When working with graphic shapes like rectangles or arcs, such as when drawing shapes or when selecting a reference point for a move operation, many additional snapping points are available that let you snap to features of existing graphic shapes.

Available snapping points for graphic shapes include:

When you hover over a snap point with a shape tool active, a graphical icon will be shown that indicates a snapping point is active and explains the type of snapping point. Clicking will use that snapping point. Some shapes display auxiliary snapping lines that appear when you snap to part of that object. For example, line segments display an auxiliary line that continues the segment beyond its endpoint, and arcs display an auxiliary circle that completes the arc’s circumference. Auxiliary shapes can be used for snapping just like the original shape. An auxiliary line and circle are shown as a solid purple line in the screenshot below. The cursor indicates that the active snapping point is the endpoint of a line.

If you move the cursor away from the snapping point, a horizontal or vertical dashed line will appear, depending on the direction of motion. This indicates a horizontal or vertical projection from the snapping point, respectively. Following the line will maintain a position that is horizontally or vertically aligned to the original snap point. This projection is shown as a purple dashed line in the screenshot below.

Interactive editing operations are snapped to the active grid. You can adjust the grid size using the grid dropdown in the top toolbar or by right-clicking and selecting a new grid from the list in the Grid submenu. Pressing the n or N hotkeys will cycle to the next and previous grid in the list, respectively.

You can also select a new grid or edit the available grids in the Grids pane of the preferences dialog. As a shortcut to reach this dialog, right click the button on the left toolbar and select Edit Grids…​.

In this dialog you can select an active grid from the list of grids, reorder the list of grids ( / ), and add (), remove (), or edit () grids. Grids defined in this dialog can have unequal X and Y spacing as well as an optional name. The grid spacing and name are specified when you create or edit a grid.

This dialog also lets you designate two grids from the list as "Fast Grids", which can be quickly selected using Alt+1 and Alt+2.

Finally, you can configure grid overrides for different types of objects. Grid overrides let you set particular grid sizes for different types of objects which will be used instead of the default grid when working with those objects. For example, you can set a 100 mil grid for footprints and pads while using smaller grids to finely position tracks, vias, and text. Grid overrides can be individually enabled and disabled in this dialog, or globally enabled and disabled using the button on the left toolbar (Ctrl+Shift+G).

To change the origin (zero point) of the grid, use Place → Grid Origin and click to place the origin in the canvas. This function is also available with the button in the right toolbar. Alternatively, you can enter explicit coordinates for the grid origin with Edit → Grid Origin…​.

The visual appearance of the grid can also be customized in several ways. You can change the thickness of the grid markings, switch their shape (dots, lines, or crosses), and set the minimum displayed spacing in the Display Options page of the preferences dialog, and you can change the grid color in the Colors page of the preferences dialog.

The grid can be shown or hidden using the button on the left-hand toolbar. By default the grid is still active even if it is hidden, but this is configurable in the Display Options preferences page. There you can set the grid to be disabled when it is hidden or even disable the grid entirely.

Footprints are automatically added to the board when the PCB is updated from the schematic. The footprint associated with each schematic symbol is added to the board if it is not already present, and each footprint pad is associated with the corresponding symbol pin’s net. Symbol pins are matched to footprint pads by pin/pad number.

When footprints are added to the board after an update from the schematic, they are clustered by schematic sheet and by geographical location in the schematic. They are initially attached to the cursor; you can place them by clicking in the desired location.

You can also add footprints to the board manually using the Add Footprint tool (A or the button).

Once footprints have been added to the board, you can reposition them in many ways.

The Move command (M) moves a footprint or a selection of footprints, ignoring any connected track segments that are not selected. No DRC checking is done when moving footprints with the Move command, although any footprint courtyards that collide with the moved footprint’s courtyard will be highlighted.

There is a reference point for the move operation, which is the point in the footprint which attaches to the cursor and therefore the point in the footprint that snaps to the grid and to other objects. The reference point during a move is determined by the location of the cursor when the Move command is initiated. If the cursor is over a pad, the pad’s center will be used as the reference point. If the cursor is not over a pad, the footprint’s anchor (coordinate origin point) will be used. To select an arbitrary snapping point, you can use the Move With Reference command instead of the regular Move command (right click → Positioning Tools → Move with Reference). After initiating the command, click on the desired reference point; KiCad will then begin the move with that point as the reference.

