To place a symbol in your schematic, use the button or the A hotkey. The Choose Symbols dialog appears and lets you select a symbol to add. Symbols are grouped by symbol library.

By default, only the symbol/library name and description columns are shown. Additional columns can be added by right-clicking the column header and selecting Select Columns.

The Choose Symbol dialog filters symbols by name, keywords, description, and all additional symbol fields according to what you type into the search field.

有一些高级筛选器可用：

如果符号指定了一个默认的封装，这个封装将在右下方预览。如果符号包括封装过滤器，可以在右边的封装下拉菜单中选择满足封装过滤器的备用封装。

选择一个要放置的符号后，该符号将被附在光标上。 左键点击原理图中所需要的位置，将符号放入原理图中。在将符号放入原理图之前，你可以通过热键或右键菜单来旋转它、镜像它和编辑它的字段。这些操作也可以在放置后进行。

如果 放置重复副本 选项被选中，在放置一个符号后 KiCad 将开始放置该符号的另一个副本。这个过程一直持续到用户按下 Esc。

对于有多个单元的符号，如果 放置所有单元 选项被选中，在放置符号后 KiCad 将开始放置该符号中的下一个单元。 这将持续到最后一个单元被放置或用户按下 Esc。

一个 《电源符号，电源符号》是一个代表与电源网络连接的符号。 这些符号被分组在 power 库中，所以它们可以使用符号选择器来放置。 然而，由于电源的放置很频繁， 工具是可用的。这个工具也类似，只是搜索是直接在 power 库和任何其他包含电源符号的库中进行。

符号可以用移动（M）或拖动（G）工具移动。这些工具作用于选定的符号，或者如果没有选定符号，则作用于光标下的符号。

移动 工具移动符号本身，而不保持与符号引脚的导线连接。

拖动 工具在移动符号时不会破坏其引脚的导线连接，因此也会移动连接的导线。

你也可以用鼠标点击并拖动符号，这取决于偏好设置中 鼠标和触摸板 部分的 左键拖动手势 设置。

符号也可以旋转（R）或在X（X）或Y（Y）方向上进行镜像。

符号的字段可以在符号的属性窗口中进行编辑。用 E 热键或通过双击符号来打开符号属性窗口。

符号属性窗口在一个表格中显示一个符号的所有字段。新的字段可以被添加，现有的字段可以被删除、编辑、重新排序、移动或调整大小。

每个字段的名称和值可以是可见的或隐藏的，并且有几个格式化选项：水平和垂直对齐、方向、位置、字体、文本颜色、文本大小和黑体/大写强调。字段的自动放置也可以在每个字段的基础上启用。对于正常显示的符号，显示的位置总是被指示的（没有旋转或镜像），并且是相对于符号的锚点而言的。

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. These functions are described later.

编辑符号…​ 打开符号编辑器，编辑原理图中的符号副本。注意，库中的原始符号将不会被修改。编辑库中的符号…​ 按钮可以打开符号编辑器来编辑库中的原始符号。在这种情况下，原理图中的符号将不会被修改，直到用户点击 更新库中的符号…​ 按钮。

符号有几个属性，它们会影响 KiCad 其他部分对符号的处理方式。

从模拟中排除 防止该符号被包括在 SPICE 模拟中。

从 BOM 中排除 防止该元件被包括在 《BOM 导出，BOM 导出》中。

从电路板中排除 意味着该符号仅用于原理图，相应的封装不会被添加到 PCB 上。

不使用 意味着该元件不应该被连接到 PCB 上，虽然相应的封装仍然应该被添加到电路板上。如下图所示，DNP 符号在原理图中显示为不饱和状态，上面有一个红色的 "X"。

When a symbol is added to the schematic, KiCad embeds a copy of the library symbol in the schematic so that the schematic is independent of the system libraries. Symbols that have been added to the schematic are not automatically updated when the library changes. Library symbol changes are manually synced to the schematic so that the schematic does not change unexpectedly.

To update symbols in the schematic to match the corresponding symbol, use Tools → Update Symbols from Library, or right click a symbol and select Update Symbol from Library. You can also access the tool from the symbol properties dialog.

The top of the dialog has options to choose which symbols will be updated. You can update all symbols in the dialog, update only the selected symbols, or update only the symbols that match a specific reference designator, value, or library identifier. The reference designator and value fields support wildcards: * matches any number of any characters, including none, and ? matches any single character.

