...
  | kbd:[Ctrl+O]
  | Open existing document
| Page Settings...
  |
  | Settings for paper size and title block info
| Pan Down
  | kbd:[Shift+Down]
  |
| Pan Left
  | kbd:[Shift+Left]
  |
| Pan Right
  | kbd:[Shift+Right]
  |
| Pan Up
  | kbd:[Shift+Up]
  |
| Pin Library
  |
  | Keep the library at the top of the list
| Plot...
  |
  | Plot
| Print...
  | kbd:[Ctrl+P]
  | Print
| Quit
  |
  | Close the current editor
| Reset Local Coordinates
  | kbd:[Space]
  |
| Revert
  |
  | Throw away changes
| Save
  | kbd:[Ctrl+S]
  | Save changes
| Save All
  |
  | Save all changes
| Save As…
  | kbd:[Ctrl+Shift+S]
  | Save current document to another location
| Save Copy As...
  |
  | Save a copy of the current document to another location
| 3D Viewer
  | kbd:[Alt+3]
  | Show 3D viewer window
| Show Context Menu
  |
  | Perform the right-mouse-button action
| Footprint Library Browser
  |
  | Browse footprint libraries
| Footprint Editor
  |
  | Create, delete and edit footprints
| Symbol Library Browser
  |
  | Browse symbol libraries
| Symbol Editor
  |
  | Create, delete and edit symbols
| Always Show Cursor
  | kbd:[Ctrl+Shift+X]
  | Display crosshairs even in selection tool
| Full-Window Crosshairs
  |
  | Switch display of full-window crosshairs
| Show Grid
  |
  | Display grid dots or lines in the edit window
| Polar Coordinates
  |
  | Switch between polar and cartesian coordinate systems
| Switch units
  | kbd:[Ctrl+U]
  | Switch between imperial and metric units
| Unpin Library
  |
  | No longer keep the library at the top of the list
| Update PCB from Schematic…
  | kbd:[F8]
  | Update PCB with changes made to schematic
| Update Schematic from PCB...
  |
  | Update schematic with changes made to PCB
| Center
  | kbd:[F4]
  | Center
| Zoom to Objects
  | kbd:[Ctrl+Home]
  | Zoom to Objects
| Zoom to Fit
  | kbd:[Home]
  | Zoom to Fit
| Zoom In at Cursor
  | kbd:[F1]
  | Zoom In at Cursor
| Zoom In
  |
  | Zoom In
| Zoom Out at Cursor
  | kbd:[F2]
  | Zoom Out at Cursor
| Zoom Out
  |
  | Zoom Out
| Refresh
  | kbd:[F5]
  | Refresh
| Zoom to Selection
  | kbd:[Ctrl+F5]
  | Zoom to Selection
| Cancel
  |
  | Cancel current tool
| Change Edit Method
  | kbd:[Ctrl+Space]
  | Change edit method constraints
| Copy
  | kbd:[Ctrl+C]
  | Copy selected item(s) to clipboard
| Cut
  | kbd:[Ctrl+X]
  | Cut selected item(s) to clipboard
| Delete
  | kbd:[Del]
  | Deletes selected item(s)
| Interactive Delete Tool
  |
  | Delete clicked items
| Duplicate
  | kbd:[Ctrl+D]
  | Duplicates the selected item(s)
| Find
  | kbd:[Ctrl+F]
  | Find text
| Find and Replace
  | kbd:[Ctrl+Alt+F]
  | Find and replace text
| Find Next
  | kbd:[F3]
  | Find next match
| Find Next Marker
  | kbd:[Shift+F3]
  |
| Paste
  | kbd:[Ctrl+V]
  | Paste item(s) from clipboard
| Paste Special...
  |
  | Paste item(s) from clipboard with options
| Redo
  | kbd:[Ctrl+Y]
  | Redo last edit
| Replace All
  |
  | Replace all matches
| Replace and Find Next
  |
  | Replace current match and find next
| Select All
  | kbd:[Ctrl+A]
  | Select all items on screen
| Undo
  | kbd:[Ctrl+Z]
  | Undo last edit
| Measure Tool
  | kbd:[Ctrl+Shift+M]
  | Interactively measure distance between points
| Select item(s)
  |
  | Select item(s)
| Configure Paths…
  |
  | Edit path configuration environment variables
| Donate
  |
  | Open "Donate to KiCad" in a web browser
| Get Involved
  |
  | Open "Contribute to KiCad" in a web browser
| Getting Started with KiCad
  |
  | Open “Getting Started in KiCad” guide for beginners
| Help
  |
  | Open product documentation in a web browser
| List Hotkeys...
  | kbd:[Ctrl+F1]
  | Displays current hotkeys table and corresponding commands
| Preferences...
  | kbd:[Ctrl+,]
  | Show preferences for all open tools
| Report Bug
  |
  | Report a problem with KiCad
| Manage Footprint Libraries...
  |
  | Edit the global and project footprint library lists
| Manage Symbol Libraries…
  |
  | Edit the global and project symbol library lists
|===