When Pcbnew is run for the first time, if the global footprint table file fp-lib-table is not found in the KiCad configuration folder then Pcbnew will ask how to create this file:

The default footprint library table includes all of the standard footprint libraries that are installed as part of KiCad.

The main Pcbnew user interface is shown above, with some key elements indicated:

The editing canvas is a view onto the board being designed. You can pan and zoom to different areas of the board, and also flip the view to show the board from the bottom.

By default, dragging with the middle or right mouse button will pan the canvas view and scrolling the mouse wheel will zoom the view in or out. You can change this behavior in the Mouse and Touchpad section of the preferences (see Configuration and Customization for details).

The hotkeys described in this manual use the key labels that appear on a standard PC keyboard. On an Apple keyboard layout, use the Cmd key in place of Ctrl, and the Option key in place of Alt.

Layers in Pcbnew represent physical copper layers on a board, as well as graphical layers used for defining things such as silkscreen, solder mask, and the board edge. There is always one layer that is active in the editor. The active layer is drawn on top of other layers and will be the layer assigned to newly-created objects. The active layer is indicated in the layer selector drop-down box in the top toolbar and is also highlighted in the appearance panel. To change the active layer, you can left-click a layer name in the appearance panel, use the drop-down layer selector in the top toolbar, or use a hotkey. Layers can be hidden to simplify the board view. You can hide a layer even if it is the active layer.

The appearance panel provides controls to manage the visibility, color, and opacity of objects in the Pcbnew drawing canvas. It has three tabs: the Layers tab contains controls for the board layers, the Objects tab contains controls for different types of graphical objects, and the Nets tab contains controls for the appearance of the ratsnest and copper items.

Selecting items in the editing canvas is done with the left mouse button. Single-clicking on an object will select it and dragging will perform a box selection. A box selection from left to right will only select items that are fully inside the box. A box selection from right to left will select any items that touch the box. A left-to-right selection box is drawn in yellow and a right-to-left selection box is drawn in blue.

The selection action can be modified by holding modifier keys while clicking or dragging. The following modifier keys apply when clicking to select single items:

The following modifier keys apply when dragging to perform a box selection:

The selection filter panel in the lower right corner of the Pcbnew window controls which types of objects can be selected with the mouse. Turning off selection of unwanted object types makes it easier to select items in a dense board. The "All items" checkbox is a shortcut to turn the other items on and off. The "Locked items" checkbox is independent of the rest, and controls whether or not items that have been locked can be selected. You can right-click any object type in the selection filter to quickly change the filter to only allow selecting that type of object.

When a connected copper item is selected, you can expand the selection to other copper items of the same net using the Expand Selection command in the right-click context menu or with the hotkey U. The first time you run this command, the selection will be expanded to the nearest pad. The second time, the selection will be expanded to all connected items on all layers.

Pressing Esc will always cancel the current tool or operation and return to the selection tool. Pressing Esc while the selection tool is active will clear the current selection.

An electrical net (or set of nets) can be highlighted in the PCB editor to visualize how the net is routed across the PCB. Net highlighting can be activated by selecting the net to highlight in the PCB editor or by selecting the corresponding net in the schematic editor when cross-probe highlighting is enabled (see below). When net highlighting is active, the highlighted net or nets will be shown in a brighter color and all other items will be shown in a dimmer color than normal.

There are three ways to select a net or nets to highlight in the PCB editor: by using the hotkey ` after selecting a copper object, by using the context menu of any copper object, and the context menu of the Nets tab of the Appearance panel. When you press the Highlight Net hotkey, the nets of any selected copper items will be highlighted. If no copper items are selected, the net of the copper item under the editor cursor will be highlighted. If there is no copper item under the cursor, any existing highlighting will be cleared. The highlighting can also be cleared by using the Clear Highlight action (hotkey ~).

When a net or nets have been selected for highlighting, the Toggle Net Highlighting action becomes enabled on the left toolbar (also accessible by hotkey, Ctrl+`). This action will turn the highlighting display on or off without choosing a new net to highlight.

KiCad allows bi-directional cross-probing between the schematic and the PCB. There are several different types of cross-probing.

Selection cross-probing allows you to select a symbol or pin in the schematic to select the corresponding footprint or pad in the PCB (if one exists) and vice-versa. By default, cross-probing will result in the display centering on the cross-probed item and zooming to fit. This behavior can be disabled in the Display Options section of the Preferences dialog.

