第一次运行 KiCad 原理图编辑器时，如果在 KiCad 配置文件夹中没有找到全局符号表文件 sym-lib-table，KiCad 将引导用户设置一个新的符号库表。这个过程将在 初始配置中描述。

符号库只有在它们被添加到全局或工程专用的符号库表中时才能使用。

通过点击 按钮然后选择一个库或点击 按钮然后输入库文件的路径来添加一个库。选定的库将被添加到当前打开的库表中（全局或特定工程）。可以通过选择所需的库条目并点击 按钮来删除库。

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 Editor or Symbol Chooser.

通过取消选中第一列中的 Active 复选框，可以使库处于非活动状态。非活动状态的库仍然在库表中，但不会出现在任何库的浏览器中，也不会从磁盘加载，这可以减少加载时间。

通过点击范围内的第一个库，然后 Shift - 点击范围内的最后一个库，可以选择一系列的库。

每个库必须有一个独特的名称：在同一个表中不允许有重复的库名称。然而，名称可以在全局和工程库表中重复。工程表中的库比全局表中的同名库优先级更高。

库的名称不一定要与库的文件名或路径有关。冒号字符（:）不能在库的名称或符号名称中使用，因为它被用作名称和符号之间的分隔符。

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

The appropriate library format must be selected in order for the library to be properly read. The supported formats are listed above. Only KiCad format libraries (.kicad_sym) can be saved. Other symbol library formats are read-only and must be converted to KiCad format before you can modify them.

有一个可选的描述字段，用于添加库条目的描述。选项字段目前不使用，所以添加选项在加载库时不会有任何影响。

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

By default, KiCad defines several path variables which are described in the project manager documentation. Path variables can be configured in the Preferences → Configure Paths…​ dialog.

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

${KIPRJMOD} is a special path variable that always expands to the absolute path of the current project directory. ${KIPRJMOD} allows libraries to be stored in the project folder without having to use an absolute path in the project library table. This makes it possible to relocate projects without breaking their project library tables.

符号库可以全局定义，也可以专门为当前加载的工程定义。在用户的全局表中定义的符号库总是可用的，并存储在用户的 KiCad 配置文件夹中的 sym-lib-table 文件中。工程专用的符号库表只对当前打开的工程文件有效。

每种方法都有其优点和缺点。在全局表中定义所有的库意味着它们在需要时总是可用的。这样做的缺点是，加载时间会增加。

在工程的基础上定义所有的符号库，意味着你只有工程所需的库，这减少了符号库的加载时间。缺点是你总是要记住添加每个工程所需的每个符号库。

一种使用模式是在全局范围内定义常用的库，并在工程专用的库表中定义工程所需的库。对于如何定义库没有任何限制。

Non-KiCad format libraries, including legacy libraries (.lib files), are read-only. They need to be converted to KiCad format (.kicad_sym files) before you can save changes to them.

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

也可以一次转换一个库，方法是在符号编辑器中打开它们并将它们另存为新库。

当加载在符号库表实现之前创建的原理图时，KiCad 将尝试将原理图中的符号库链接重新映射到适当的库表符号。 这个过程的成功与否取决于几个因素：

KiCad provides a symbol editing tool that allows you to create libraries; add, edit, delete, or transfer symbols between libraries; export symbols to files; and import symbols from files. The Symbol Editor can be launched from the KiCad Project Manager or from the Schematic Editor (Tools → Symbol Editor).

一般来说，设计一个符号的流程包括：

The Symbol Editor main window is shown below. It has three toolbars for quick access to common features and a symbol viewing/editing canvas. Not all commands are available on the toolbars, but all commands are available in the menus.

In addition to the toolbars, there are collapsible panels for the symbol tree and Properties Manager on the left. The bottom of the window contains a message panel that shows details about the selected object.

The button displays or hides the list of available libraries, which allows you to select an active library. When a new symbol is created, it will be placed in the active library.

