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

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

Some advanced filters are available:

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

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

这是放置期间的符号：

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

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

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

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

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

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

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

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

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

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

每个字段都可以是可见的或隐藏的，并且可以水平或垂直显示。 始终为正常显示的符号（无旋转或镜像）指示显示的位置，并且相对于符号的锚点。

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

A drawing sheet template file can also be selected.

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

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

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

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

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

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

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

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

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

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

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

Here you can see three errors:

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

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

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

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

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

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

单击所需的单元格方块可以更改规则，使其循环选择：正常，警告，错误。

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

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

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

The Symbol Fields Table is accessed with Tools → Edit Symbol Fields…​, or with the button on the top toolbar.

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

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

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

The top toolbar contains the following commands:

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

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

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

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

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

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

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

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

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

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

The top toolbar contains the following commands:

The left toolbar contains the following commands:

The tool has several options to control its behavior.

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…​).

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.

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.

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

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.

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

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

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

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.

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

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

The KiCad format netlist for this schematic is as follows:

In Spice format, the netlist is as follows:

The first time the KiCad Schematic Editor is run and the global symbol table file sym-lib-table is not found in the KiCad configuration folder, KiCad will guide the user through setting up a new symbol library table. This process is described above.

Symbol libraries can only be used if they have been added to either the global or project-specific symbol library table.

Add a library either by clicking the button and selecting a library or clicking the button and typing the path to a library file. The selected library will be added to the currently opened library table (Global or Project Specific). Libraries can be removed by selecting desired library entries and clicking the button.

The and buttons move the selected library up and down in the library table. This does not affect the display order of libraries in the Symbol Library Browser, Symbol Editor, or Add Symbol tool.

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

A range of libraries can be selected by clicking the first library in the range and then Shift-clicking the last library in the range.

Each library must have a unique nickname: duplicate library nicknames are not allowed in the same table. However, nicknames can be duplicated between the global and project library tables. Libraries in the project table take precedence over libraries with the same name in the global table.

Library nicknames do not have to be related to the library filename or path. The colon character (:) cannot be used in library nicknames or symbol names because it is used as a separator between nicknames and symbols.

Each library entry must have a valid path. Paths can be defined as absolute, relative, or by environment variable substitution.

The appropriate library format must be selected in order for the library to be properly read. "KiCad" format is used for KiCad version 6 libraries (.kicad_sym files), while "Legacy" format is used for libraries from older versions of KiCad (.lib files). Legacy libraries are read-only, but can be migrated to KiCad format libraries using the Migrate Libraries button (see section Migrating Legacy Libraries).

There is an optional description field to add a description of the library entry. The option field is not used at this time so adding options will have no effect when loading libraries.

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} 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.

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.

每种方法都有优点和缺点。 在全局表中定义所有库意味着它们将在需要时始终可用。 这样做的缺点是加载时间会增加。

在项目特定的基础上定义所有符号库意味着您只有项目所需的库，这会减少符号库加载时间。 缺点是您必须始终记住添加每个项目所需的每个符号库。

一种使用模式是全局定义常用库，而库只需要项目特定库表中的项目。 对如何定义库没有限制。

Legacy libraries (.lib files) are read-only, but they can be migrated to KiCad version 6 libraries (.kicad_sym). KiCad version 6 libraries cannot be viewed or edited by KiCad versions older than 6.0.0.

Legacy libraries can be converted to KiCad 6 libraries by selecting them in the symbol library table and clicking the Migrate Libraries button. Multiple libraries can be selected and migrated at once by Ctrl-clicking or shift-clicking.

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

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

The 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.

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.

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

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

There are also several graphical options.

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

将使用上面的属性创建一个新符号，它将出现在编辑器中，如下所示。

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 icon and clicking on the new desired anchor position.

通常，您要制作的符号类似于符号库中已有的符号。 在这种情况下，很容易加载和修改现有符号。

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 icon to show the dialog below.

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.

下面的示例显示了未选中 “放置引脚名称” 选项的符号。 注意名称和引脚号的位置。

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

To edit the alternate representation, click on the icon. Use the dropdown shown below to select the unit you wish to edit.