Highlight cross-probing allows you to highlight a net in the schematic and PCB at the same time. If the option "Highlight cross-probed nets" is enabled in the Display Options section of the Preferences dialog, highlighting a net or bus in the schematic editor will cause the corresponding net or nets to be highlighted in the PCB editor.

The left toolbar provides options to change the display of items in Pcbnew.

A printed circuit board in KiCad is generally made up of footprints representing electronic components and their pads, nets defining how those pads connect to each other, tracks, vias, and filled zones that form the copper connections between pads in each net, and various graphic shapes defining the board edge, silkscreen markings, and any other desired information.

KiCad normally keeps the information about nets on a PCB synchronized with an associated schematic, but nets can also be created and edited directly within the PCB editor.

KiCad is capable of creating printed circuit boards with up to 32 copper layers, 14 technical layers (silkscreen, solder mask, component adhesive, solder paste, etc), and 13 general-purpose drawing layers.

The internal measurement resolution of all objects in KiCad is 1 nanometer, and measurements are stored as 32-bit integers. This means it is possible to create boards up to appproximately 4 meters by 4 meters.

KiCad currently supports one board file per project / schematic.

Creating a board from a schematic is the recommended workflow for KiCad. When you create a new project, KiCad will generate an empty board file with the same name as the project. To start designing the board after you have created a schematic, simply open the board file. You can do this either from the KiCad project manager, or by clicking the "Open PCB in board editor" button in the schematic editor. To import the schematic design information into the board editor, including footprints and net connections, use the Tools → Update Schematic from PCB…​ action (F8). You can also use the icon in the top toolbar.

The tool adds the footprint for each symbol to the board and transfers updated schematic information to the board. In particular, the board’s net connections are updated to match the schematic.

The changes that will be made to the PCB are listed in the Changes To Be Applied pane. The PCB is not modified until you click the Update PCB button.

You can show or hide different types of messages using the checkboxes at the bottom of the window. A report of the changes can be saved to a file using the Save…​ button.

It is also possible to create a board with no matching schematic, although this workflow has some limitations and is not recommended for most users. To do this, you must start the PCB editor standalone (not from the KiCad project manager). Before beginning your design, it is a good idea to save the board file, which will also create a project file to store board settings. Use "Save As…​" from the File menu to choose where to save your board file. A project file with the same name will be created in the same location you choose to save the board file in.

Before beginning your board design, use the Board Setup dialog to configure the basic parameters of the board. To open Board Setup, click the icon in the top toolbar or choose "Board Setup…​" from the File menu.

Placement and drawing tools are located in the right toolbar. When a tool is activated, it stays active until a different tool is selected or the tool is canceled with the Esc key. The selection tool is always activated when any other tool is canceled.

Some toolbar buttons have more than one tool available in a palette. These tools are indicated with a small arrow in the lower-right corner of the button:

To show the palette, you can click and hold the mouse button on the tool or click and drag the mouse. The palette will show the most recently used tool when it is closed.

When moving, dragging, and drawing board elements, the grid, pads, and other elements can have snapping points depending upon the settings in the user preferences. In complex designs, snap points can be so close together that it makes the current tool action difficult. Both grid and object snapping can be disabled while moving the mouse by using the modifier keys in the table below.

All objects have properties that are editable in a dialog. Use the hotkey E or select Properties from the right-click context menu to edit the properties of selected item(s). You can only open the properties dialog if all the items you have selected are of the same type. To edit the properties of different types of items at one time, see the section below on bulk editing tools.

In properties dialogs, any field that contains a numeric value can also accept a basic math expression that results in a numeric value. For example, a dimension may be entered as 2 * 2mm, resulting in a value of 4mm. Basic arithmetic operators as well as parentheses for defining order of operations are supported.

The properties of each individual pad of a footprint can be inspected and edited after placing the footprint on the board. In other words, it is possible to override the design of an individual footprint pad in a specific instance of the footprint on the board, if the footprint design in the library is not appropriate. For example, you may wish to remove the solder paste aperture for a pad that needs to remain unsoldered in a specific design, or you may wish to move the location of a through-hole pad for an axial-lead resistor in order to fit a specific design.

The pad properties dialog is opened through the context menu or default hotkey E when a pad is selected. Note that KiCad assumes that if you click near a pad, you are probably trying to select the entire footprint rather than a single pad. To select a single pad, make sure to click inside the pad area, or turn off the Footprints setting in the selection filter (and make sure the Pads setting is turned on) to prevent accidental selection of the entire footprint rather than a specific pad.