The middle of the dialog has options to control what parts of the symbol will be updated. You can select specific fields to update or not update, which properties of the fields to update (text, visibility, size and style, and position), and how to handle fields that are missing or empty in the library symbol. You can also choose whether to update symbol attributes, such as do not populate and exclude from simulation / bill of materials / board.

The bottom of the dialog displays messages describing the update actions that have been performed.

To change an existing symbol to a different symbol, use Edit → Change Symbols…​, or right click an existing symbol and select Change Symbol…​. This dialog is also accessible from the symbol properties dialog.

The options for the Change Symbols dialog are very similar to the Update Symbols from Library dialog.

Another way to swap existing symbols for new ones is to use Tools → Edit Symbol Library Links…​. This dialog contains a table of every symbol in the design, grouped by current library symbol. By choosing a new symbol in the New Library Reference column, you can make all instances of the existing symbol instead point to the new symbol. If the Update symbol fields from new library option is used, the contents of the existing symbols' fields will be updated to match the new symbols' fields.

The Map Orphans button attempts to automatically remap orphaned symbols to symbols with the same name in an active library. For example, if there is a symbol with the current library reference mylib:symbol123, but the mylib library cannot be found, the Map Orphans button will attempt to find a symbol named symbol123 in any of the libraries that are present. This button is only enabled if orphaned symbols are present in the schematic (see the legacy schematics section).

This dialog is primarily useful for managing symbols that appear in multiple libraries, when you want to switch from one library to another. For example, if a schematic uses symbols that are in both a global library and a project-specific library, the Symbol Library References dialog could be used to switch between using the global symbols or the equivalent project-specific symbols. It does not have features for fine-grained control of how fields are updated; for that, use the Change Symbols dialog.

符号字段表允许你在电子表格界面中查看和修改所有符号的字段值。你可以用 按钮打开符号字段表。

单元格可以用方向键导航，或者用 Tab / Shift+Tab 向右/向左移动，Enter / Shift+Enter 向下/向上移动。

通过点击和拖动可以选择一个单元格范围。选定的整个单元格范围将被复制（Ctrl+C）或粘贴到（Ctrl+V）复制或粘贴操作上。从表中复制单元格的范围对于创建 BOM 非常有用。下面将介绍复制和粘贴单元格的更多细节。

任何符号字段都可以通过左边的 显示 复选框来显示或隐藏，或者通过右键点击表格的标题。新的符号字段可以用 添加字段…​ 按钮添加。

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 Group Symbols checkbox enables or disables symbol grouping, and the button recalculates groupings.

Symbols can be filtered using the Filter textbox at the top. The filter supports wildcards: * matches any number of any characters, including none, and ? matches any single character.

你可以使用 导出为 CSV…​ 按钮，将符号字段保存到外部文件。这可以作为一个简单的 BOM 生成工具，尽管 《BOM 导出，BOM 工具》提供了对生成的输出的更好控制。

启用自动批注后，符号被添加到原理图中时将被自动批注。你可以在 偏好设置 中 原理图编辑器 → 批注选项 窗格中选中 自动批注符号 复选框来启用自动批注。自动批注也可以通过左侧工具栏的 按钮进行切换。

当同时添加多个符号时，它们会根据 顺序 设置进行批注，按 X 或 Y 位置排序。

编号 选项为新的位号设置起始编号。 这可以是最低的可用数字，也可以是基于原理图编号的数字。

关于注解选项的更多信息，请参见《批注工具，批注工具》的文档。

批注工具会自动为原理图中的符号指定位号。要启动批注工具，请点击顶部工具栏上的 按钮。

该工具提供了几个选项来控制符号的批注方式。

范围： 选择批注是否适用于整个原理图、仅适用于当前原理图或仅适用于选定的符号。如果选择了 递归到子原理图 的选项，所选范围的子原理图中的符号将被重新批注；否则子原理图中的符号将不会被重新批注。例如，如果 递归到子原理图 和 仅选择，任何选定的子原理图中的符号将被重新批注。

选项： 选择批注是否应适用于所有符号和重置 现有的位号，或仅适用于未批注的符号。

顺序： 选择编号的方向。如果符号按 X 位置排序，原理图页面左侧的所有符号将比页面右侧的符号编号低。如果符号按 Y 位置排序，则原理图顶部的所有符号的编号将低于原理图底部的符号的编号。

