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 grouped 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, which can be the local origin, the grid origin, or another arbitrary point, such as a pad in another footprint. The selected footprint is moved to the specified offset from the reference point.

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. 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 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.

There are two options for editing the footprint 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.

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.

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 /)。

在没有明显的 “最佳” 形态的情况下(例如，从过孔开始布线时)，KiCad 将使用鼠标光标的移动来选择形态。如果希望布线从直线 (水平或垂直) 线段开始，请在水平或垂直方向上将鼠标从起始位置移开。如果您希望布线以斜线开始，请沿斜线方向移动。一旦光标与布线起始位置相距足够远，形态就会被锁定，并且除非光标回到起始位置，否则不会再更改。可以在交互式布线器设置对话框中禁用从鼠标光标移动检测形态，如下所述。

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.

布线的线段的宽度是通过以下三种方式之一来确定的：如果布线的起点是现有线段的终点，并且顶部工具栏上的 按钮被启用，宽度将被设置为现有布线的宽度。 否则，如果顶部工具栏中的布线宽度下拉菜单被设置为 "使用网络类宽度"，则宽度将取自布线的网络类（或任何为网络类指定不同宽度的自定义设计规则，例如在颈缩区域内）。 最后，如果布线宽度下拉菜单被设置为电路板设置对话框中配置的预定义布线尺寸之一，则将使用该宽度。

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 or Shift-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。

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。

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。

有两种不同的拖动命令可用于修改导线。拖动 (45 度模式) 命令，快捷键 D ，用于通过布线器拖动导线。如果布线器模式设置为推挤，则使用此命令拖动将推挤附近的布线。如果布线器模式设置为绕走，则使用此命令拖动将绕过障碍物或停在障碍物处。以自由角度拖动命令，快捷键 G，用于将导线一分为二，并将新的角拖动到任何位置。以自由角度拖动的行为类似于高亮碰撞布线器模式：不会避开或推挤障碍物，只会高亮。

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。

在移动封装的同时，可以对连接在封装上的导线进行重新布线。 要做到这一点，在选择了一个封装的情况下使用拖动命令（D）。 任何以封装的某个焊盘为终点的导线都将与封装一起被拖动。 这个功能有一些限制：它只在高亮冲突模式下运行，所以连接在封装上的导线不会绕过障碍物或将附近的导线推开。 此外，只有以封装的焊盘为终点的导线才会被拖动。 仅仅经过焊盘或在焊盘原点以外的焊盘上结束的导线将不会被拖动。

You can modify the width of tracks and the size of vias, without re-routing them, in the properties of the track or via. You can choose a predefined size or set the size to an arbitrary value. You can also change the position of tracks and vias or change a via’s start and end layers.

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.

Filter items by net filters to items assigned the specified net. Filter items by netclass filters to items assigned to the specified netclass.

按层筛选对象 筛选到指定板层上的对象。

Filter tracks by width filters to tracks with the specified track width. Filter vias by size filters to vias with the specified track width.

Selected items only filters to the current selection.

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.

Drop-down lists can be set to -- leave unchanged -- to preserve existing values, or set to a pre-defined track or via size to change the filtered objects' size. You can also change the filtered objects' layer.

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 track and pads, vias, or other tracks. Teardrops are added to increase the mechanical robustness of a trace connection. They also reduce the risk of a misaligned drill hole disconnecting a trace 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. Adding a teardrop to an object that already has a teardrop will update the existing teardrop with the new settings. When adding teardrops, you can choose to use the default teardrop settings from the Board Setup dialog, or choose specific values for the new teardrops.

Prefer zone connection: if selected, a teardrop will not be created if the object is also connected to a zone. Allow teardrops to span 2 track segments: if selected, the teardrop will be able to spread over a second track segment if the first segment is too short to support a full teardrop. Maximum track width: a teardrop will not be created for a track connection that is wider than this percentage of the pad width (minimum pad dimension). Best length: the ideal length of the teardrop, as a percentage of the width (smallest dimension) of the attached object. Maximum length: the maximum length of the teardrop, as an absolute length. Best width: the ideal width of the teardrop, as a percentage of the width (smallest dimension) of the attached object. Maximum width: the maximum width of the teardrop, as an absolute width. Curved edges: if selected, the teardrop edges will be curved instead of a straight line. If curved, points controls the number of points in the curve; more points will result in a smoother curve.

Default properties for teardrops can be configured in the Board Setup dialog. These defaults will be used in the Edit Teardrops dialog when add teardrops with default values for shape is selected in that dialog. The defaults are configured separately for teardrops connecting to round shapes, rectangular shapes, or between tracks. The available options for each type of teardrop are the same as in the Edit Teardrops dialog.

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.

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.

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

弧线有两种编辑模式，可在 偏好设置 → PCB编辑器 → 编辑选项 中选择，或通过右键单击右侧工具栏上的 按钮。第一种模式（保持弧中心，调整半径）在拖动弧端点或中点时保持弧中心的位置，必要时改变半径。 第二种模式（保持圆弧端点或起点方向）随着中点或中心的拖动，保持圆弧端点的位置和圆弧的曲率方向。

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. Rectangles, circles, and polygons can be filled shapes or outlines. The line width option controls the width of the outline, even for filled objects. The outline width extends on both sides of the "ideal" shape of the graphic object. For example, a graphic circle that is defined to have 2mm radius and 0.2mm line width will consist of a torus with an outer radius of 2.2mm and inner radius of 1.8mm. If the filled shape option is enabled and the line width is set to 0, the shape will be a filled circle with 2mm radius. Several line styles are available: solid, dashed, dotted, dash-dot, and dash-dot-dot.

