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:

You can swap the position of two selected footprints using the Swap command (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, and 3D models, 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.

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, 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.

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.

在水平(H) / 垂直 (V) / 45 度模式下布线时，形态 是指一组两个线段如何连接单个 H/V/45 度线段无法到达的两个点。 在这种情况下，这些点将由一条水平或垂直线段和一条斜线段 (45度) 连接。形态指的是这些线段的顺序：是水平/垂直线段在前还是斜线段在前。

KiCad 的布线器会尝试根据一系列因素自动选择最佳形态。一般说来，布线器会尝试最大限度地减少路线中的拐角数量，并尽可能避免 "槽糕" 的拐角 (如锐角)。当从焊盘布线或布线到焊盘时，KiCad 将选择使路线与焊盘最长边缘对齐的形态。

在某些情况下，KiCad 无法正确猜测您想要的形态。要在布线时切换布线的形态，请使用切换布线形态命令 (快捷键 /)。

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.

当以 H/V/45 模式布线时，KiCad 的布线器可以放置尖角或圆角 (弧形) 的布线。要在尖角和圆角之间切换，请使用布线拐角模式命令 (快捷键 Ctrl+/)。使用圆角布线时，每个布线步骤将放置直线段、单个圆弧或同时放置直线段和圆弧。布线形态决定首先放置圆弧还是直线段。

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 的布线器支持活动布线过程中的布线宽度调整。 换句话说，要改变导线中间的宽度，必须结束布线，然后从上一个布线的末端重新开始一条新的布线。 要改变活动布线的宽度，可使用快捷键 W 和 Shift+W，切换在电路板设置对话框中配置的布线宽度。

在进行布线时，切换层会在当前（未固定）导线的末端插入一个过孔。 一旦你放置了过孔，布线将继续在新层上进行。 有几种方法可以选择一个新层并插入过孔：

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 trace 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 trace, without changing layers, by pressing V and then double-clicking to place the via.

过孔的尺寸将取自当前的 “过孔尺寸” 设置中，可通过顶部工具栏的下拉列表或使用快捷键 (') “增加过孔尺寸” 及快捷键 (\) “减小过孔尺寸” 。与布线宽度类似，当过孔大小设置为"使用网络类尺寸" 时，将使用 "电路板设置" 的 "网络类" 部分中配置的过孔大小 (除非被自定义设计规则覆盖)。

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. 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.

布线器放置的过孔被认为是已布线导线的一部分。 这意味着过孔网络可以自动更新（就像导线网络一样），例如，当从原理图中更新 PCB 时改变了导线的网络名。 在某些情况下，这可能是不需要的，例如在创建缝合孔时。 对于特定的过孔，可以通过关闭过孔属性对话框中的 "自动更新过孔网络" 复选框来禁用过孔网络的自动更新。 使用 "添加独立过孔" 工具放置的过孔在创建时禁用这一设置。

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".

布线完成后，可以通过移动或拖动来修改它们，或者删除并重新布线。 当选择一个导线时，快捷键 U 可以用来将选择范围扩大到所有连接的导线。 第一次按下 U 将选择与焊盘或过孔最近的连接点之间的导线。 第二次按 U 将再次扩大选择范围，包括所有层上与所选导线相连的所有导线。 用这种技术选择导线可以用来快速删除整个布线网络。

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. 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.

移动命令（快捷键 M）也可以在导线上使用。 该命令将拾取选定的导线，而忽略任何未被选中的附加导线或过孔。 使用移动命令移动导线时，不会进行 DRC 检查。

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 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.

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:

Delete tracks connecting different nets: removes any track segments that short multiple nets.

Delete redundant vias: remove vias that are redundant because they are located on top of another via or on top of a through hole pad.

Delete vias connected on only one layer: removes vias that are only connected to copper on a single layer and are therefore unnecessary.

Merge co-linear tracks: merges any track segments that are connected and co-linear into a single equivalent track segment.

Delete tracks unconnected at one end: removes track segments that have at least one dangling end.

Delete tracks fully inside pads: removes tracks that have both start and end points within a pad and are therefore unnecessary.

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

Filter items by net: limits the cleanup to tracks and vias assigned to the specified net.