The General tab of the pad properties dialog shows the physical properties of the pad, including its geometry, shape, and layer settings.

Pad type: this setting controls which features are enabled for the pad:

SMD pads are electrically-connected and have no hole. In other words, they exist on a single copper layer.

Through-hole pads are electrically-connected and have a plated hole. The hole exists on every layer, and the copper pad exists on multiple layers (see Copper layers setting below).

Edge Connector pads are SMD pads that are allowed to overlap the board outline on the Edge.Cuts layer.

NPTH, Mechanical pads are non-plated through holes that do not have an electrical connection.

SMD Aperture pads are pads that have no hole and no electrical connection. These can be used to add specific designs to a technical layer, for example a paste or solder mask aperture.

The Copper layers setting controls which copper layers will have a shape associated with the pad.

For SMD pads, the options are F.Cu or B.Cu, controlling whether the pad sits on the front or the back of the board relative to the footprint’s location. In other words, if a pad is set to exist on B.Cu in its properties, and the footprint is flipped to the back of the board, that pad will now exist on F.Cu, because it also has been flipped.

For through-hole pads, it is possible to remove the pad shape from copper layers where the pad is not electrically connected to other copper (tracks or filled zones). Setting the copper layers to connected layers only will remove the pad shape from any unconnected layers, and setting to F.Cu, B.Cu, and connected layers will remove the pad shape from any internal unconnected layers. This can be useful in dense board designs to increase the routable area on internal layers.

The Technical layers checkboxes control which technical layers will have an aperture added with the pad’s shape. By default, pads have apertures on the paste and mask layers matching their copper layer.

Specify pad to die length: This setting allows a length to be associated with this pad that will be added to the routed track length by the track length tuning tools and the Net Inspector. This can be used to specify internal bondwire lengths for more accurate length matching, or in other situations where the electrical length of a net is longer than the length of the routed tracks on the board.

The aperture appearing on any technical layer will have the same shape and size as the pad shape on the copper layer(s). In the PCB manufacturing process, the manufacturer will often change the relative size of mask and paste apertures relative to the copper pad size, but since this size change is specific to a manufacturing process, most manufacturers expect the design data to be provided with the apertures set to the same size as the copper pads. For specific situations where you need to oversize or undersize a technical layer aperture in the design data, you can use the settings in the Overrides tab.

Pad clearance controls the minimum clearance between the pad and any copper shape (tracks, vias, pads, zones) on a different net. This value is normally set to 0 which will cause the pad clearance to be inherited from any clearance override set on the footprint, or the board’s design rules and netclass rules if the footprint clearance is also set to 0.

Solder mask clearance controls the size difference between the pad shape and the aperture shape on the F.Mask and B.Mask layers. A positive number means the solder mask aperture will be larger than the copper shape. This number is an inflation applied to all directions. For example, a value of 0.1mm here will cause the solder mask aperture to be inflated by 0.1mm, meaning that there will be an 0.1mm border on all sides of the pad and the solder mask opening will be 0.2mm wider than the pad when measured along a given axis.

Solder paste absolute clearance controls the size difference between the pad shape and the aperture shape on the F.Paste and B.Paste layers. Its behavior is otherwise identical to the behavior of the solder mask clearance setting.

Solder paste relative clearance allows setting a solder paste clearance value as a percentage of the pad size rather than an absolute distance value. If both relative and absolute clearances are specified, they are added together to determine the solder paste aperture size.

The Overrides tab also has controls for how the pad connects to any copper zone that overlaps it and shares its net.

Pad connection controls whether the pad will have a solid, thermal relief, or no connection to the zone. Like the other overrides, this one may be set for an individual pad or for an entire footprint. The default setting for this control is From parent footprint, and the default footprint setting is to use the connection mode specified in the zone properties.

Thermal relief spoke width controls the width of the spokes generated when the zone connection mode is Thermal Relief.

Thermal relief gap controls the length of the thermal spokes, or the gap between the pad’s shape and the filled copper area of the zone.

Custom pad shape in zone controls the behavior of the zone filler when the pad uses a custom shape rather than one of the default shapes. This can be used to achieve different results when using thermal reliefs and custom pad shapes.