Graphical shapes on copper layers can have a net assigned in their properties dialog. Copper shapes with a net make connections like tracks or zones. Unlike zones, copper graphical objects always maintain their shape and do not keep clearance to other copper objects.

KiCad has several tools for modifying combinations of graphic shapes in useful ways, such as chamfering two lines or combining two polygons. These tools are used by selecting the shapes you want to modify, right clicking, and then choosing the relevant tool in the Shape Modification submenu. Different tools are available for different combinations of selected shapes.

Heal shapes fixes a discontinuity between two lines or arcs. A new line segment is added to connect the ends of each shape together, up to a specified tolerance.

Fillet lines adds an arc to round the corner between two connected lines with a specified radius. The two original lines are shortened to meet the endpoints of the arc.

Chamfer lines adds a line segment to create a new edge between two connected lines with a specified setback. The two original lines are shortened to meet the endpoints of the new segment.

Extend lines to meet lengthens two selected lines until they intersect each other. The two lines will share a coincident endpoint.

Merge polygons combines two or more selected polygons into one new polygon that is the union of the original shapes.

Subtract polygons subtracts one or more polygons from another polygon, resulting in a new polygon that is the difference of the original shapes. The first-selected polygon(s) are subtracted from the last-selected polygon.

Intersect polygons results in a new polygon that is the shape of the overlapping area between two or more selected polygons.

KiCad provides tools to convert graphic objects to other types of objects, other types of objects to graphic objects, and graphic objects to other kinds of graphic objects. These tools are used by selecting the shapes you want to convert, right clicking, and then choosing the desired result object from the Create From Selection submenu. Most types of object conversions have several conversion options that are presented in a settings dialog. The exact options differ based on the target object type.

When converting to a graphic polygon, rule area, or zone, there are several options for how to convert the source objects into a polygonal outline.

Most conversions provide a delete source objects after conversion option, which will result in the original object being deleted during the conversion, only leaving the new object in place. If this option is not selected, the conversion will leave the original object in place in addition to the new object. The original object will be selected following the conversion so that it can be manually deleted by pressing Delete.

The following conversion types are available:

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.

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

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

There are several formatting options: text can be bolded, italicized, left/right/center aligned, and reversed. Regular text objects (not text boxes) can also have their vertical alignment adjusted. The knockout option, which is also limited to regular text objects, adds a solid rectangle surrounding the text and makes the text itself a negative cutout.

The text itself can use any TTF font available on your system, or the built-in KiCad stroke font.

You can adjust the text size with the text width and text height controls. When you are using the KiCad font, you can also adjust the stroke width with the thickness control.

Position X and position Y control the text object’s location. These properties are not available for text boxes.

Orientation is the rotation angle of the text object. You can select an angle in 90 degree increments from the dropdown, or type in an arbitrary angle.

Text boxes additionally have options controlling their border. The border checkbox makes the border visible or invisible. For visible borders, you can adjust the border’s thickness with the border width control and the line style with the border style control (solid, dashed, dotted, dash-dot, or dash-dot-dot).

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

覆盖值： 启用后，您可以直接在 值 字段中输入测量值，而不是实际测量值。

前缀： 此处输入的任何文字都将显示在测量值之前。

后缀： 此处输入的任何文字都将显示在测量值之后。

图层: 选择尺寸标注对象存在于哪个图层。

单位： 选择显示测量值的单位。 当更改电路板编辑器的显示单位时，自动 单位会导致尺寸标注单位发生变化。

单位格式： 从几种内置的单位显示风格中选择。

精度： 选择要显示多少位的精度。

大多数尺寸标注文本选项与其他图形文本对象的选项相同（见上面的图形对象部分）。 也有一些特殊的选项适用于尺寸标注文本：

定位模式：选择是手动定位尺寸标注文本，还是自动保持与尺寸测量线对齐。

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

线条粗细： 设置构成标注形状的图形线的粗细。

Arrow length: Sets the length of the arrow segments of the dimension’s shape. A negative arrow length reverses the arrow direction.

延长线偏移：设置从测量点到延长线起点的距离。

Extension line overshoot: Sets the distance from the dimension’s line to the end of the extension lines.

值： 输入要在引线行末尾显示的文本。

文本框： 选择所需的文本周围的边界（圆形、矩形或无）。

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

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.

KiCad supports displaying reference images in the canvas. These are background images that you can use to help you lay out a board; they are purely for reference during the design process and are not included in any fabrication outputs.

To add a reference image, use the button on the right toolbar and select the desired reference image file.

Once the image has been added to the canvas, you can scale it by dragging the editing canvas or open its properties dialog (E) and set the scale explicitly in the Image tab. Here you can also Convert to Greyscale if you wish.

Reference images have an associated layer; they are shown and hidden along with this layer. The layer initially associated with a reference image is the layer that was active when the image was added. You can change the associated layer in the image’s properties.

Another way to hide reference images is with the appearance manager. You can show or hide all reference images by toggling the visibility of Image objects in the Objects tab ( button). You can also adjust the opacity of reference images here.