You can also use the Drag command (D) to move the selected footprint using the interactive router, maintaining all track connections to the footprint. Dragging footprints behaves like the Highlight Collisions router mode: obstacles will not be avoided or shoved, only highlighted. Ordinarily the router will prevent you from dragging a footprint into a position that violates DRC: when you click to commit a drag in a position that violates DRC, the footprint will return to its original position. To force a drag to be committed even if it violates DRC, Ctrl-click to commit the drag. Like the Move command, colliding courtyards are highlighted.

You can move a footprint to the opposite side of the board with the Flip command (F). Any parts of the footprint on a front layer will be swapped to the corresponding back layer, and vice versa.

Footprints can be rotated counter-clockwise using the R hotkey, or clockwise using Shift+R. By default, footprints are rotated by 90 degrees every time the rotate command is used, but you can configure the rotation angle step in Preferences → PCB Editor → Editing Options.

You can directly set a footprint’s exact absolute position, rotation angle, and PCB side using either the Footprint Properties dialog or the Properties panel.

To reposition a footprint relative to its current position, use the Move Exactly tool (Shift+M). The dialog lets you specify an X and Y translation, as well as a rotation, that will be applied to the footprint. The rotation can be performed relative to either the footprint’s anchor, the local coordinate origin, or the drill/place origin. You can also use polar coordinates instead of Cartesian coordinates.

To position a footprint relative to another object, you can use the Position Relative tool (Shift+P). With this tool, you select a reference point for the move and specify an offset. The footprint is moved to the specified offset relative to the reference point. The reference point can be one of the following:

To position a footprint such that an arbitrary point in the footprint is positioned a certain distance from another arbitrary reference point, you can use the Position Interactively tool (right click a footprint → Positioning Tools → Position Interactively…​).

This tool lets you interactively select two points that form the start and end of a position vector. The first point is a reference point in the footprint, and will move along with the footprint. The second point is a fixed reference that will remain stationary when the footprint is moved. The vector from the first point to the second point is shown graphically in the editing canvas. You can then give new X and Y (or polar) dimensions for the vector, which will move the footprint reference relative to the fixed reference such that the fixed reference is the specified distance from the footprint reference point. The dialog initially contains the vector dimensions before any move is performed, or in other words the initial distance between the footprint reference point to the fixed reference.

You can swap the position of two selected footprints using the Swap command (Alt+S). The first footprint is assigned the location, rotation, and board side of the second footprint, and vice versa. If there are more than two footprints selected, the locations are cycled: the last footprint gets the position of the first footprint, the first footprint gets the location of the second, and so on.

There are several convenience features that make it easier to find, select, and move specific footprints or footprints related to another footprint.

The Get and Move Footprint command (T) prompts you to choose a footprint from a list or by typing a reference designator. KiCad then attaches the chosen footprint to your cursor for a move operation.

There are two commands to select other footprints that need to be connected to the selected footprint but don’t yet have routed connections. The Select All Unconnected Footprints command (O) selects all footprints that have ratsnest lines to the currently selected footprints. The command can be executed repeatedly to further expand the selection based on the newly selected items. The Grab Nearest Unconnected Footprint command (Shift+O) selects the closest footprint with ratsnest lines to the currently selected footprint, and additionally begins to move it. If there are multiple footprints initially selected, the command will act like the Move Individually command described below, individually moving the closest unconnected footprint for each of the initially selected footprints.

You can select footprints based on their schematic sheet using the right click → Select → Items in Same Hierarchical Sheet command, which selects all other footprints that are in the same schematic sheet as the originally selected footprint.

If you want to move multiple selected footprints in sequence, use the Move Individually command (Ctrl+M). After triggering the command, KiCad will begin moving the first selected footprint. After you click to place the footprint, KiCad will immediately start moving the next footprint, in the same order that you selected the footprints. You can skip moving a footprint by pressing Tab, commit the current move and skip any remaining moves by double-clicking, or cancel all moves (including those already completed) by pressing Esc.

If you want to move a collection of footprints at once into one area, the Pack and Move Footprints command (P) closely packs the selected footprints together and moves them as a block.