Copper zones, also sometimes called copper pours or fills by other EDA tools, are solid or hatched areas of copper assigned to a particular net that automatically keep clearance from other copper objects. Zones are commonly used to fill in all free space on a board layer (or a portion of a layer) in order to create ground and power planes, carry high currents, or to provide shielding.

Zones are defined by a polygonal outline that defines the maximum extent of the filled copper area. This outline does not represent physical copper and will not appear in exported manufacturing data. The actual copper areas of the zone must be filled each time the outline, or any objects inside the outline, are modified. The filling process may be run on a single zone, or on all zones in a board (default hotkey B). Zones may be unfilled (default hotkey Ctrl+B) to improve performance and reduce visual clutter while editing large boards.

To draw a zone, click the Add Filled Zone tool () on the right toolbar, or use default hotkey Ctrl+Shift+Z. Click to choose the first point of the zone outline. The Zone Properties dialog will appear, allowing you to choose the zone net and other properties. These properties may be edited at any time, so it is not critical to choose them all correctly at first. Accept the dialog and continue placing points to define the zone outline. To finish the zone, double-click to set the last point. Zone outline points may be modified like graphic polygons, by dragging the square handles to move a corner or dragging the circular handles to move an edge. To edit the zone’s properties, use hotkey E or select Properties from the context menu.

Layer: A single zone object can create filled copper on one or more copper layers. Check the box next to each copper layer that this zone outline should fill on. The copper on each layer will be filled independently, but all layers will share the same net.

Net: Select the electrical net that the zone copper should be connected to. It is possible to create zones with no net assignment. Zones with no net will keep clearance from any copper objects on any net.

Zone name can be used to assign a specific name to a zone. This name can be used to refer to the zone in custom DRC rules.

Zone priority level determines the order in which multiple zones on a single layer are filled. The highest priority level zone on a given layer will be filled first. Lower-priority zones will keep clearance to the filled areas of higher-priority zones. Two zones on the same layer with the same priority level will overlap (short-circuit) with each other.

Constrain outline to H, V and 45 degrees controls the initial behavior of the zone outline drawing tool. When this option is enabled, the zone outline will be restricted to 45-degree angles. Note that after the zone outline has been created, this option has no effect. Outline points may be modified freely after creation.

Locked controls whether or not the zone outline object is locked. Locked objects may not be manipulated or moved, and cannot be selected unless the Locked Items option is enabled in the Selection Filter panel.

Outline display controls how the zone outline is drawn on screen. In Line mode, only the border lines of the outline are drawn. In Hatched mode, hatch lines are drawn on the inside of the outline border for a short distance, to make the zone outline more apparent. In Fully Hatched mode, hatch lines are drawn across the entire inside of the zone outline.

Corner smoothing controls the behavior of the filled copper areas at corners of the outline. Corners can be smoothed by a chamfer or fillet, or can extend all the way to the outline corner if smoothing is disabled.

Clearance controls the minimum clearance the filled areas of this zone will keep from other copper objects. Note that if two clearance values are in conflict, the larger clearance value will be used. For example, if a zone is set to use 0.2mm clearance but its netclass is set to use 0.3mm clearance, the result will be an 0.3mm clearance.

Minimum width controls the minimum size of narrow necks of copper created inside the zone. Any copper areas that would be below this minimum width are removed during the filling process.

Pad connection controls the way that the filled zone areas will connect to footprint pads on the same net. Solid connections will result in the copper completely overlapping the pads. Thermal reliefs will result in small copper spokes connecting the pad to the rest of the copper zone, increasing the thermal resistance between the pad and the rest of the zone. This can be useful for hand soldering. Reliefs for PTH will apply thermal reliefs to plated through-hole pads and use solid connections for surface mount pads. None will result in the zone not connecting to any pads on the same net.

Thermal relief gap controls the distance maintained between any pad and the copper zone when the pad connection mode is set to generate thermal reliefs.

Thermal spoke width controls the width of the "spokes", or short copper segments connecting the pad to the rest of the copper zone.

Fill type controls how the copper zone is filled: the default is solid fill, which will result in copper filling in all available space within the zone outline. The zone can also be set to fill a hatch pattern, which will fill the area with a pattern that contains less copper. This can be useful for flexible printed circuits and other specialty applications.

Orientation controls the angle of the hatch pattern lines. An orientation of 0 degrees will result in the hatch pattern using horizontal and vertical lines.

Hatch width controls the width of each line in the hatch pattern.

Hatch gap controls the distance between each line in the hatch pattern.