Filter items by netclass: limits the cleanup to tracks and vias in the specified netclass.

Filter items by layer: limits the cleanup to tracks and vias on the specified layer.

Selected items only: limits the cleanup to just the selected tracks and vias.

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 traces 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 press Shift+X to route from each pad in sequence. The router will begin a trace from the first selected pad, which you can route as you would any other trace. When you complete the trace, the router will automatically begin a new trace from the next pad in the selection, in the same order that you selected the pads. Pads that already have traces attached are skipped. You can also skip routing the current trace 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 traces to a set of pads, instead of from the pads, you can use the Route Selected From Other End tool (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 trace is the other end of the ratsnest line for each selected pad.

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

Finally, you can quickly unroute traces connected to an object (footprint, pad, or trace) by selecting the object, right-clicking, and selecting Unroute Selected. Any traces 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 traces, based on the connections defined in the schematic. This can be thought of as a limited form of auto-routing that considers a single trace 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 trace. The trace will be automatically routed from the end of the last fixed trace segment to the closest ratsnest anchor. If the router can’t automatically finish the trace, it will allow you to complete the trace 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 traces by selecting footprints, pads, and traces to route from and pressing 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 trace manually. With the automatic completion paused for a manual connection, you can press Esc to skip routing the current trace. After manually completing the trace 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.

要对差分对进行布线，请点击差分对布线 图标（从绘图工具栏或从顶部工具栏 布线 下）或使用快捷键 6。 点击一个焊盘、过孔或现有差分对线段的末端，开始布线。 你可以从差分对的正网络或负网络开始布线。

差分对布线器将尝试用设计规则中的间隙规则进行布线(差分对间隙可以在电路板设置对话框的 “网络类” 部分中配置，也可以通过使用自定义设计规则来配置)。如果布线的起始或结束位置与配置的间隙不同，布线器将创建一个较短的 "扇出" 部分，以最大限度地缩短差分对未耦合的布线长度。

当切换层或使用 放置过孔 (V) 操作时，差分对布线器将创建两个相邻的过孔。这些过孔将被放置在尽可能靠近彼此的位置，同时遵守铜的间隙规则以及孔到孔的间隙规则。

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 traces 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 trace 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 trace 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.

You can add teardrops to your design in bulk using the Edit → Edit Teardrops…​ dialog. This dialog has controls for filtering which objects are affected and settings for configuring the shape of the new teardrops. It also lets you edit or remove existing teardrops.

The Scope section controls which types of objects will be affected: PTH pads, SMD pads, vias, and/or track-to-track connections. The Filter Items section lets you filter objects by other criteria; you can filter items by net, net class, and layer, or choose to act only on round pads, pre-existing teardrops, or the objects in your selection.

The Action section controls whether to add or remove teardrops, as well as the size and shape of the new teardrops.

Remove Teardrops will remove teardrops that match the scope and filtering options at the top of the dialog. Remove All Teardrops will remove all teardrops on the board, even if they do not match the scope and filters.

Add teardrops with default values for shape will add teardrops with the configured default teardrop settings to every board object that matches the scope and filters. To configure the default teardrop settings, click the Edit default values in Board Setup link or manually open the Teardrops panel in Board Setup. The defaults are configured separately for teardrops connecting to round shapes, rectangular shapes, or between tracks. Instead of using the default values, you can provide custom teardrop settings by selecting Add teardrops with specified values.

The available teardrop settings are:

Adding a teardrop to an object that already has a teardrop will update the existing teardrop with the new settings. However, you can leave any existing teardrop setting in an object unchanged by setting the value to -- leave unchanged -- in a textbox, or by selecting the third, indeterminate state for a checkbox. Any value set this way will not be updated in the targeted objects' teardrop settings.

Rather than in bulk, you can add or edit teardrops for individual vias in the properties dialog for that via, or for individual pads in the Connections tab of the pad’s properties dialog. The settings in the properties dialogs are the same as in the Edit Teardrops dialog. You can also edit teardrops for individual pads and vias with the Properties Manager.