Finally, KiCad can automatically place footprints onto the board. The auto-place function attempts to optimally place footprints to simplify ratsnest connections to other footprints. You can auto-place the selected footprints with Place → Auto-Place Footprints → Place Selected Footprints, or auto-place all footprints outside of the board outline with Place → Auto-Place Footprints → Place Off-Board Footprints.

Footprints in the board can be individually edited, both in terms of their properties (fields, attributes, clearance settings, etc.) and in terms of their physical pads and graphics. Editing a footprint in the board only affects that particular instance of the footprint; it does not affect any other copies of that footprint in the board, and it does not affect the library footprint.

To edit the properties of a footprint in the board, open its properties dialog (E)

The majority of the settings in this dialog are the same as in the footprint editor. You can edit the footprint’s fields, attributes, clearance and zone connection settings, 3D models, and embedded files, as in the footprint editor. However, here you can also set the footprint’s position, orientation, and side. You can also update the footprint from the library, exchange it for a different footprint, or edit the footprint itself in the footprint editor.

To edit the footprint’s physical form, i.e. its pads and graphics, you need to use the footprint editor. There are two buttons for opening a footprint in the editor, depending on whether you want to edit a single copy of a footprint in the board or a footprint’s source copy in the library.

The Update Footprint from Library…​ button is used to update the board’s copy of the footprint to match the copy in the library. The Change Footprint…​ button is used to swap the current footprint to a different footprint in the library. These functions are described later.

An individual symbol text field can be edited directly with the E hotkey (with a field selected instead of a footprint) or by double-clicking on the field.

The options in this dialog are the same as those in the full Footprint Properties dialog, but are specific to a single field.

Only footprint fields can be edited this way in the board editor. Unlike fields, Footprint text is a graphic object that can only be edited or moved in the footprint editor.

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

To update footprints in the board to match the corresponding library footprint, use Tools → Update Footprints from Library…​, or right click a footprint and select Update Footprint…​. You can also access the tool from the footprint properties dialog.

The top of the dialog has options to choose which footprints will be updated. You can update all footprints on the board, update only the selected footprints, or update only the footprints 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 footprint will be updated. You can select specific fields to update or not update, which properties of the fields to update (text content, visibility, size and style, and position), and how to handle fields that are missing or empty in the library footprint. You can also choose whether to update footprint attributes, such as footprint type, not in schematic, exclude from position files / bill of materials, exempt from courtyard requirement, and do not populate.

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

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

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

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

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

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

By default, the comparison displays both versions of the footprint 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 footprint in the superimposed view (making the board version of the footprint more transparent) or drag it to the left to emphasize the board version (making the library version more transparent). At the far right and left ends of the slider, the board and library versions of the footprint, respectively, are fully hidden. It may be helpful to drag the slider back and forth to see the changes more clearly.

You can press the A/B button, or use the / hotkey, to quickly toggle back and forth between the board and library versions.

The screenshot above shows a visual comparison with the board version of the footprint deemphasized. Looking at pad 1 on the left, you can see a large, partially transparent pad (from the board footprint) surrounding a fully opaque, smaller pad (from the library footprint). This indicates that the pad was enlarged in the board version of the footprint, or shrunk in the library version of the footprint.

Instead of editing a single zone with the Zone Properties dialog, you can use the Zone Manager tool to you view, edit, and prioritize all zones in the board at once. To run the Zone Manager, click Tools → Zone Manager.

The top left of the dialog shows a list of all zones in the board, displaying the name (if any), net, and layers for each zone. The order of the zones in the list reflects the priority of each zone: higher priority zones are higher in the list. To change the priority of a zone, use the and buttons to move it up or down in the list. You can filter the list of zones by typing into the filter box. The filter matches against the zones' name and/or net, depending on which filter options are enabled.

Selecting a zone in the list shows a preview of that zone in the top right. If the selected zone spans multiple layers, each layer is shown individually. You can preview each layer by clicking the appropriate layer tab above the preview.

The bottom part of the dialog shows the settings for the selected zone, which are explained above. You can preview the new settings by clicking the Update Displayed Zones button, which updates the zone preview without affecting the board. Changing the properties of a zone in the Zone Manager will not update the board until you press OK. If the Refill zones option is enabled, all zones will be refilled when you accept the dialog. If Refill zones is not enabled, zones will not be refilled until you manually refill them.