Smoothing effort controls the style of smoothing applied to the hatch pattern. A value of 0 will result in no smoothing, and a value of 3 will result in the finest smoothing. Higher values will result in longer processing time and larger Gerber files.

Smoothing amount is a ratio that controls the size of the smoothing chamfers or fillets that are generated when smoothing effort is set to a value other than 0. An amount of 0.0 results in no smoothing, and a value of 1.0 results in maximum smoothing (in other words, a chamfer or fillet equal to half of the hatch gap).

Remove islands controls the behavior of isolated copper areas, also called islands, after the initial zone fill. When this is set to always, isolated areas inside the zone are removed. When set to never, isolated areas are left alone, and will result in copper areas that are not connected to the rest of the net. When set to below area limit, a minimum island size can be specified, and islands below this threshold will be removed.

Graphical objects (lines, arcs, rectangles, circles, polygons, and text) can exist on any layer but cannot be assigned to a net. Rectangles, circles, and polygons can be set to be filled or outlines in their properties dialogs. The line width property will control the width of the outline even for filled shapes. Line width can be set to 0 for filled shapes to disable the outline.

Dimensions are graphical objects used to show a measurement or other marking on a board design. They may be added on any drawing layer, but are normally added to one of the User layers. KiCad currently supports four different types of dimension: aligned, orthogonal, center, and leader.

Aligned dimensions () show a measurement of distance between two points. The measurement axis is the line that connects those two points, and the dimension graphics are kept parallel to that axis.

Orthogonal dimensions () also measure the distance between two points, but the measurement axis is either the X or Y axis. In other words, these dimensions show the horizontal or vertical component of the distance between two points. When creating orthogonal dimensions, you can select which axis to use as the measurement axis based on where you place the dimension after selecting the two points to measure.

Center dimensions () create a cross mark to indicate a point or the center of a circle or arc.

Leader dimensions () create an arrow with a leader line connected to a text field. This text field can contain any text, and an optional circular or rectangular frame around the text. This type of dimension is often used to call attention to parts of the design for reference in fabrication notes.

After creating a dimension, its properties may be edited (hotkey E) to change the format of the displayed number and the style of the text and graphic lines.

KiCad features an interactive router that:

By default, the router respects the configured design rules when placing tracks: the size (width) of new tracks will be taken from the design rules and the router will respect the copper clearance set in the design rules when determining where new tracks and vias can be placed. It is possible to disable this behavior if desired by using the Highlight Collisions router mode and turning on the Allow DRC Violations option in the router settings (see below).

The router has three modes that can be selected at any time. The router mode is used for routing new tracks, but also when dragging existing tracks using the Drag (hotkey D) command. These modes are:

Which mode to use is a matter of preference. For most users, we recommend using Shove mode for the most efficient routing experience or Walk Around mode if you do not want the router to modify tracks that are not being routed. Note that Shove and Walk Around modes always create horizontal, vertical, and 45-degree (H/V/45) track segments. If you need to route tracks with angles other than H/V/45, you must use Highlight Collisions mode and enable the Free Angle Mode option in the Interactive Router Settings dialog.

There are five main routing functions: Route Single Track, Route Differential Pair, Tune length of a single track, Tune length of a differential pair, and Tune skew of a differential pair. All of these are present in both the Route menu dropdown (individually) on the top toolbar and the drawing toolbar in two overloaded icons on the drawing toolbar on the right. The use of the overloaded icons is described above. One is for the two Route functions and one is for the three Tune functions. In addition, the Route menu allows the selection of Set Layer Pair and Interactive Router Settings.

To route tracks, click the Route Tracks icon (from the drawing toolbar or from the top toolbar under Route) or use the hotkey X. Click on a starting location to select which net to route and begin routing. The net being routed will automatically be highlighted and the allowable clearance for the net will be indicated with a gray outline around the tracks being routed. The clearance outline can be disabled by changing the Clearance Outlines setting in the Display Options section of the Preferences dialog.

When the router is active, new track segments will be drawn from the routing start point to the editor cursor. These tracks are unfixed temporary objects that show what tracks will be created when you use a left-click or the Enter key to fix the route. The unfixed track segments are shown in a brighter color than the fixed track segments. When you exit the router using the Esc key or by selecting another tool, only the fixed track segments will be saved. The Finish Route action (hotkey End) will fix all tracks and exit the router.