编号： 选择编号位号的起点。每一个位号都会选择在起点之上的最低的未使用的数字。起始点可以是一个任意的数字（通常是 0），也可以是纸张编号乘以 100 或 1000，这样每个零件的位号就与它所在的原理图页相对应。

清除批注 按钮可以清除所选范围内的所有位号。

批注信息可以用底部的复选框进行过滤，或用 保存…​ 按钮保存到报告中。

导线用于在两点之间直接建立电气连接。 要建立连接，必须将一段导线的末端与另一段导线或一个引脚相连。只有导线的末端才能建立连接；如果一根导线穿过另一根导线的中间，就不会建立连接。

未连接的导线端有一个小方块，表示连接点。 当连接到导线端时，这个方块就会消失。未连接的引脚有一个圆圈，当进行连接时也会消失。

标签是用来给导线和引脚分配网络名称的。具有相同网络名称的导线被认为是连接在一起的，所以标签可以用来进行连接，而不需要直接画线连接。

一个网络只能有一个名称。如果有两个不同的标签放在同一个网络上，将产生一个 ERC 违规。 在网表中只使用其中一个网络名称。最终的网络名称是根据下面描述的《网络名称分配规则》决定的。

有三种类型的标签，每种都有不同的连接范围。

总线是一种在原理图中分组相关信号的方法，以简化复杂的设计。 总线可以像导线一样用总线工具画出来 ，并像信号线一样用标签命名。

在下面的原理图中，许多引脚都连接到总线上，也就是中间的蓝色粗线。

当一个符号的电源引脚是可见的，它们必须被连接，就像其他信号一样。然而，诸如门和触发器等符号有时会画出隐含的电源输入引脚，这些引脚是隐性连接的。

KiCad 会自动将类型为 "电源输入" 的隐形引脚连接到与该引脚同名的全局网络。例如，如果一个符号有一个名为 VCC 的隐藏电源输入引脚，这个引脚将被全局连接到所有原理图上的 VCC 网络。

可能有必要将不同名称的电源网络连接起来（例如，TTL 元件中的 GND 和 MOS 元件中的 VSS）。为了达到这个目的，为每个网络添加一个 《电源符号,电源符号》，并用一根导线连接它们。

如果使用隐藏的电源引脚，不建议使用本地标签进行电源连接，因为它们不会连接到其他片上的隐藏电源引脚。

电源符号是传统上用来表示与电源网连接的符号，如`VCC` 或 GND。除了作为连接网络是电源布线的视觉指示外，电源符号还可以进行全局连接：两个具有相同引脚名称的电源符号在原理图中的任何地方都可以相互连接，而不用考虑原理图。

Power symbols are virtual: they do not represent a physical component on the PCB.

在下图中，电源符号用于将电容器的正负极分别连接到 VCC 和 GND 网路上。

In the KiCad standard library, power symbols are found in the power library, but power symbols can be created in any library.

To create a custom power symbol, 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 symbol is described in more detail in the Symbol Editor section.

原理图中的每个网都被分配了一个名称，无论这个名称是由用户指定还是由 KiCad 自动生成。

当多个标签附加到同一个网时，最终的网络名将按以下顺序确定，从最高优先级到最低：

如果一个网络有多个同一类型的标签，则按字母顺序排序，使用第一个。

如果一个网络穿过《层次原理图,层次》的多张原理图，它将从它有层次标签或局部标签的层次结构的最高层取名。通常，局部标签优先于层次标签。

如果上面的标签类型都没有附加到网络中，那么网络的名称将根据连接的符号引脚自动生成。

在上面的截图中可以看到两个 PWR_FLAG 符号。它们向 ERC 表明，两个电源网络 VCC 和 GND 实际上连接到一个电源上，因为没有明确的电源，如连接到任何一个网络的电压调节器输出。

如果没有这两个标志，ERC 工具会诊断出：错误：输入电源引脚没有被任何输出电源引脚驱动。

PWR_FLAG 符号可以在 power 符号库中找到。通过将任何电源输出引脚连接到网络上，可以达到同样的效果。

No-connection flags () are used to indicate that a pin is intentionally unconnected. These flags prevent "unconnected pin" ERC warnings for pins that are intentionally unconnected.