Clicking on a symbol name opens that symbol in the editor, and hovering the cursor over the name of a symbol displays a preview of the symbol.

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 icon.

To save the symbol changes to a new symbol, click File → Save Copy As…​. The symbol can be saved in the current library or a different library, and a new name can be set for the symbol.

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

You can create a new symbol library by clicking File → New Library…​. At this point you must choose whether the new library should be added to the global symbol library table or the project symbol library table. Libraries in the global library table will be available to all projects, while libraries in the project library table will only be available in the current project.

Following selection of the library table, you must choose a name and location for the new library. A new, empty library will be created at the specified location.

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

还有几种图形选项。

这些属性以后也可以在符号属性窗口中修改。

一个新的符号将使用上述属性被创建，并将出现在编辑器中，如下图所示。

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 button and clicking on the new desired anchor position.

符号属性是在创建符号时设置的，但它们可以在任何时候被修改。要改变符号属性，请点击 图标，显示符号属性对话框。你也在编辑画布中空白位置双击打开属性对话框。

设置 单元数量，并检查 所有单元都可互换 和 具有交替的主体风格（如适用）是很重要的，因为这些设置会影响引脚和图形被添加到每个符号单元的方式。

如果你在向符号添加引脚后再改变符号的单元数，你将需要做额外的工作来为额外的单元添加引脚和图形。如果最初正确设置了这些属性，引脚和图形就会自动添加到每个单元。尽管如此，还是可以在任何时候修改这些属性。

图形选项 显示引脚编号 和 显示引脚名称 用来定义引脚编号和引脚名称文本的可见性。选项 将引脚名称置于内部 定义了引脚名称相对于引脚主体的位置。如果该选项被选中，引脚名称将被显示在符号的轮廓内。在这种情况下，引脚名称位置偏移 属性定义了文字远离引脚末端的位置。通常，0.02 到 0.05 英寸是合理的。

下面的例子显示了一个没有勾选 将引脚名称置于内部 选项的符号。注意名称和引脚编号的位置。

Symbols contain multiple fields, which are named values containing information related to the symbol. Fields can be displayed on the schematic or hidden and only shown in the symbol’s properties. Some fields have special meaning to KiCad: Reference and Footprint are both critical for creating a PCB, for example. Other fields may contain information that is important for a design but is not interpreted by KiCad, like pricing or stock information for a part.

Any fields defined in a library symbol will be included in the symbol when it is added to a schematic. You can also add new fields to symbols in the schematic. Whether they are in the library symbol or not, these fields can then be edited on a per-symbol basis in the schematic. They are also transferred to the symbol’s corresponding footprint in the PCB.

All library symbols are defined with five default fields: Reference, Value, Footprint, Datasheet, and Description, which are added whenever a symbol is created. These default fields cannot be deleted. Only the Reference field is required to have a value: the contents of a library symbol’s Reference field is used as the reference designator prefix when the symbol is added to a schematic. In the schematic, the symbol’s Reference field contains the entire reference designator.

如果使用 封装 字段，则包含符号与封装关联。格式是 LIBNAME:FOOTPRINTNAME，其中 LIBNAME 是封装库表中的封装库名称（见 PCB 编辑器手册中的 封装库表部分），FOOTPRINTNAME 是 LIBNAME 库中的封装名称。

The Description field can contain text describing the symbol such as the component function, distinguishing features, and package options. Together with the symbol’s name and keywords, text in this field is used when searching for symbols in the Symbol Chooser or Symbol Editor. Before KiCad version 8.0, this was a dedicated property (like the symbol name and keywords) rather than a symbol field.

Symbols defined in libraries are typically defined with only these five default fields. Additional fields such as vendor, part number, unit cost, etc. can be added to library symbols but generally this is done in the schematic editor so the additional fields can be added to every symbol in the schematic, not just all symbols of one type.

