Advanced topics

Configuration and Customization

Pcbnew has a variety of preferences that can be configured through the Preferences dialog. Like all parts of KiCad, the preferences for Pcbnew are stored in the user configuration directory and are independent between KiCad minor versions to allow multiple versions to run side-by-side with independent preferences.

The first sections of the Preferences dialog (Common, Mouse and Touchpad, and Hotkeys) are shared between all KiCad programs. These sections are described in detail in the KiCad manual under the “Common preferences” section. Note that even though the Hotkeys section is shared between all programs, there are many Pcbnew-specific hotkeys that only appear in the list when Pcbnew is running.

Display options

Rendering Engine: Controls if Accelerated graphics or Fallback graphics are used.

Grid style: Controls how the alignment grid is drawn.

Grid thickness: Controls how thick grid lines or dots are drawn.

Min grid spacing: Controls the minimum distance, in pixels, between two grid lines. Grid lines that violate this minimum spacing will not be drawn, regardless of the current grid setting.

Snap to grid: Controls when drawing and editing operations will be snapped to coordinates on the active grid. “Always” will enable snapping even when the grid is hidden; “When grid shown” will enable snapping only when the grid is visible.

Cursor shape: Controls whether the editing cursor is drawn as a small crosshair or a full-screen crosshair (a set of lines covering the entire drawing canvas). The editing cursor shows where the next drawing or editing action will occur and will be snapped to a grid location if snapping is enabled.

Always show crosshairs: Controls whether the editing cursor is shown all the time or only when an editing or drawing tool is active.

Net names: Controls whether or not net name labels are drawn on copper objects. These labels are guides for editing only and do not appear in fabrication outputs.

Show pad numbers: Controls whether or not pad number labels are drawn on footprint pads.

Show pad <no net> indicator: Controls whether or not pads with no net are indicated with a special marker.

Track clearance: Controls whether or not clearance outlines around tracks and vias are shown. Clearance outlines are shown as thin shapes around objects that indicate the minimum clearance to other objects, as defined by constraints and design rules.

Show pad clearance: Controls whether or not clearance outlines around pads are shown.

Center view on cross-probed items: When both Eeschema and Pcbnew are running, controls whether clicking a component or pin in Eeschema will center the Pcbnew view on the corresponding footprint or pad.

Zoom to fit cross-probed items: Controls whether the view will be zoomed to show a cross-probed footprint or pad.

Highlight cross-probed nets: Controls whether or not nets highlighted in Eeschema will be highlighted in Pcbnew when the highlight tool is activated in both tools.

Editing options

Flip board items L/R: Controls the direction board items will be flipped when moving them between the top and bottom layers. When checked, items are flipped Left-to-Right (about the Vertical axis); when unchecked, items are flipped Top-to-Bottom (about the Horizontal axis).

Step for rotate commands: Controls how far the selected object(s) will be rotated each time the Rotate command is used.

Allow free pads: Controls whether or not the pads of footprints can be unlocked and edited or moved separately from the footprint.

Magnetic points: This section controls object snapping, also called magnetic points. Object snapping takes precedence over grid snapping when it is enabled. Object snapping only works to objects on the active layer. Hold Shift to temporary disable object snapping.

Snap to pads: Controls when the editing cursor will snap to pad origins.

Snap to tracks: Controls when the editing cursor will snap to track segment endpoints.

Snap to graphics: Controls when the editing cursor will snap to graphic shape points.

Always show selected ratsnest: When enabled, the ratsnest for a selected footprint will always be shown even if the global ratsnest is hidden.

Show ratsnest with curved lines: Controls whether ratsnest lines are drawn straight or curved.

Mouse drag track behavior: Controls the action that will occur when you drag a track segment with the mouse: “Move” will move the track segment independent of any others. “Drag (45 degree mode)” will invoke the push-and-shove router to drag the track, respecting design rules and keeping other track segments attached. “Drag (free angle)” will move the nearest corner of the track segment, highlighting collisions with other objects but not moving them out of the way.

Limit actions to 45 degrees from start Controls whether lines drawn with the graphic drawing tools can take on any angle. Note that this only affects drawing new lines: lines can be edited to take on any angle.

Show page limits: Controls whether or not the page boundary is drawn as a rectangle.

Refill zones after Zone Properties dialog: Controls whether or not zones are automatically refilled after editing the properties of any zone. This may be disabled on complicated designs or slower computers to improve responsiveness.