Note that no-connection flags are distinct from the "unconnected" symbol pin type, although they both prevent "unconnected pin" ERC warnings on the pin in question.

网络类在 原理图设置 对话框的 网络类 面板中管理。

顶部的窗格列出了设计中存在的网络类。默认 网络类总是存在的，你可以通过 按钮添加额外的网络类，或者通过 按钮删除选定的网络类。

每个网络类可以有独特的图形属性，决定该网络类的导线如何在原理图中显示。导线和母线的厚度、颜色和线条风格（实线、虚线、点线等）都可以调整。将颜色设置为透明将使用主题的默认导线/总线颜色，该颜色可在《偏好设置颜色，偏好设置》中配置。

You can also set board design rules for each netclass, although the DRC fields are hidden by default. Right click the header row to show or hide additional columns. For more information about setting netclass design rules, see the PCB editor documentation.

The bottom pane lists pattern-based netclass assignments. Each row has a net name pattern and a netclass; nets with names that match the pattern are assigned to the specified netclass. If a net matches multiple patterns, the first match is used. Pattern-based netclass assignments are dynamic: when a new net is added that matches an existing pattern, it will be assigned to the associated netclass automatically. Net patterns can use both wildcards (* to match any number of any characters, including none, and ? to match any character) and regular expressions. The nets that match the selected pattern are displayed to the right of the pattern list.

For example, the net* pattern matches nets named net, net1, network, and any other net name beginning with net. Because * has a slightly different meaning in a regular expression (* matches zero or more of the preceding character), the net* pattern would also match a net named ne.

使用 按钮来添加网络类分配模式，或 按钮来删除模式。

您可以从原理图画布上直接创建网络类图案，而不是在原理图设置对话框中添加网络类图案。右击一个网络，选择分配网络类…​，就会出现添加网络类分配对话框。网络类模式会预先填上所选网络的名称，但如果需要，也可以改变模式。所有符合该模式的网都显示在对话框中。

作为基于模式的网络类分配的替代方法，网络类可以用 网络类指令 或 标签 以图形方式分配给原理图中的网络。网络类必须在《原理图设置网络类，原理图设置》中创建，然后才能以图形方式分配。

在下面的图片中，一个网络类指令被用来给 50R 网络类分配信号。

网络类指令是通过右边工具栏的 按钮添加的。它们的行为类似于《标签，标签》，除了它们不能被用来命名一个网络。根据指令的 网络类 字段的值，附加的网络被分配了一个网络类。`网络类`字段提供了一个设计中所有网络类的下拉列表。

如果一个指令被附加到一个总线上，总线上的所有成员都被分配到指定的网络类。

除了相关的网络类，你还可以在指令的属性中编辑指令的形状（点、圆、钻石或矩形）、方向、引脚长度 和 颜色。

《标签网络类，网络标签也可以用来给网络分配网络类》，方法是在标签中添加一个 网络类 字段。

如果超过一个不同的网络类被图形化地分配给一个网络，《ERC 检查清单，ERC 将报告一个问题》。图形化的网络类分配优先于基于模式的分配：如果一个网络与网络类模式分配相匹配，并且也有一个图形化的网络类分配，那么将使用图形化的网络类分配。

有两种文本可以被添加到原理图中，它们被称为文本（）和文本框（）。两者都是使用右侧工具栏中各自的按钮添加的。

这两种文本项目都支持多行文本和基本的格式化功能，但文本框将文本包起来以适应大纲，并有额外的格式化选项。所有的文本都有可调整的字体、颜色、大小、黑体和斜体强调，左右对齐，以及垂直和水平方向。文本框还支持水平居中，垂直对齐选项，以及彩色边框和填充。

图形矩形（）、圆形（）、弧形（）和直线（）都可以使用右侧工具栏中各自的按钮添加。

线条的宽度、颜色和样式（实线、虚线或点线）可以在每个形状（E）的属性对话框中进行配置。矩形、圆形和弧线也可以设置填充颜色并去除其轮廓。

Setting a shape’s line width to 0 uses the schematic default line width, which is configurable in Schematic Setup. Spacing for line dashes is also configurable there. Removing a line or fill color uses the color theme’s graphics color, which is configurable in Preferences.

