Editing a board

Placement and drawing operations

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.

Snapping

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.

Editing object properties

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.

Working with footprints

Working with pads

Working with zones

Graphical objects

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.

Creating graphical shapes

Creating text objects

Graphical text may be placed by using the () icon in the right toolbar or by keyboard shortcut Ctrl+Shift+T. Click to place the text origin, and then edit the text and its properties in the dialog that will appear:

Text may be placed on any layer, but note that text on copper layers cannot be associated with a net and cannot form connections to tracks or pads. Copper zones will fill around the rectangular bounding box of text objects.

Board outlines (Edge Cuts)

KiCad uses graphical objects on the Edge.Cuts layer to define the board outline. The outline must be a continuous (closed) shape, but can be made up of different types of graphical object such as lines and arcs, or be a single object such as a rectangle or polygon. If no board outline is defined, or the board outline is invalid, some functions such as the 3D viewer and some design rule checks will not be functional.

Dimensions

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.

Dimension format options

Override value: When enabled, you may enter a measurement value directly into the Value field that will be used instead of the actual measured value.

Prefix: Any text entered here will be shown before the measurement value.

Suffix: Any text entered here will be shown after the measurement value.

Layer: Selects which layer the dimension object exists on.

Units: Selects which units to display the measured value in. Automatic units will result in the dimension units changing when the display units of the board editor are changed.

Units format: Select from several built-in styles of unit display.

Precision: Select how many digits of precision to display.

Dimension text options

Most of the dimension text options are identical to those options available for other graphical text objects (see the Graphical Objects section above). Some specific options for dimension text are also available:

Position mode: Choose whether to postion the dimension text manually, or to automatically keep it aligned with the dimension measurement lines.

Keep aligned with dimension: When enabled, the orientation of the dimension text will be adjusted automatically to keep the text parallel with the measurement axis.

Dimension line options

Line thickness: Sets the thickness of the graphical lines that make up a dimension’s shape.

Extension line offset: Sets the distance from the measurement point to the start of the extension lines.

Arrow length: Sets the length of the arrow segments of the dimension’s shape.

Leader options

Value: Enter the text to show at the end of the leader line.

Text frame: Select the desired border around the text (circle, rectangle, or none).

Routing tracks

KiCad features an interactive router that:

• Allows manual or guided (semi-automatic) routing of single tracks and differential pairs.

• Enables modifications of existing designs by:

  • Re-routing existing tracks when they are dragged

  • Re-routing tracks attached to footprint pads when the footprint is dragged

• Allows tuning of track lengths and differential pair skew (phase) by inserting serpentine
  tuning shapes for designs with tight timing requirements

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:

• Highlight Collisions: in this mode, most of the router features are disabled and routing is fully manual. When routing, collisions (clearance violations) will be highlighted in green and the newly-routed tracks cannot be fixed in place if there is a collision unless the Allow DRC Violations option is turned on. In this mode, up to two track segments may be placed at a time (for example, one horizontal and one diagonal segment).

• Shove: in this mode, the track being routed will walk around obstacles that cannot be moved (for example, pads and locked tracks/vias) and shove obstacles that can be moved out of the way. The router prevents DRC violations in this mode: if there is no way to route to the cursor position that does not violate DRC, no new tracks will be created.

• Walk Around: in this mode, the router behaves the same as in Shove mode, except no obstacles will be moved out of the way.

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.

Track posture

When routing in H/V/45 mode, the posture refers to how a set of two track segments connect two points that cannot be reached by a single H/V/45-degree segment. In such a case, the points will be connected by one horizontal or vertical segment and one diagonal (45-degree) segment. The posture refers to the order of these segments: whether the horizontal/vertical segment or the diagonal segment comes first.

KiCad’s router attempts to pick the best posture automatically based on a number of factors. In general, the router will attempt to minimize the number of corners in a route, and will avoid “bad” corners such as acute angles whenever possible. When routing from or to a pad, KiCad will choose the posture that lines up the route with the longest edge of the pad.

