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. You can choose to sort search results alphabetically or by best match by clicking on the button.

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.

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

Each field’s name and value can be visible or hidden, and there are several formatting options: horizontal and vertical alignment, orientation, position, font, text color, text size, and bold/italic emphasis. Field autoplacement can also be enabled on a per-field basis. The displayed position is always indicated for a normally displayed symbol (no rotation or mirroring) and is relative to the anchor point of the symbol.

The 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.

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.

Symbols have several attributes that affect how the symbols are treated by other parts of KiCad.

Exclude from simulation prevents the symbol from being included in SPICE simulations.

Exclude from bill of materials prevents the component from being included in BOM exports.

Exclude from board means that the symbol is schematic-only, and a corresponding footprint will not be added to the PCB.

Do not populate means that the component should not be attached to the PCB, although a corresponding footprint should still be added to the board. DNP symbols appear desaturated and with a red "X" over them in the schematic, as shown below.

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 library symbol, use Tools → Update Symbols from Library…​, or right click a symbol and select Update Symbol…​. 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 schematic, 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.

When a symbol in a schematic diverges from the corresponding symbol in the original symbol library, you can use the Compare Symbol with Library tool to inspect the differences between the two versions of the symbol. Run the tool using Inspect → Compare Symbol With Library.

The Summary tab shows the name of the symbol, including its library and schematic reference designator, and provides a list of the differences between the schematic and library versions of the symbol.

The Visual tab shows a visual comparison of the schematic and library versions of the symbol. This can be used as a visual diff tool.

By default, the comparison displays both versions of the symbol superimposed on each other. To see the changes more easily, you can drag the slider at the bottom of the tab to the right to emphasize the library version of the symbol in the superimposed view (making the schematic version of the symbol more transparent) or drag it to the left to emphasize the schematic version (making the library version more transparent). At the far right and left ends of the slider, the schematic and library versions of the symbol, respectively, are fully hidden. It may be helpful to drag the slider back and forth to see the changes more clearly.

The screenshot above shows a visual comparison with the schematic version of the symbol deemphasized. You can see a partially transparent pin 5 (from the schematic version of the symbol) is in a different location than the fully opaque pin 5 (from the library symbol). This indicates that the pin was moved in either the schematic or library version of the symbol.

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 to move down, 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 button; a field with that name will be added to every symbol. Each field can have its own label, which doesn’t have to be the same as the field name, and is used as the column header. Fields can be renamed with the button or deleted with the button.

Similar symbols can optionally be grouped by any symbol field using the Group By checkboxes. Symbols are grouped into a single row in the table if all of their Group By fields are identical. 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.

Presets are available to configure the list of fields. Presets store which fields are displayed, which fields are used for grouping, and the column order. You can create and save your own presets or use one of several default presets. Custom presets can be deleted in this dialog or in the Schematic Setup dialog.

Symbols can be filtered by reference designator using the Filter textbox at the top. The filter supports wildcards: * matches any number of any characters, including none, and ? matches any single character. You can also change the display scope, showing only symbols in the current sheet, the current sheet and all of its subsheets, or the entire project. Symbols with the DNP (do not populate) attribute set can be optionally excluded by checking the Exclude DNP box.

You can cross-probe from this dialog by selecting a row in the table. Depending on the Cross-probe action setting at the bottom of the dialog, this can highlight the corresponding symbol in the schematic, select the corresponding symbol in the schematic, or do nothing. The selection action can also select the symbol’s footprint in the board editor, depending on the PCB Editor cross-probing settings.

The Symbol Fields Table is also a bill of materials tool. You can use the Export button to save the symbol fields to an external file. The fields are exported to the BOM exactly as they are currently shown in the spreadsheet view. File format settings are configured in the Export tab. For more information about exporting a BOM, see the BOM tool documentation.

When auto-annotation is enabled, symbols will be automatically annotated when they are added to the schematic. You can enable auto-annotation by checking the Automatically annotate symbols checkbox in the Schematic Editor → Annotation Options pane in Preferences. Auto-annotation can also be toggled using the button in the left toolbar.

When multiple symbols are added simultaneously, they are annotated according to the Order setting, sorted by either X or Y position.