像《画和编辑导线，导线》一样，图形线服从线的绘制模式设置（90 度，45 度，或自由角度），你可以用左边工具栏上的切换按钮来设置（，，和 ，分别）。 Shift+Space 循环浏览这些模式。

As with PCB tracks, the / hotkey switches line posture.

位图图像可以通过 按钮添加到原理图中。原理图中的图像可以被移动和缩放。属性对话框允许设置位置和比例，以及将图像转换为灰度。

文本和图形的属性可以通过 编辑文本和图形属性 对话框（工具 → 编辑文本和图形属性…​）进行批量编辑。该工具还可以修改导线和总线的视觉属性。

标题块是用页面设置工具（）编辑的。

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 next to Issue Date. Note that the date in the schematic will not be automatically updated.

也可以选择一个原理图模板文件。

原理图编号（X/Y纸）会自动更新，但原理图页码也可以用 编辑 → 编辑原理图页码…​ 手动设置。

The formatting panel contains settings for the appearance of symbols, text, labels, graphics, and wires.

Symbol unit notation sets how each unit of a multi-unit symbol is referred to in its reference designator. By default, a different letter for each unit is appended to the reference designator with no separator, for example U1B for the second unit of symbol U1, but this can be changed. Numbers can be used instead of letters, and various separators can be used between the symbol designator and the unit identifier (., -, _, or none).

Default text size sets the default text height used by the text, text box, and label tools. Label offset ratio controls the vertical spacing between a local label’s text and the attached wire, relative to the label’s text size. This also affects the spacing between symbol pins and their pin number. Global label margin defines the size of the box around a global label, relative to the global label’s text size. Increasing the margin may be useful to avoid overlapping text with overbars (~{}) or letters with descenders, but this may cause closely packed global labels to overlap with each other.

Default line width sets the default line width for symbol graphics, if the symbol does not override the default line width. Pin symbol size scales symbol pin graphic style annotations, such as the bubble on an inverted pin.

Junction dot size sets the schematic’s default wire junction dot size. The default size can be overridden by editing an individual junction dot’s properties.

Show inter-sheet references enables or disables the display of inter-sheet references, which are a list of page numbers next to a global labels that link to other places in the schematic where the same global label appears. Show own page reference controls whether the current page is included in the list of page numbers. Standard and abbreviated determine whether to display the complete list of page numbers or only the first and last page numbers. The prefix and suffix fields add optional characters before and after the list of page numbers. In the image of an inter-sheet reference below, a prefix and suffix of [ and ], respectively, have been added.

Dashed line appearance is controlled in the Formatting section. Dash length controls the length of dashes, while Gap length controls the spacing between dashes and dots. The dash and gap lengths are relative to the line width: a gap length of 2 means twice the width of the line.

Field name templates are empty symbol fields that are automatically added to all symbols in the schematic. These can be useful when every symbol in the schematic needs additional fields beyond the fields that are defined in the library symbols, for example a field for the manufacturer’s part number.

Template fields can be set as visible or invisible, and can also be set as URL fields.

Field name templates that are defined in schematic setup apply only to the current project. Field name templates can also be defined in Preferences, which apply to all projects edited on your computer.

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

The Pin Conflicts Map 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. For example, by default an error is produced when an output pin is connected to another output pin.

These panels are explained in more detail in the ERC section.

The Net Classes panel allows you to manage netclasses for the project and assign nets to netclasses with patterns. Managing netclasses in this panel is equivalent to managing them in the Board Setup dialog. Nets can also be assigned to netclasses in the schematic using graphical assignments with net class directives or net labels.

Pattern-based netclass assigment is explained in more detail in the net classes section.

The Bus Alias Definitions panel allows you to create bus aliases, which are names for groups of signals in a bus. For more information about bus aliases, see the bus alias documentation.

Text replacement variables can be created in the Text Variables section. These variables allow you to substitute the variable name for any text string. This substitution happens anywhere the variable name is used inside the variable replacement syntax of ${VARIABLENAME}.

For example, you could create a variable named VERSION and set the text substitution to 1.0. Now, in any text object on the PCB, you can enter ${VERSION} and KiCad will substitute 1.0. If you change the substitution to 2.0, every text object that includes ${VERSION} will be updated automatically. You can also mix regular text and variables. For example, you can create a text object with the text Version: ${VERSION} which will be substituted as Version: 1.0.