While you are routing, you can use the Undo Last Segment command (hotkey Backspace) to unfix the tracks you most recently fixed. You can use this command repeatedly to step back through the route that you have already fixed.

In previous versions of KiCad, using the left mouse button or Enter to fix the routed segments would fix all segments up to but not including the segment ending at the mouse cursor location. In KiCad 6, this behavior is now optional, and by default, all segments including the one ending at the mouse cursor location will be fixed. The old behavior can be restored by disabling the "Fix all segments on click" option in the Interactive Router Settings dialog.

While routing, you can hold the Ctrl key to disable grid snapping, and hold the Shift key to disable snapping to objects such as pads and vias.

Most objects can be locked through their properties dialogs, by using the right-click context menu, or by using the Toggle Lock hotkey (L). Locked objects cannot be selected unless the "Locked items" checkbox is enabled in the selection filter. Attempting to move locked items will result in a warning dialog:

Selecting "Override Locks" in this dialog will allow moving the locked items. Selecting "OK" will allow you to move any unlocked items in the selection; leaving the locked items behind. Selecting "Do not show again" will remember your choice for the rest of your session.

The measurement tool allows you to make distance and angle measurements between points on the PCB. To activate the tool, click the icon in the right toolbar, or use the hotkey Ctrl+Shift+M. Once the tool is active, click once to set the measurement start point, then click again to finish a measurement.

The design rule checker is used to verify that the PCB meets all the requirements established in the Board Setup dialog and that all pads are connected according to the netlist or schematic. KiCad can automatically prevent some design rule violations while routing tracks, but many others cannot be prevented automatically. This means it is important to use the design rule checker before creating manufacturing files for a PCB.

To use the design rule checker, click the icon in the top toolbar, or select Design Rules Checker from the Inspect menu.

The top section of the DRC Control window contains some options that control the design rule checker:

Refill all zones before performing DRC: when enabled, zones will be refilled every time the design rule checker is run. Disabling this option may result in incorrect DRC results if zones have not been refilled manually.

Report all errors for each track: when enabled, all clearance errors will be reported for each track segment. When disabled, only the first error will be reported. Enabling this option will result in the design rule checker running more slowly.

Test for parity between PCB and schematic: when enabled, the design rule checker will test for differences between the schematic and PCB in addition to testing the PCB design rules. This option has no effect when running the PCB editor in standalone mode.

After running DRC, any violations will be shown in the center part of the DRC Control window. Rule violations, unconnected items, and differences between the schematic and the PCB are shown in three different tabs. The controls below the list of violations can be used to show or hide violations depending on their severity. A report file in plain text format can be created after running DRC using the Save button.

Each violation involves one or more object on the PCB. In the list of violations, the objects involved are listed below the violation. Clicking on the violation in the list view will move the PCB Editor view so that the affected area is centered. Clicking on one of the objects involved in a violation will highlight the object.

Right-clicking a violation in the list view will open a context menu with additional actions including excluding the selected violation. Excluded violations are hidden unless the Exclusions checkbox is enabled at the bottom of the DRC Control window. Excluded violations are remembered between runs of the design rule checker.

The Net Inspector allows you to view statistics about all the nets in a board. To open the inspector, click the icon at the top of the Nets section of the Appearance panel, or select Net Inspector from the Inspect menu.

Clicking a net in the list will highlight that net on the board. Clicking a column title allows you to sort the list of nets by that column.

The Group By field allows you to combine different nets together and view the total length of the combined nets. For example, if you have two nets named DATA0 and DATA0_EXT, using a Group By value of DATA0* will create a group containing both nets. More complicated groupings can be created by changing the Group By mode from Wildcard to RegEx (regular expressions). The substring (Substr) variants of the Group By mode will create groups for each set of nets that matches the pattern differently.

For example, if you have the nets U1D+, U1D-, U2D+, and U2D-, the grouping pattern U*D will match all four nets in Wildcard mode, creating a single group U*D. In Wildcard Substr mode, it will match all four nets, but create two different groups: U1D and U2D.

Pad Count and Via Count show the number of pads (surface mount and through hole) and vias on a net. Via Length shows the total height of each via (not accounting for which copper layers the via connects to). In other words, Via Length is equal to Via Count multipled by the stackup height of the board. Track Length shows the total length of all track segments in a net, not accounting for topology. Die length shows the total of all Pad to Die Length values set for pads on the net.