The Numbering option sets the starting number for new reference designators. This can be the lowest available number, or a number based on the sheet number.

For more information about annotation options, see the documentation for the Annotation tool.

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. If the Recurse into subsheets option is selected, symbols in subsheets of the selected scope will be reannotated; otherwise symbols in subsheets will not be reannotated. For example, if Recurse into subsheets and Selection only selected, symbols in any selected subsheets will be reannotated.

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.

Wires are used to directly establish electrical connections between two points. 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.

Labels are used to assign net names to wires and pins. Wires with the same net name are considered to be connected, so labels can be used to make connections without drawing direct wire connections.

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.

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.

Power symbols are symbols that are conventionally used to represent a connection to a power net, such as VCC or GND. Power symbols are virtual: they do not represent a physical component on the PCB.

In addition to being a visual indicator that the attached net is a power rail, power symbols make global connections: two power symbols with the Value connect to each other anywhere in the schematic, regardless of sheet. The power symbol’s Value field determines the name of the attached net.

In the figure below, power 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 symbols are found in the power library, but power symbols can be created in any library. Creating custom power symbols is described in the symbol editor documentation. Instead of making a new symbol, you can also modify an existing power symbol in the schematic: changing its Value field will change the net the power symbol connects to.

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 of a hierarchy, it will take its name from the highest level of the hierarchy where it has a hierarchical label or local label. As usual, local labels take priority over hierarchical labels.

If none of the label types 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 prevent "unconnected pin" ERC warnings for pins that are intentionally unconnected. Also, while symbol pins that are stacked on top of each other are normally connected to the same net, if a no-connection flag is added to the stacked pins they will instead be connected to separate nets.

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 and prevent stacked pins from connecting to each other.

When the power pins of a symbol are visible, they must be connected, as with any other signal. However, symbols 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. This kind of implicit connection is not recommended in new designs.

Net classes are managed in the Net Classes panel of the Schematic Setup dialog.

The top pane lists the net classes that exist in the design. The Default net class always exists, and you can add additional net classes with the button or remove the selected net class with the button.

Net classes can be moved up and down in priority order with the and buttons. Note that the Default net class will always be the lowest priority net class and can therefore not be moved.

Each net class can have unique graphic properties that determine how wires of that net class are displayed in the schematic. Wire and bus thicknesses, color, and line style (solid, dashed, dotted, etc.) can all be adjusted. Setting the color to transparent will use the theme’s default wire/bus color for the net class, which is configurable in Preferences.

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

All net class parameters for user-defined net classes are optional. However, all properties belonging to the Default net class must be set. When a net has more than one net class assigned, the appropriate value for graphic properties or board design rules is taken from the highest priority assigned net class with the relevant value set. If only one net class is assigned which contains missing properties, any missing values will be taken from the Default net class.

The bottom pane lists pattern-based net class assignments. Each row has a net name pattern and a net class; nets with names that match the pattern are assigned to the specified net class. If a net matches multiple patterns, the first match is used. Pattern-based net class assignments are dynamic: when a new net is added that matches an existing pattern, it will be assigned to the associated net class 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.

Use the button to add a net class assignment pattern or the button to remove a pattern.

Instead of adding net class patterns in the Schematic Setup dialog, you can directly create net class patterns from the schematic canvas. Right click a net and select Assign Netclass…​ to bring up the Add Netclass Assignment dialog. The net class pattern is pre-filled with the name of the selected net, but the pattern can be changed if desired. All nets matching the pattern are displayed in the dialog. This method can only be used on nets with an assigned name.

As an alternative to pattern-based net class assignment, net classes can be graphically assigned to nets in the schematic using either directive labels, net labels, or rule areas. Net classes must be created in Schematic Setup before they can be assigned graphically.

In the image below, a directive label is used to assign signals to the 50R net class.

Directive labels are added with the button in the right toolbar. They behave like labels, except that they cannot be used to name a net. The attached net is assigned a net class according to the value of the directive’s Net Class field. The Net Class field presents a dropdown list of all the net classes in the design.

If a directive is attached to a bus, all members of the bus are assigned to the specified net class.

In addition to the associated net class, you can edit the directive’s shape (dot, circle, diamond, or rectangle), orientation, pin length, and color in the directive’s properties.