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

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 set 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.

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 tracks on either side of the corner to be filleted. If a contiguous track selection contains multiple corners, they will all be filleted.

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.

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:

After using any of the above methods to add a via and change layer, but before clicking to fix the via and commit the current track segment, you can cancel placing the via by pressing V. The via will be removed and routing will continue on the original layer.

You can place a via and end the current track, without changing layers, by pressing V and then double-clicking to place the via.

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).

You can also place microvias and blind/buried vias while routing. Use the hotkey Ctrl+V to place a microvia and Alt+Shift+V to place a blind/buried via. While regular vias always go through every board layer, microvias and blind/buried vias can start and end on any layer, not just the outer layers.

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.

The active layer is swapped with the other one in the current layer pair using the Place Via hotkey (V).

You can define the active pair along with a list of "preset" layer pairs in the Set Layer Pair dialog, accessed from the two-color swatch on the toolbar. These pairs are stored in the project file.

Each can be enabled or disabled, and given an optional user-friendly name.

The enabled presets can be cycled using the Cycle Layer Pair Presets hotkey (Shift+V). If the last-used or current layer pair is not a preset, it is included in the list with the name "Manual".

In addition to placing vias while routing, you can also place standalone vias. These vias connect to items that they touch when they are placed. Free vias may be useful for via stitching, via shielding, thermal design, or other reasons.

To place a free via, click the button or press Ctrl+Shift+X, then click in the desired location in the editing canvas. If you place a via directly over a track, it will connect to that track as if it was placed while routing: it will take the track’s net, it will create a joint in the track, and dragging the via will also drag the attached tracks.

The net assigned to a free via depends on where the via was placed. If the via was placed over a track or pad, it will have the same net as the track, and its Automatically update via nets setting will be enabled so that its net changes with the track’s net. Otherwise, the via will take the net of any zone under the via, if one exists, and its net will not update automatically. If there are multiple zones under the via, you will be prompted to choose which net to use. If there is no zone, the via will not have a net assigned.

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 reposition 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. Multiple tracks can be dragged at once using this command. 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 also possible to move a footprint while keeping tracks attached to the footprint as it moves. To do so, use the drag command (D) with one or more footprints selected. Any tracks that end at one of the footprint’s pads will be dragged along with the footprints. 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. Any DRC violations caused by the drag operation will be highlighted and will be prevent the footprint drag from being committed when you click. To ignore the violations and commit the drag anyway, use Ctrl+click. 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.

To break a single track segment into two, use the Break tool (right click a track → Break Track). The track will be broken into two connected track segments at the cursor location. Each track segment can then be selected, moved, and edited individually. To recombine the segments into a single segment, drag the drack, or use the merge co-linear tracks option in the Cleanup Tracks and Vias dialog.

You can modify the width of tracks and the size of vias, without re-routing them, in the properties dialog for the track or via. This modifies all selected tracks and vias. The properties dialog shows the relevant properties for the items in the selection: if both tracks and vias are selected, then properties for both types of objects will be displayed, but if only one type of object is selected then properties for the other type of object will not be shown.

In the Common section, you can change the assigned net of the selected objects using the Net dropdown. If the Automatically update via nets option is checked, the selected vias cannot have their assigned net manually changed, but instead will be assigned the net of any zone or pad that they touch. You can also lock the selected objects.

In the Tracks section, you can set the start and end position of the tracks and the layer they are on. You can also change the track width, either from a list of pre-defined sizes or to an arbitrary value.

You can remove the solder mask from on top of tracks on outer layers by enabling the Solder mask checkbox. When enabled, solder mask openings will be drawn for each of the selected tracks with the same shape as the source track. The Expansion textbox controls the size of the mask opening relative to the original track: the expansion value will be added to each side of the original track to form the mask shape. For example, a 1mm wide track with a 1mm expansion would result in a 3mm wide mask cutout, because the 1mm expansion is added to both sides of the track.

In the Vias section you can change the properties of selected vias. You can change the position of a via, the via’s type (through, micro, or blind/buried), and which layers it spans. Through vias always start and end on the front and back copper layers, but micro vias and blind/buried vias can start and end ony any layers.