In some cases, KiCad cannot guess the posture you intend correctly. To switch the posture of the track while routing, use the Switch Track Posture command (hotkey /).

In situations where there is no obvious “best” posture (for example, when starting a route from a via), KiCad will use the movement of your mouse cursor to select the posture. If you would like the route to begin with a straight (horizontal or vertical) segment, move the mouse away from the starting location in a mostly horizontal or vertical direction. If you would like the route to begin diagonally, move in a diagonal direction. Once the cursor is a sufficient distance away from the routing start location, the posture is “locked” and will no longer change unless the cursor is brought back to the starting location. Detection of posture from the movement of the mouse cursor can be disabled in the Interactive Router Settings dialog as described below.

Track corner mode

KiCad’s router can place tracks with either sharp or rounded (arc) corners when routing in H/V/45 mode. To switch between sharp and rounded corners, use the Track Corner Mode command (hotkey Ctrl+/). When routing with rounded corners, each routing step will place either a straight segment, a single arc, or both a straight segment and an arc. The track posture determines whether the arc or the straight segment will be placed first.

Track corners can also be rounded after routing by using the Fillet Tracks command after selecting the desired tracks.

Track width

The width of the track being routed is determined in one of three ways: if the routing start point is the end of an existing track and the button on the top toolbar is enabled, the width will be set to the width of the existing track. Otherwise, if the track width dropdown in the top toolbar is set to “use netclass width”, the width will be taken from the netclass of the net being routed (or from any custom design rules that specify a different width for the net, such as inside a neckdown area). Finally, if the track width dropdown is set to one of the pre-defined track sizes configured in the Board Setup dialog, this width will be used.

KiCad’s router supports a single track width for the active route. In other words, to change widths in the middle of a track, you must end the route and then restart a new route from the end of the previous route. To change the width of the active route, use the hotkeys W and Shift+W to step through the track widths configured in the Board Setup dialog.

Placing vias

While routing tracks, switching layers will insert a through via at the end of the current (unfixed) track. Once you place the via, routing will continue on the new layer. There are several ways to select a new layer and insert a via:

• By using the hotkey to select a specific layer, such as PgUp to select F.Cu or PgDn to select B.Cu.

• By using the “next layer” or “previous layer” hotkeys (+ and -).

• By using the “Place Via” hotkey (V), which will switch to the next layer in the active layer pair.

• By using the Select Layer and Place Through Via action (hotkey <), which will open a dialog to select the target layer.

The size of the via will be taken from the active Via Size setting, accessible from the drop-down in the top toolbar or the Increase Via Size (‘) and Decrease Via Size (\) hotkeys. Much like track width, when the via size is set to “use netclass sizes”, the via sizes configured in the Net Classes section of the Board Setup will be used (unless overridden by a custom design rule).

If microvias or blind/buried vias are enabled in the Constraints section of the Board Setup dialog, these vias can be placed while routing. Use the hotkey Ctrl+V to place a microvia and Alt+Shift+V to place a blind/buried via. Microvias may only be placed such that they connect one of the outer copper layers to an adjacent layer. Blind/buried vias may be placed on any layer.

Vias placed by the router are considered to be part of a routed track. This means that the via net can be updated automatically (just like track nets can), for example when updating the PCB from the schematic changes the net name of the track. In some cases this may not be desired, such as when creating stitching vias. The automatic update of via nets can be disabled for specific vias by turning off the “automatically update via nets” checkbox in the via properties dialog. Vias placed with the Add Free-standing Vias tool are created with this setting disabled.

Routing differential pairs

Differential pairs in KiCad are defined as nets with a common base name and a positive and negative suffix. KiCad supports using + and -, or P and N as the suffix. For example, the nets USB+ and USB- form a differential pair, as do the nets USB_P and USB_N. In the first example, the base name is USB, and USB_ in the second. The suffix styles cannot be mixed: the nets USB+ and USB_N do not form a differential pair. Make sure you name your differential pair nets accordingly in the schematic in order to allow use of the differential pair router in the PCB editor.