Net labels can also be used to assign net classes to nets by adding a Net Class field to the label.

The Rule Area tool can be used to draw a shape to which net class directives can be attached. Any wire, bus, label, or symbol pin which crosses or is inside the rule area will be assigned the net class of a net class directive attached to the rule area border. An example is shown in the image below; all wires passing through the rule area will be assigned the RAM_ADDR net class.

You can show or hide directive labels in the schematic using the View → Show Directive Labels option.

Two kinds of text can be added to schematics, which are referred to as text () and text boxes (). Both are added using their respective buttons in the right toolbar. Text boxes are similar to regular text except that they have an optional border and they automatically reflow text within that border.

Both kinds of text item support multiline text and basic formatting features, but text boxes wrap text to fit in the outline and have additional formatting options. All text has adjustable fonts, color, size, bold and italic emphasis, left and right alignment, and vertical and horizontal orientation. Text boxes additionally support horizontal centering, vertical alignment options, and colored borders and fill.

Graphic rectangles (), circles (), arcs (), and lines () can all be added using their respective buttons in the right toolbar.

Line width, color, and style (solid, dashed, or dotted) can be configured in the properties dialog for each shape (E). Rectangles, circles, and arcs can also have a fill color set and have their outlines removed.

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.

Like wires, graphic lines obey the line drawing mode setting (90 degree, 45 degree, or free angle), which you can set using the toggle buttons on the left toolbar (, , and , respectively). Shift+Space cycles through the modes.

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

Bitmap images can be added to the schematic with the button. Images in the schematic can be moved and scaled. The properties dialog allows setting a location and scale as well as converting the image to greyscale.

Properties of text and graphics can be edited in bulk using the Edit Text and Graphic Properties dialog (Tools → Edit Text and Graphic Properties…​). The tool can also modify visual properties of wires and buses.

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 next to Issue Date. Note that 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…​.

You can quickly add wires, labels, or no-connection markers to a selection of pins using the Pin Helpers tools in the right-click context menu. This can help you quickly break out unconnected pins from a symbol or hierarchical sheet. By selecting Pin Helpers → Wire, the wire tool will begin drawing a wire from all selected pins at once. If you select No Connect, no-connection markers will be added to the end of each selected pin. And if you choose Net Label, Hierarchical Label, or Global Label, a label of the respective type will be placed at the end of each selected pin. Each label’s name will be set to the corresponding pin name. The new labels will remain selected, so you can easily move them away from the symbol using M or G, depending on whether you wish to maintain a wired connection between the pins and the labels.

Existing labels and text objects can be changed to another type of label or text by right clicking the object(s) and selecting the target object type from the Change To submenu. The allowed types for source and target objects are local labels, global labels, hierarchical labels, directive labels, text objects, and text boxes. The value of the original object is preserved in the resulting object: when a text object is converted to a label, the label’s value (net name) will be the original text, and vice versa.

You can swap the position of two selected objects using the Swap command (S; also available in the right-click context menu). This works on symbols, labels, and graphical items. The first object is assigned the location and rotation of the second object, and vice versa. If there are more than two objects selected, the locations are cycled: the last object gets the position of the first object, the first object gets the location of the second, and so on.

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. Overbar offset ratio controls the vertical spacing between text and an overbar (~{}) over that text, as a ratio of the text height. 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 ratio 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. Connection width specifies the grid size used for the Symbol pin or wire end off connection grid ERC check. Schematics typically use a 50 mil grid for electrical connections, so this should usually remain set at 50 mils.

The Operating Point Overlay settings configure how operating point simulation results are displayed on the schematic canvas. The significant digits settings control the number of significant digits printed on voltage and current overlays. The range settings control the units used to display voltage and current measurements.

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.

BOM presets are saved configurations for the Symbol Fields Table and BOM export tool. There are two types of presets. BOM presets configure which fields are displayed in the symbol fields table, which order they are displayed in, and how they are used to group symbols. These fields are also directly used in the BOM output. BOM formatting presets configure the output BOM file format, including which separator characters are used to separate fields. Both types of presets are created in the Symbol Fields Table, but can are listed and can be deleted here.

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

Pattern-based net class 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…​.