You can modify the via annulus and hole diameters, either from a list of pre-defined sizes or to arbitrary values. A via’s diameter and hole size can be defined on a per-layer basis. This is also known as defining the via’s padstack. The Padstack mode controls whether the via shape is the same on all layers or whether individual layers are individually controlled.

The Annular rings setting controls which layers will have annular rings for the via.

Annular rings can be removed or added in bulk using the Edit Track and Via Properties dialog or by running the Unused Pads tool.

The Front tenting and Back Tenting options control whether the via has front and back solder mask covering it.

If the button is pressed, the front and rear tenting settings will be linked. If it is unpressed, they can be modified independently.

You can also change the teardrop properties for vias in this dialog.

To modify tracks and vias in bulk you can use the Edit Track and Via Properties dialog (Edit → Edit Track & Via Properties…​)..

Scope settings restrict the tool to editing only tracks, vias, or both. If no scopes are selected, nothing will be edited.

Filter Items restricts the tool to editing particular objects in the selected scope. Objects will only be modified if they match all enabled and relevant filters (some filters do not apply to certain types of objects. For example, via size filters do not apply to tracks). If no filters are enabled, all objects in the selected scope will be modified. For filters with a text box, wildcards are supported: * matches any characters, and ? matches any single character.

Properties for filtered objects can be set to new values in the bottom part of the dialog. Properties can be set to arbitrary values by selecting set to specified values or set to the default value from the net class (or custom rule) by selecting set to net class / custom rule values.

When setting to specified values, you can choose -- leave unchanged -- to preserve objects' existing values, or select a new value from the dropdown menu. For Track width and Via size, the options are the pre-defined track or via sizes from Board Setup.

You can quickly remove unused annular rings from pads and vias using the Unused Pads tool (Tools → Remove Unused Pads…​). This will leave annular rings in place on layers where they are used and remove them on layers where they are not used. An annular ring is considered unused if there are no track or zone connections to the pad/via on that layer.

The Remove Unused Layers button removes all unused annular rings from pads and vias that meet the selected filter settings. The Restore All Layers button restores all annular rings to the pads and vias that meet the selected filter settings.

The checkboxes filter which objects will be modified (annular rings removed or restored) and which layers will be removed for those objects.

There is a dedicated tool for performing common cleanup operations on tracks and vias, which is run via Tools → Cleanup Tracks & Vias…​.

The following cleanup actions are available and will be performed when selected:

You can also filter the objects that will be cleaned up by net, netclass, layer, or selection.

Any changes that will be applied to the board are displayed at the bottom of the dialog after clicking the Build Changes button. After building the changes, the button changes to say Update PCB. The changes are not applied until you press the Update PCB button.

KiCad offers several functions to make certain routing operations more convenient.

If you need to route a number of tracks from a set of pads, you can use the Route Selected tool to quickly route from each pad in sequence. Select the pads you want to use as starting points, then right click and choose Route Selected (Shift+X) to route from each pad in sequence. The router will begin a track from the first selected pad, which you can route as you would any other track. When you complete the track, the router will automatically begin a new track from the next pad in the selection, in the same order that you selected the pads. Pads that already have tracks attached are skipped. You can also skip routing the current track and move on to the next pad by pressing Esc. You can also select footprints instead of pads; all unrouted pads in the selected footprints will be used as starting points.

If you want to route a number of tracks to a set of pads, instead of from the pads, you can use the Route Selected From Other End tool. Select the pads you want to use as ending points, then right click and choose Route Selected From Other End (Shift+E). This tool works the same way as the Route Selected tool, except it uses each selected pad as an end point rather than a starting point. The starting point for each track is the other end of the ratsnest line for each selected pad.

Routing from the other end is also possible while routing individual tracks: press Ctrl+E while routing a track to commit the current segment and begin routing from the other end of the in-progress track’s ratsnest line.

Finally, you can quickly unroute tracks connected to an object (footprint, pad, or track) by selecting the object, right-clicking, and choosing Unroute Selected. Any tracks connected to the selected object will be removed, starting at the selected object and continuing until another pad is encountered.

KiCad’s router can automatically route individual tracks, based on the connections defined in the schematic. This can be thought of as a limited form of auto-routing that considers a single track at a time. The router will only use the current layer; it will not use vias or change layers.