To route a differential pair, click the Route Differential Pairs icon (from the drawing toolbar or from the top toolbar under Route) or use the hotkey 6. Click on a pad, via, or the end of an existing differential pair track to start routing. You can start routing from either the positive or negative net of a differential pair.

The differential pair router will attempt to route the pair of tracks with a gap taken from the design rules (differential pair gap can be configured in the Net Classes section of the Board Setup dialog, or by using custom design rules). If the starting or ending location of the route is a different distance apart from the configured gap, the router will create a short “fan out” section to minimize the length of track where the differential pair is not coupled.

When switching layers or using the Place Via (V) action, the differential pair router will create two vias next to each other. These vias will be placed as close as possible to each other while respecting the design rules for copper and hole-to-hole clearance.

Modifying tracks

After tracks have been routed, they can be modified by moving or dragging, or deleted and re-routed. When a single track segment is selected, the hotkey U can be used to expand the selection to all connected track segments. The first press of U will select track segments between the nearest junctions with pads or vias. The second press of U will expand the selection again to include all track segments connected to the selected track on all layers. Selecting tracks with this technique can be used to quickly delete an entire routed net.

There are two different drag commands that can be used to modify a track segment. The Drag (45-degree mode) command, hotkey D, is used to drag tracks using the router. If the router mode is set to Shove, dragging with this command will shove nearby tracks. If the router mode is set to Walk Around, dragging with this command will walk around or stop at obstacles. The Drag Free Angle command, hotkey G, is used to split a track segment into two and drag the new corner to any location. Drag Free Angle behaves like the Highlight Collisions router mode: obstacles will not be avoided or shoved, only highlighted.

The Move command (hotkey M) can also be used on track segments. This command will pick up the selected track segments, ignoring any attached track segments or vias that are not selected. No DRC checking is done when moving tracks using the Move command.

It is possible to re-route tracks attached to footprints while moving the footprints. To do so, use the drag command (D) with a footprint selected. Any tracks that end at one of the footprint’s pads will be dragged along with the footprint. This feature has some limitations: it only operates in Highlight Collisions mode, so the tracks attached to footprints will not walk around obstacles or shove nearby tracks out of the way. Additionally, only tracks that end at the origin of the footprint’s pads will be dragged. Tracks that simply pass through the pad or that end on the pad at a location other than the origin will not be dragged.

It is possible to modify the width of tracks and the size of vias without re-routing them using the Edit Tracks and Vias dialog. See the section below on bulk editing tools for details.

Length tuning

The length tuning tools can be used to add serpentine tuning shapes to tracks after routing. To tune the length of a track, first pick the appropriate length tuning tool. The single track tuning tool (icon or hotkey 7) will add serpentine shapes to bring the length of a single track up to the target value. The differential pair tuning tool (icon or hotkey 8) will do the same for a differential pair. The differential pair skew tuning tool (icon or hotkey 9) will add length to the shorter member of a differential pair in order to eliminate skew (phase difference) between the positive and negative sides of the pair. As with the Routing icons, the Tuning icons are found in both the Route menu dropdown from the top toolbar and the drawing toolbar on the right.

To select the target length for the length tuning tools, open the Length Tuning Settings dialog from the context menu or with the hotkey Ctrl+L after activating the length tuning tool:

This dialog can also be used to configure the size, shape, and spacing of the meander shapes.

After configuring the target length, click a track in the area that you wish to start placing meander shapes. Move the mouse cursor along the track, and meander shapes will be added. A status window will appear next to the cursor showing the current length of the track and the target length. Click again to finish placing the current meander. Multiple meanders can be placed on the same track if desired.

Interactive router settings

The interactive router settings can be accessed through the Route menu, or by right-clicking on the Route Tracks button in the toolbar. These settings control the router behavior when routing tracks as well as when dragging existing tracks.

Forward and back annotation

Geographical re-annotation

Locking

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.

Bulk editing tools

Cleanup tools

Importing graphics

Importing vector drawings from DXF and SVG files

Importing bitmap images