KiCad uses Gerber files as its primary plotting format for PCB manufacturing. To create Gerber files, open the Plot dialog from the File menu, or select Gerbers from the Fabrication Outputs section of the File menu. The Plot dialog will open, allowing you to configure and generate Gerber files.

KiCad can generate CNC drilling files required by most PCB manufacturing processes in either Excellon or Gerber X2 format. KiCad can also generate a drill map: a graphical plot of the board showing drill locations. Select the Generate Drill Files option from the Fabrication Outputs menu to open the dialog:

Output folder: Choose the folder to save generated drill and map files to. If a relative path is entered, it will be relative to the project directory.

Drill file format: Choose whether to generate Excellon drill files (required by most PCB manufacturers) or Gerber X2 files.

Mirror Y axis: For Excellon files, choose whether or not to mirror the Y-axis coordinate. This option should in general not be used when having PCBs manufactured by a third party, and is provided for convenience for users who are making PCBs themselves.

Minimal header: For Excellon files, choose whether to output a minimal header rather than a full file header. This option should not be enabled unless requested by your manufacturer.

PTH and NPTH in single file: By default, plated holes and non-plated holes will be generated in two different Excellon files. With this option enabled, both will be merged into a single file. This option should not be enabled unless requested by your manufacturer.

Oval holes drill mode: Controls how oval holes are represented in an Excellon drill file. The default setting, Use route command, is correct for most manufacturers. Only choose the Use alternate drill mode setting if requested by your manufacturer.

Map file format: Choose the output format for plotting a drill map.

Drill origin: Choose the coordinate origin for drill files. Absolute will use the page origin at the top left corner. Drill/place file origin will use the origin specified in the board design.

Drill units: Choose the units for drill coordinates and sizes.

Zeros format: Controls how numbers are formatted in an Excellon drill file. Select an option here based on your manufacturer’s recommendations.

Component placement files are text files that list each component (footprint) on the board along with its center position and orientation. These files are usually used for programming pick-and-place machines, and may be required by your manufacturer if you are ordering fully-assembled PCBs.

Format: Choose between generating a plain text (ASCII), comma-separated text (CSV), or Gerber placement file format.

Units: Choose the units for component locations in the placement file.

Files: Choose whether to generate separate files for footprints on the front and back of the board or a single file combining both sides.

Include only SMD footprints: When enabled, only footprints with the SMD fabrication attribute will be included. Check with your manfuacturer to determine if non-SMD footprints should be included or excluded from the position file.

Exclude all footprints with through hole pads: When enabled, footprints will be excluded from the placement file if they contain any through-hole pads, even if their fabrication type is set to SMD.

Include board edge layer: For Gerber placement files, controls whether or not the board outline is included with the footprint placement data.

Use drill/place file origin: When enabled, component positions will be relative to the drill/place file origin set in the board design. When disabled, the positions will be relative to the page origin (upper left corner).

KiCad can also generate footprint report files, IPC-D-356 netlist files, and a bill of materials (BOM) from the board design. These output formats have no configurable options.

KiCad can print the board view to a standard printer using the Print action in the File menu.

Included layers: Select the layers to include in the printout. Unselected layers will be invisible.

Output mode: Choose whether to print in black and white or full color.

Print border and title block: When enabled, the page border and title block will be printed.

Print according to objects tab of appearance manager: When enabled, any objects that have been hidden in the Objects tab of the Appearance panel will be hidden in the printout. When disabled, these objects will be printed if the layer they appear on is selected in the Included Layers area.

Print background color: When printing in full color, this option controls whether or not the view background color will be printed.

Use a different color theme for printing: When printing in full color, this option allows a different color theme to be used for printing. When disabled, the color theme used by the board editor will be used for printing.

Drill marks: Controls whether to show drilled holes at their actual size, at a small size, or hide them from the printout.

Print mirrored: When enabled, the printout will be mirrored horizontally.

Print one page per layer: When enabled, each layer selected in the Included Layers area will be printed to an individual page. If this option is enabled, the Print board edges on all pages option controls whether to add the Edge.Cuts layer to each printed page.

Scale: controls the scale of the printout relative to the page size configured in Page Setup.

KiCad can export a board design to various third-party formats for use with external software. These functions are found in the Export section of the File menu.

Specctra .DSN: creates a file suitable for importing into certain third-party autorouter software. This exporter has no configurable options.

Hyperlynx: creates a file suitable for importing into Mentor Graphics (Siemens) HyperLynx simulation and analysis software.

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.

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.

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.