Text variables can also be created in Board Setup. Text variables are project-wide; variables created in the schematic editor are also available in the board editor, and vice versa.

There are also a number of built-in system text variables.

Modern versions of KiCad can open schematics created in versions prior to KiCad 6.0, but the cache library file (<projectname>-cache.lib) must be present to load the schematic correctly.

Since version 6.0, KiCad stores all symbols used in a project in the schematic. This means that you can open a schematic made in KiCad 6.0 or later on any computer, even if the libraries used in the project are not installed or have changed. Modern KiCad schematic files use the .kicad_sch extension.

Prior to version 6.0, KiCad did not store symbols in the schematic. Instead, KiCad stored references to the symbols and their libraries. It also stored a copy of every symbol used by the project in a separate cache library file (<projectname>-cache.lib). As long as the cache library was included with the project, the project could be distributed without the system library files, because KiCad could load any needed symbols from the cache library as a fallback if the libraries referenced in the schematic were missing. Legacy KiCad schematic files use the .sch extension.

When you open a legacy schematic, KiCad will look in the cache library to find all of the symbols used in the schematic in the cache library. When you save the legacy schematic, KiCad will save it as a new file in the modern schematic format (.kicad_sch), with the necessary symbols embedded in the schematic itself. The original legacy schematic and the cache library will remain, unmodified, but they are no longer necessary once the schematic has been saved in the modern format.

When you open a legacy schematic, KiCad may display the Project Rescue Helper dialog. This means that one or more symbols in the cache library do not match the corresponding symbol in the external library. The dialog helps you "rescue" symbols from the cache library into your schematic, if desired. You can also open the rescue dialog at any time using Tools → Rescue Symbols…​. The cache library file must be present in order to use the rescue tool.

The rescue dialog lists all symbols that don’t match between the cache library and the external symbol library. The discrepancy can be because:

For each symbol in the list, selecting the symbol displays the reference designator and value for each instance of the symbol, and shows a visual preview of the symbol. If a corresponding symbol exists in the system symbol library, the dialog shows both copies of the symbol for comparison. If the symbol only exists in the cache library, the dialog only shows the cached symbol.

In this example, the project originally used a diode with the cathode facing left, but the library now contains one with the cathode facing right. This change would break the design, so it would be important to use the cached symbol as the original designer intended.

Pressing Rescue Symbols here will cause the selected symbols from the cache library to be saved into a special rescue library (<projectname>-rescue.kicad_sym). The corresponding symbols in the schematic will be updated to use the newly rescued symbols. Any unselected symbols will not be rescued, but their symbol linkage can be updated in the schematic later.

Alternatively, pressing Skip Symbol Rescue will exit the dialog without rescuing any symbols. KiCad will use the versions of the symbols found in the external libraries. You can run the rescue function again with Tools → Rescue Symbols…​, or manually edit symbol linkage in the symbol’s properties.

If you would prefer not to see this dialog, you can press Never Show Again. This has the same effect as pressing Skip Symbol Rescue for the current schematic and all future schematics.

If a symbol in a legacy schematic cannot be found in either the cache library or the external library, KiCad cannot rescue that symbol. A placeholder symbol is inserted into the schematic in its place, as shown below.

You can attempt to remap these orphaned symbols using the Change Symbols or Edit Symbol Library Links dialogs, but either option may require manual corrections to the schematic. These tools are explained in more detail in the Updating and exchanging symbols section.

Modern versions of KiCad can open schematics created in versions prior to KiCad 5.0, but you will need to go through a symbol remapping process to open the schematic without losing symbol information.

Since version 5.0, KiCad schematics refer to specific symbols using both the symbol and library name. Even if multiple libraries each contain a symbol with the same name, the designer’s intended symbol is unambiguously specified.

Prior to version 5.0, KiCad schematics stored only the symbol name, not the library name. Symbols in the schematic were indirectly mapped back to the original library by searching through the project’s library list for a matching symbol. When you open a pre-5.0 schematic, KiCad will attempt to automatically "remap" the symbols so that each bare symbol name is replaced with a fully-specified symbol library and symbol name pair. The original schematics will be backed up in a rescue-backup folder.

You can skip the automatic remapping, but you will need to remap the symbols yourself using the Change Symbols dialog. You can also re-run the Remap Symbols tool using Tools → Remap Legacy Library Symbols…​.