Teardrops in KiCad are small zones, meaning that when they refill they avoid shorting to copper objects on other nets. They are initally filled when they are added, but they are unfilled and refilled with other zones on the board: when using the Unfill All Zones and Refill All Zones commands, running DRC, generating fabrication outputs, etc. Teardrops can be shown in filled or outline mode using the zone display controls in the left toolbar.

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.

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.

尺寸标注是用于显示测量值或电路板设计上的其他标记的图形对象。 它们可以被添加到任何绘图层中，但通常被添加到某个用户层。 KiCad 目前支持五种不同类型的标注：对齐、正交、中心、径向和引线。

创建一个尺寸标注后，可以编辑其属性（快捷键 E）以改变显示数字的格式以及文本和图形线的风格。

Properties of text and graphics, including 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.

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 will be the reference, containing manually placed and routed footprints. The other rule areas will have the reference placement and routing copied to them. Placement rule areas 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.

使用 "从原理图更新 PCB" 工具将设计信息从原理图编辑器同步到电路板编辑器。在原理图编辑器和电路板编辑器中都可以用 工具 → 从原理图更新 PCB（F8）来访问该工具。你也可以使用电路板编辑器顶部工具栏上的 图标。这个过程通常被称为正向批注。

该工具将每个符号的封装添加到电路板上，并将更新的原理图信息传输到电路板上。尤其重要的是，电路板的网络连接也将更新以匹配原理图。

将对 PCB 进行的变更列在 待应用的变更 窗格中。在你点击 更新 PCB 按钮之前，PCB 不会被修改。

你可以使用窗口底部的复选框来显示或隐藏不同类型的信息。可以使用 保存…​ 按钮将变更的报告保存到文件中。

KiCad 的典型工作流程是在原理图中进行修改，然后使用 "从原理图更新 PCB" 工具将修改内容同步到电路板上。然而，相反的过程也是可行的：可以在电路板上进行设计修改，然后在原理图或电路板编辑器中使用 工具 → 从 PCB 更新原理图 同步到原理图上。这个过程通常被称为反向批注。

该工具将位号、值、封装分配和网络名称的变化从电路板同步到原理图。每种类型的变更都可以单独启用或禁用。

将对原理图进行的变更列在 待应用的变更 窗格中。在您点击 更新原理图 按钮之前，原理图不会被修改。

你可以使用窗口底部的复选框来显示或隐藏不同类型的信息。可以使用 保存…​ 按钮将变更的报告保存到文件中。

The Geographical Reannotation tool lets you automatically set the reference designators of footprints based on their physical location on the board.

To run the Geographical Reannotation tool, use Tools → Geographical Reannotate…​. This opens the geographical reannotation dialog with options for how to perform the reannotation.

The Options tab contains settings for how footprint locations affect reannotation. The arrow diagrams indicate which geographical ordering to use when reannotating. You can reannotate from left-to-right, right-to-left, top-to-bottom, or bottom-to-top, and you can select whether to use a column-major order (go through all footprints in the same column before moving to the next column) or row-major order (go through all footprints in the same row before moving to the next row).

Geographical reannotation can either use the location of the footprint itself or the location of the footprint’s reference designator. You can also select how much to round footprint locations before determining which footprints are at the same X or Y position. Rounding to a finer coordinate resolution will result in fewer footprints considered to be in the same row or column.

Finally, you can select which footprints to reannotate. You can reannotate all footprints on the board, all footprints on the front or back of the board, or all footprints in your selection.

The Reference Designators tab contains options for how to allocate new reference designators. There are separate settings for footprints on the front and back of the board.

Reference start controls the number for the first new reference designator on each side of the board. If no start value is given for the back of the board, back side footprints will be annotated starting at one higher than the last front side reference designator.

Prefix specifies a prefix string to insert at the beginning of each newly assigned reference designator. This prefix will be inserted before any prefix that is already present. If the remove prefix option is selected, footprints with the specified prefix will instead have that prefix removed instead of added. Footprints without that prefix will not have not have any prefix added or removed.

If exclude locked footprints is checked, locked footprints will not be reannotated. You can also avoid reannotating specific footprints by entering their reference designators as a comma-separated list in the exclude references box.

When you click the Reannotate PCB button, footprints will be reannotated according to the selected settings.