While routing, press the F key to have the router attempt to automatically finish the current track. The track will be automatically routed from the end of the last fixed track segment to the closest ratsnest anchor. If the router can’t automatically finish the track, it will allow you to complete the track manually. This action can also be performed by clicking Attempt Finish in the context menu while routing.

When the router is not the active tool, you can automatically route multiple tracks by selecting footprints, pads, and tracks to route from, right clicking, and choosing Attempt Finish Selected (Autoroute) (Shift+F). You do not need to select both ends of a desired connection; the router will route from the selected item to its nearest ratsnest anchor. If multiple items were selected, each item will be routed in sequence, in the order that they were selected. If a connection cannot be automatically completed, the tool will pause with the router active so that you can complete the track manually. With the automatic completion paused for a manual connection, you can press Esc to skip routing the current track. After manually completing the track or skipping the connection, the tool will continue attempting to route the remaining connections.

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.

The length tuning tools can be used to add serpentine tuning shapes to tracks after routing. Length tuning shapes are persistent objects that can be modified after they are created. To tune the length of a track, first pick the appropriate tool.

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.

When a tuning tool is active, you can hover over tracks in the board to show a status window that displays their current length or skew as well as the target values. Click on the desired track to start tuning it. As you move the mouse cursor along the track, meander shapes will be added interactively. If a target length has been set, meanders will stop being added when the target length is reached. You can set a target length with custom DRC rules or in the tuning shape properties; both methods are explained below. The popup window next to the cursor shows a live measure of the length or skew compared to the design targets. You can adjust the spacing (1 to increase and 2 to decrease) and amplitude (3 to increase and 4 to decrease) while you tune. When you are done, click again to commit the tuned shape. The tuned track doesn’t need to be perfect because you can adjust the shape after committing it. You can also place multiple tuning shapes on the same track.

Teardrops are areas of extra copper that smooth the transition between tracks and pads, vias, or other tracks with different width. Teardrops are added to increase the mechanical robustness of a track connection. They also reduce the risk of a misaligned drill hole disconnecting a track from a drilled pad or via.

There are two ways to add teardrops to your design. You can add them in bulk using the Edit Teardrops dialog, or you can add them to individual pads and vias in the respective properties of the pad or via.

Graphical shapes are geometric objects that can be drawn on any board layer.

When they are drawn on copper layers, graphical objects can be assigned nets and make connections to other copper objects, much like tracks and zones. There are differences between copper shapes and tracks or zones, however:

The buttons on the right toolbar can be used to create:

To place a shape, select the tool, then click in the canvas to place the shape’s first point. Click again to place the shape’s second point. For rectangles and circles, placing the second point will fully define the shape and finish drawing it. Some shapes require three or more points to be placed, however. Arcs require three points, while lines, polygons and bezier curves can accept an arbitrary number of points, and require a double click to complete.

To modify an existing graphical object, select it, then drag its editing handles to change the shape. Moving a handle at the vertex of a shape will move that vertex. Moving a handle on the edge of a shape will move that edge while maintaining the edge’s angle.

Arcs have two vertex editing modes, which are selectable in Preferences → PCB Editor → Editing Options or by right clicking the button on the right toolbar.

Just like with tracks, you can expand a selection from one graphic line to include all other contiguous graphic lines by pressing U.

The properties of a graphic shape can be adjusted in the shape’s properties dialog or with the Properties Manager.

Graphical text may be placed by using the button in the right toolbar or by keyboard shortcut Ctrl+Shift+T. Activating the tool brings up a text properties dialog. After configuring the text and its properties and accepting the dialog, you can click in the canvas to place the text.

You can also add text boxes, which are similar to regular text except that they have an optional border and they automatically reflow text within that border. Text boxes are placed with the button, and require clicking twice to specify the top left and bottom right corners of the box.

Text boxes additionally have options controlling their border.

Finally, text supports markup for superscripts, subscripts, overbars, evaluating project variables, and accessing symbol field values.

You can use a table to organize text in a tabular format. Tables have customizable borders, cell sizes, and headers, and can be placed on any layer.