Colors

Pcbnew supports switching between different color themes to match your preferences. Kicad 6.0 comes with two built-in color themes: “KiCad Default” is a new theme designed to have good contrast and balance for most cases and is the default for new installations. “KiCad Classic” is the default theme from KiCad 5.1 and earlier versions. Neither of these built-in themes can be modified, but you can create new themes to customize the look of Pcbnew as well as install themes made by other users.

Color themes are stored in JSON files located in the colors subdirectory of the KiCad configuration directory. The “Open Theme Folder” button will open this location in your system file manager, making it easy to manage your installed themes. To install a new theme, place it in this folder and restart KiCad. The new theme will be available from the drop-down list of color themes if the file is a valid color theme file.

To create a new color theme, choose New Theme…​ from the drop-down list of color themes. Enter a name for your theme and then begin editing colors. The colors in the new theme will be copied from whatever theme was selected before you created the new theme.

To change a color, double-click or middle-click the color swatch in the list. The “Reset to Default” button will reset that color to its corresponding entry in the “KiCad Default” color theme.

Color themes are saved automatically; all changes are reflected immediately when you close the Preferences dialog. The window on the right side of the dialog shows a preview of how the selected theme will look.

Action plugins

The KiCad PCB editor supports plugins written in Python that can perform actions on the board being edited. These plugins can be installed using the built-in Plugin and Content Manager (see the KiCad chapter for details) or by placing the plugin files inside the user plugins directory. See the Scripting section below for details.

Each plugin that is detected will be shown in a row on this preferences page. Plugins may show a button on the top toolbar of the PCB editor. If the “Show button” control is unchecked for a plugin, it may still be accessed from the Tools > External Plugins menu.

The arrow controls at the bottom of the list allow changing the order that the plugins appear in the toolbar and menu. The folder button will launch a file explorer to the plugin folder, to make installing new plugins easier. The refresh button will scan the plugin folder for any new or removed plugins and update the list.

Origin & axes

Display origin: Determines which coordinate origin is used for coordinate display in the editing canvas. The page origin is fixed at the corner of the page. The drill/place file origin and the grid origin can be moved by the user.

X axis: Controls whether X-coordinates increase to the right or to the left.

Y axis: Controls whether Y-coordinates increase upwards or downwards.

Custom design rules

KiCad’s custom design rule system allows creating design rules that are more specific than the generic rules available in the Constrants page of the Board Setup dialog. Custom design rules have many applications, but in general they are used to apply certain rules to a portion of the board, such as a specific net or netclass, a specific area, or a specific footprint.

Custom design rules are stored in a separate file with the extension kicad_dru. This file is created automatically when you start adding custom rules to a project. If you are using custom rules in your project, make sure to save the kicad_dru file along with the kicad_pcb and kicad_pro files when making backups or committing to a version control system.

The Custom Rules editor

The custom rules editor is located in the Board Setup dialog and provides a text editor for entering custom rules, a syntax checker that will test your custom rules and note any errors, and a syntax help dialog that contains a quick reference to the custom rules language and some example rules.

It is a good idea to use the Check rule syntax button after editing custom rules to make sure there are no syntax errors. Any errors in the custom rules will prevent the design rule checker from running.

Custom rule syntax

The custom design rule language is based on s-expressions and allows you to create design constraints that are not possible with the built-in constraints. Each design rule generally contains a condition defining what objects to match, and a constraint defining the rule to be applied to the matched objects.

The language uses parentheses (( and )) to define clauses of related tokens and values. Parentheses must always be matched: for every ( there must be a matching ). Inside a clause, tokens and values are separated by whitespace. By convention, a single space is used, but any number of whitespace characters between tokens is acceptable. In places where text strings are valid, strings without any whitespace may be quoted with " or ', or unquoted. Strings that contain whitespace must always be quoted. Where nested quotes are required, a single level of nesting is possible by using " for the outer quote character and ' for the inner (or vice versa). Newlines are not required, but are typically used in examples for clarity.

In the syntax descriptions below, items in <angle brackets> represent tokens that must be present and items in [square brackets] represent tokens that are optional or only sometimes required.

The Custom Rules file must start with a version header defining the version of the rules language. As of KiCad 6.0, the version is 1. The syntax of the version header is (version <number>). So in KiCad 6.0 the header should read:

(version 1)

After the version header, you can enter any number of rules. Rules are evaluated in reverse order, meaning the last rule in the file is checked first. Once a matching rule is found for a given set objects being tested, no further rules will be checked. In practice, this means that more specific rules should be later in the file, so that they are evaluated before more general rules.