每个图形元素（线，弧，圆等）可以被定义为对于所有单元和/或主体样式是共同的或者对于给定单元和/或主体样式是特定的。 右键单击元素可以快速访问元素选项，以显示所选元素的上下文菜单。 下面是线元素的上下文菜单。

您还可以双击元素以修改其属性。 下面是多边形元素的属性对话框。

图形元素的属性是:

The 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.

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.

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.

重要笔记：

引脚属性对话框允许您编辑引脚的所有特性。 创建引脚或双击现有引脚时，会自动弹出此对话框。 此对话框允许您修改：

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.

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

You can 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.

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 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 button on the tool bar. To edit the pin number for each unit, select the appropriate unit using the drop down control.

Another way to edit pins is to use the Pin Table, which is accessible via the 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 and icons, respectively.

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

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

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

Alternate pin definitions 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.

要编辑现有符号字段，请右键单击字段文本以显示下面显示的字段上下文菜单。

To add new fields, delete optional fields, or edit existing fields, use the icon on the main tool bar to open the Symbol Properties dialog.

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

重要笔记：

无源 选项卡允许用户将无源器件模型（电阻，电容或电感）分配给元件。 这是一个很少使用的选项，因为通常被动元件的模型分配了 模拟无源模型，隐形 ，除非元件引用与实际设备类型不匹配。

Model 选项卡用于分配外部库文件中定义的半导体或复杂模型。 Spice 模型库通常由设备制造商提供。

主文本小部件显示所选的库文件内容。 将模型描述放在库文件中是常见的做法，包括节点顺序。

Source 选项卡用于分配电源或信号源模型。 有两个部分：“DC/AC 分析” 和“转换分析”。 每个都定义了相应模拟类型的源参数。

Source type 选项适用于所有模拟类型。

有关源的更多详细信息，请参阅 ngspice文档 ，第4章（电压和电流源）。

顶部工具栏提供对最常执行的操作的访问。

将模拟结果可视化为图。 可以在单独的选项卡中打开多个图，但只有在执行模拟时才会更新活动图。 这样就可以比较不同运行的模拟结果。

可以使用 “模拟菜单视图，视图” 菜单切换网格和图例可见性来自定义绘图。 当图例可见时，可以拖动它来改变其位置。

绘图面板交互：

输出控制台显示来自模拟器的消息。 建议检查控制台输出以确认没有错误或警告。

显示活动图中显示的信号列表。

信号列表交互:

显示游标列表及其坐标。 每个信号可以显示一个光标。 使用 “模拟信号列表，信号” 列表设置游标可见性。

显示使用 “模拟调谐工具，调谐“ 工具选取的元件。 调谐面板允许用户快速修改元件值并观察它们对模拟结果的影响 - 每次更改元件值时，都会重新运行模拟并更新图形。

对于每个元件，有一些控件关联：

三个文本字段识别 Spice 单元前缀。

调谐器工具允许用户选择要调整的元件。

要选择要调整的元件，请在工具处于活动状态时单击原理图编辑器中的一个元件。 所选元件将出现在 “模拟调谐工具，调谐” 面板中。 只能调整被动元件。

探针工具提供了一种用户友好的方式来选择用于绘图的信号。

要向绘图添加信号，请在工具处于活动状态时单击原理图编辑器中的相应导线。

模拟设置对话框允许用户设置模拟类型和参数。有四个选项卡：

前三个选项卡提供可以指定模拟参数的表单。 最后一个选项卡允许用户键入自定义 Spice 指令以设置模拟。 有关仿真类型和参数的更多信息，请参见 ngspice文档 ，第1.2章。

配置模拟的另一种方法是在原理图上的文本字段中键入 “模拟指令，Spice 指令”。 与模拟类型相关的任何文本字段指令都会被对话框中选择的设置覆盖。 这意味着一旦开始使用模拟对话框，该对话框将覆盖原理图指令，直到重新打开模拟器。

所有模拟类型共有两个选项：

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

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

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

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

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

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

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

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

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

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

For a netlist exporter using xsltproc, an example is:

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

For a BOM exporter using Python, an example is:

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

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

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

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

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

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

此示例提供了网表文件格式的概念。

Some example netlist exporters using XSLT are included below.

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

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