To place a table, use the button in the right toolbar. Click in the canvas to place the top left corner of the table, then click again to place the bottom right corner of the table and finish drawing the table. The bigger you draw the table, the more rows and columns will be added by default, but rows and columns can be added or deleted after the table is created.

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 five different types of dimension: aligned, orthogonal, center, radial, and leader.

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.

Properties of text and graphics, including footprint fields and dimensions, can be edited in bulk using the Edit Text and Graphics Properties dialog (Edit → Edit Text & Graphic Properties…​).

There is a dedicated tool for performing common cleanup operations on graphics, which is run via Tools → Cleanup Graphics…​.

The following cleanup actions are available and will be performed when selected:

Any changes that will be applied to the board are displayed at the bottom of the dialog. They are not applied until you press the Update PCB button.

The drawing sheet’s title block is edited with the Page Settings tool (). You can also open this tool by double clicking on any part of the drawing sheet.

Each field in the title block can be edited, as well as the paper size and orientation.

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 listed in the board title block is not automatically updated. It is only updated when changed in this dialog.

A drawing sheet file can also be selected to replace the default drawing sheet. When choosing a drawing sheet, you can enable the Embed File checkbox in the file browser to embed the drawing sheet in the board instead of referencing an external file. This means the board will appear the same when it is opened on another computer that does not have the drawing sheet file available at the same external file path. For more information, see the embedded files documentation.

Designing a multichannel layout begins in the schematic. You need to specify which components (symbols) belong to each channel. Each channel in the schematic must be equivalent to the other channels. This means channels must match each other in the following ways:

In the example schematic below, Channels 1, 2, 3, and 4 are equivalent and therefore can be used to share routing in a multichannel design. Even though the net connections are drawn differently in some channels, the underlying net connections are the same. The different symbols in Channel 2 and the different values in Channel 3 also do not break the equivalency. Footprint assignments are not shown in the image, but the symbols that correspond between channels must use the same footprints. In this example, this means that R1, R3, R5, and R7 each must use the same footprint, as must R2, R4, R6, and R8.

In contrast, Channels A and B are not equivalent to Channels 1-4, nor to each other. Channel A contains an extra parallel resistor not present in the other channels, and Channel B is missing a connection between the two resistors.

You can assign symbols to channels in two ways, either using hierarchical sheets or using component classes.

In the board, each channel is represented with a rule area with its rules configured for placement. You need to add a rule area for each channel. One rule area is the reference, containing manually placed and routed footprints. The other rule areas are targets and have the reference placement and routing copied to them. Placement rule areas, whether for reference or target channels, need the following settings configured in their properties:

Placement rule areas can be manually created like any rule area, or they can be automatically generated by selecting Tools → Multi-Channel → Generate Placement Rule Areas…​. This tool can draw basic placement rule areas for any of the hierarchical sheets or component classes in the design, depending on which you select.

The tool has several options:

Automatically generated rule areas are preconfigured as placement rule areas with the appropriate source hierarchical sheet or component class selected. Their layers are set to just the front and back copper layers. They are drawn as the minimum size rectangle that encloses their constituent footprints, without extra space for routing or other items. After generating a rule area, you may want to change the configured layers to ensure all desired items in the reference channel get copied to the target channels. You also may want to edit the shape of the rule area, although rule areas for target channels will have their shapes automatically adjusted to match the reference rule area.

Once you have created rule areas for each channel and completed placing footprints and routing for the reference channel, you can use the Repeat Layout tool to copy the reference channel’s layout to the other channels. Run this tool using Tools → Multi-Channel → Repeat Layout…​.

If a rule area is selected when the tool is run, that rule area will be used as the reference rule area. If no rule area is selected, you will be prompted to select a rule area. When the reference rule area is determined, a dialog will appear.

The table at the top of the dialog controls which target rule areas will receive the layout from the reference channel. Any target rule areas that are not selected will not be updated. The tool will only copy items to a target rule area if the target’s status is listed as "OK". If the status is not "OK", the target channel’s circuit topology cannot be matched to the reference channel; see the requirements for how channels need to match in the schematic for more information.

There are several options to control which items from the reference channel are copied to the selected target areas, and how those copied items are handled:

After clicking OK, the layout from the reference channel will be applied to the target channels. When the repeat layout is completed, each channel can be individually edited like any other part of the board design.