For example, if you create one rule that limits the minimum clearance between tracks in the net HV and tracks in any other net and a second rule that limits the minimum clearance for all objects inside a certain rule area, make sure the first rule appears later in the custom rules file than the second rule. Otherwise tracks in the HV net could have the wrong clearance if they fall inside the rule area.

Each rule must have a name and one or more constraint clause. The name can be any string and is used to refer to the rule in DRC reports. The constraint defines the behavior of the rule. Rules may also have a condition clause that determines which objects should have the rule applied and an optional layer clause, which specifies which board layers the rule applies to.

(rule <name>
    [(layer <layer_name>)]
    [(condition <expression>)]
    (constraint <constraint_type> [constraint_arguments]))

The custom rules file may also include comments to describe rules. Comments are denoted by any line that begins with the # character (not including whitespace).

# Clearance for 400V nets to anything else
(rule HV
    (condition "A.NetClass == 'HV'")
    (constraint clearance (min 1.5mm)))

Layer Clause

The layer clause determines which layers the rule will work on. While the layer of objects can be tested in the condition clause as described below, using the layer clause is more efficient.

The value of the layer clause can be any board layer name, or the shortcuts outer to match the front and back copper layers (F.Cu and B.Cu) and inner to match any internal copper layers.

If the layer clause is omitted, the rule will apply to all layers.

Some examples:

# Do not allow footprints on back layer (no condition clause means this rule always applies)
(rule "Top side footprints only"
    (layer B.Cu)
    (constraint disallow footprint))
# This rule does the same thing, but is less efficient
(rule "Top side footprints only"
    (condition "A.Layer == 'B.Cu'")
    (constraint disallow footprint))
# Larger clearance on outer layers (inner layer clearance set by board minimum clearance)
(rule "clearance_outer"
    (layer outer)
    (constraint clearance (min 0.25mm)))

Condition Clause

The rule condition is an expression contained inside a text string (and therefore usually surrounded by quotes in order to allow whitespace for clarity). The expression is evaluated against each pair of objects that is being tested by the design rule checker. For example, when checking for clearance between copper objects, each copper object (track segment, pad, via, etc.) on each net is checked against other copper objects on other nets. If a custom rule exists where the expression matches the two given copper objects and the constraint defines a copper clearance, this custom rule could be used to determine the required clearance between the two objects.

The objects being tested are referred to as A and B in the expression language. The order of the two objects is not important because the design rule checker will test both possible orderings. For example, you can write a rule that assumes that A is a track and B is a via. There are some expression functions that test both objects together; these use AB as the object name.

The expression in a condition must resolve to a boolean value (true or false). If the expression resolves to true, the rule is applied to the given objects.

Each object being tested has properties that can be compared, as well as functions that can be used to perform certain tests. The syntax for using properties and functions is <object>.<property> and <object>.<function>([arguments]) respectively.

The object properties and functions are compared using boolean operators to result in a boolean expression. The boolean operators are based on C/C++ syntax, and the following operators are supported:

For example, A.NetClass == 'HV' will apply to any objects that are part of the “HV” netclass and A.NetClass != B.NetClass will apply to any objects that are in different netclasses. Parentheses can be used to clarify the order of operations in complex expressions but they are not required.

Some properties represent a physical measurement, such as a size, angle, length, position, etc. On these properties, unit suffixes can be used in the custom rules language to specify what units are being used. If no unit suffix is used, the internal representation of the property will be used instead (nanometers for distances and degrees for most angles). The following suffixes are supported:

Constraints

The constraint clause of the rule defines the behavior of the rule on the objects that are matched by the condition. Each constraint clause has a constraint type and one or more arguments that set the behavior of the constraint. A single rule may have multiple constraint clauses, in order to set multiple constraints (for example, clearance and track_width) for objects that match the same rule conditions.

Many constraints take arguments that specify a physical measurement or quantity. These constraints support minimum, optimal, and maximum value specification (abbreviated “min/opt/max”). The minimum and maximum values are used for design rule checking: if the actual value is less than the minimum or is greater than the maximum value in the constraint, a DRC error is created. The optimal value is only used for some constraints, and informs KiCad of a “best” value to use by default. For example, the optimal diff_pair_gap is used by the router when placing new differential pairs. No errors will be created if the differential pair is later modified such that the gap between the pair is different from the optimal value, as long as the gap is between the minimum and maximum values (if these are specified). In all cases where a min/opt/max value is accepted, any or all of the minimum, optimal, and maximum value can be specified.