要编辑一个现有的符号字段，请双击该字段，选择它或悬停并按 E，或右击字段文本并选择 属性…​。

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 can be arbitrarily named, but names starting with ki_, e.g. ki_description, are reserved by KiCad and should not be used for user fields.

Fields have a number of properties, each of which is shown as a column in the properties grid. Not all columns are shown by default; columns can be shown or hidden by right clicking on the grid header and selecting or deselecting columns from the menu.

封装筛选器标签用于定义哪些封装适合与符号一起使用。筛选器可以在封装分配工具中使用，以便只显示每个符号合适的封装。

可以定义多个封装筛选器。符合任何一个筛选器的封装将被显示；如果没有定义筛选器，那么所有的封装都将被显示。

筛选器可以使用通配符。* 匹配任何数量的字符，包括零，而 ? 匹配零或一个字符。例如，SOIC-* 将匹配 SOIC-8_3.9x4.9mm_P1.27mm 封装以及任何其他以 SOIC- 开头的封装。筛选器 SOT?23 匹配 SOT23 以及 SOT-23。

Symbols can have more than one unit per package, each with different graphics and pin configurations. This is often used for logic gates, opamps, or other components that have multiple subunits within one physical package. Symbols can also have up to two body styles, a standard symbol and an alternate symbol often referred to as a "De Morgan equivalent".

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

By default, pins are specific to a unit and body style. When a pin is common to all units or all body styles, it only needs to be created once, no mattery how many units or body styles are used. This is also the case for the body style graphic shapes and text, which may be common to each unit, but typically are specific to each body style.

要向一个符号添加额外的单元，在符号属性对话框中将 单元数量 属性设置为适当的数字。默认情况下，符号单元被命名为 单元 A、单元 B 等，但你可以使用 编辑 → 设置单元显示名称…​ 为当前单元设置一个任意的名称。

Use the unit selection dropdown to select the unit you wish to edit.

要添加一个备用的主体样式，请在符号属性对话框中设置 存在备用的主体样式（德摩根） 属性。

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.

Graphical elements create the visual representation of a symbol and contain no electrical connection information. You can draw new graphic shapes using the buttons on the right toolbar. The following types of objects are available:

Each graphic item (line, arc, circle, etc.) can be defined as common to all units and/or body styles or specific to a given unit and/or body style.

Element options can be quickly accessed by right-clicking on the element to display the context menu for the selected element. You can also double-left-click on an element to modify its properties, or edit its properties using the Properties Manager pane.

Below is the properties dialog for a polygon element.

图形元素的属性是：

可以点击 按钮来创建和插入一个引脚。可以通过双击引脚来编辑引脚的属性。也可以删除或移动你已经添加的引脚。必须小心地创建引脚，因为任何错误都会对 PCB 设计产生影响。

一个引脚是由它的图形表示、名称和编号定义的。引脚的名称和编号可以包含字母、数字和符号，但不能包含空格。 为了使电气规则检查（ERC）工具发挥作用，引脚的电气类型（输入、输出、三态…​）也必须被正确定义。如果这个类型定义不正确，原理图上的 ERC 检查结果可能是无效的。

要点：

Power symbols are symbols that are used to label a wire as part of a global power net, like VCC or GND. The power symbol’s Value field determines the net label. The behavior of power symbols is described in the electrical connections section. Power symbols are handled and created the same way as normal symbols, but there are several additional considerations described below.

将电源符号放在一个专门的库中可能是有用的。KiCad 的符号库将电源符号放在 power 库中，用户可以创建库来存储自己的电源符号。如果在符号的属性中勾选了 定义为电源符号 框，该符号就会出现在原理图编辑器的 添加电源符号 对话框中，以便于访问。

Power symbols consist of a single pin of type Power Input. They must also have the Define as power symbol property checked.

下面是一个 GND 电源符号的例子。

要创建一个电源符号，请使用以下步骤：

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

符号编辑器可以检查符号中的常见问题。使用顶部工具栏上的 按钮运行符号检查器。

符号检查器检查的是：