Min/opt/max values are specified as (min <value>), (opt <value>), and (max <value>). For example, a track width constraint may be written as (constraint track_width (min 0.5mm) (opt 0.5mm) (max 1.0mm)) or simply (constraint track_width (min 0.5mm)) if only the minimum width is to be constrained.

Object property and function reference

The following properties can be tested in custom rule expressions:

Common Properties

These properties apply to all PCB objects.

Connected Object Properties

These properties apply to copper objects that can have a net assigned (pads, vias, zones, tracks).

Footprint Properties

Pad Properties

Track and Arc Properties

Via Properties

Zone and Rule Area Properties

These properties apply to copper and non-copper zones, and rule areas (formerly called keepouts).

Graphic Shape Properties

These properties apply to graphic lines, arcs, circles, rectangles, and polygons.

Text Properties

These properties apply to text objects (footprint fields, free text labels, etc).

Expression functions

The following functions can be called on objects in custom rule expressions:

Custom design rule examples

(rule RF_width
    (layer outer)
    (condition "A.NetClass == 'RF'")
    (constraint track_width (min 0.35mm) (max 0.35mm)))
(rule "BGA neckdown"
    (constraint track_width (min 0.2mm) (opt 0.25mm))
    (constraint clearance (min 0.05mm) (opt 0.08mm))
    (condition "A.insideCourtyard('U3')"))
(rule "Distance between Vias of Different Nets"
    (constraint hole_to_hole (min 0.25mm))
    (condition "A.Type =='Via' && B.Type =='Via' && A.Net != B.Net"))
(rule "Distance between test points"
    (constraint courtyard_clearance (min 1.5mm))
    (condition "A.Reference =='TP*' && B.Reference == 'TP*"))
# This assumes that there is a cutout with 1mm thick lines
(rule "Clearance to cutout"
    (constraint clearance (min 0.8mm))
    (condition "A.Layer=='Edge.Cuts' && A.Thickness == 1.0mm"))
(rule "Max Drill Hole Size Mechanical"
    (constraint hole (max 6.3mm))
    (condition "A.Pad_Type == 'NPTH, mechanical'"))
(rule "Max Drill Hole Size PTH"
    (constraint hole (max 6.35mm))
    (condition "A.Pad_Type == 'Through-hole'"))
# Specify an optimal gap for a particular differential pair
(rule "Clock gap"
    (condition "A.inDiffPair('CLK') && AB.isCoupledDiffPair()")
    (constraint diff_pair_gap (opt 0.8mm)))
# Specify a larger clearance between differential pairs and anything else
(rule "Differential pair clearance"
    (condition "A.inDiffPair('*') && !AB.isCoupledDiffPair()")
    (constraint clearance (min 1.5mm)))

Scripting

Scripting allows you to automate tasks within KiCad using the Python language. It is possible to add functionality to KiCad through Python “action plugins” that can be added to the top toolbar. It is also possible to write standalone scripts that interact with KiCad files, for example, to generate fabrication outputs from a board file automatically.

This manual covers general scripting concepts. Users wishing to write or modify scripts should also use the Doxygen documentation located at https://docs.kicad.org/doxygen-python/namespaces.html.

KiCad 6 or newer requires Python 3 for scripting support. Python 2 is no longer supported.

Python script locations

Plugin scripts for the PCB editor can be installed automatically using the Plugin and Content Manager (PCM), or manually by copying the plugin to a folder. Each plugin should be in its own folder within the plugins folder. The location of the plugins folder is by default:

Action plugins

Footprint wizards

The footprint wizards are a collection of python scripts that can be accessed from the Footprint Editor. If you invoke the footprint dialog you select a given wizard that allows you to see the footprint rendered, and you have some parameters you can edit.

If the plugins are not properly distributed to your system package, you can find the latest versions in the KiCad source tree at gitlab.

Using the scripting console

Pcbnew comes with a built-in Python console that can be used to inspect and interact with the board. To launch the console, use the icon in the top toolbar. The Pcbnew Python API is not automatically loaded, so to load it, type import pcbnew into the console. The command pcbnew.GetBoard() will then return a reference to the board currently loaded in Pcbnew, which can be inspected and modified through the console.

Writing external scripts

Writing action plugins