当 Pcbnew 第一次运行时，如果在 KiCad 配置文件夹中没有找到全局封装表文件 fp-lib-table，那么 Pcbnew 将询问如何创建这个文件：

The first option is recommended (Copy default global footprint library table (recommended)). The default footprint library table includes all of the standard footprint libraries that are installed as part of KiCad.

If this option is disabled, KiCad was unable to find the default global footprint library table. This probably means you did not install the standard footprint libraries with KiCad, or they are not installed where KiCad expects to find them. On some systems the KiCad libraries are installed as a separate package.

Footprint library management is described in more detail later.

主 Pcbnew 用户界面如上所示，其中指出了一些关键元素：

编辑画布是正在设计的板上的视图。您可以平移和缩放到电路板的不同区域，也可以翻转视图以从底部显示电路板。

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

Several other zoom tools are available in the top toolbar:

The cursor’s current position is displayed at the bottom of the window (X and Y), along with the current zoom factor (Z), the cursor’s relative position (dx, dy, and dist), the grid setting, and the display units.

The relative coordinates can be reset to zero by pressing Space. This is useful for measuring distance between two points or aligning objects.

The Ctrl+F1 shortcut displays the current hotkey list. The default hotkey list is included in the Actions Reference section of the manual.

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

Many actions do not have hotkeys assigned by default, but hotkeys can be assigned or redefined using the hotkey editor (Preferences → Preferences…​ → Hotkeys).

Hotkeys are stored in the file user.hotkeys in KiCad’s configuration directory. The location is platform-specific:

KiCad can import hotkey settings from a user.hotkeys file using the Import Hotkeys button in the hotkey editor.

Pcbnew 中的层表示线路板上的物理铜层，以及用于定义诸如丝印、阻焊和电路板边缘的图形层。 在编辑器中始终有一个处于活动状态的层。 活动图层被画在其他层之上，并且将是指定给新创建对象的层。 活动图层在顶部工具栏的层选择器下拉框中显示，并在外观面板中也高亮显示。 若要变更活动图层，可以左键单击外观面板中的图层名称、使用顶部工具栏中的下拉图层选择器或使用快捷键。 可以隐藏图层以简化电路板视图。即使层是活动层，也可以隐藏该层。

外观面板提供用于管理 Pcbnew 绘图画布中对象的可见性、颜色和不透明度的控件。它有三个选项卡：图层选项卡包含电路板层的控件，对象选项卡包含不同类型图形对象的控件，网络选项卡包含飞线和铜项外观的控件。

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

可以通过在单击或拖动的同时按住快捷键来修改选择操作。单击以选择单个项目时，将应用以下快捷键：

拖动以执行选框时，将应用以下快捷键：

Pcbnew 窗口右下角的选择过滤器面板控制可以用鼠标选择哪些类型的对象。关闭对不需要的对象类型的选择可以更容易地选择密集电路板中的项目。“所有项目”复选框是打开和关闭其他项目的快捷方式。“锁定的项目”复选框独立于其他复选框，并控制是否可以选择已锁定的项目。您可以在选择过滤器中的任何对象类型上单击鼠标右键以快速更改过滤器，使其仅允许选择该类型的对象。

当一个连接的铜线项目被选中时，你可以使用右键菜单中的 "扩展选择" 命令或热键 U 将选择扩展到同一网络的其他铜线项目。 第一次运行这个命令时，选择将被扩展到最近的焊盘。 第二次，选择将被扩展到所有层上的所有连接项。

Selecting an object displays information about the object in the message panel at the bottom of the window. Double-clicking an object opens a window to edit the object’s properties.

按 Esc 将始终取消当前工具或操作，并返回到选择工具。在选择工具处于活动状态时按 Esc 将清除当前选择。

电气网络（或一组网络）可以在 PCB 编辑器中被高亮显示，以显示该网络是如何在 PCB 上布线的。 通过在 PCB 编辑器中选择要高亮的网络，或者在启用交叉探测高亮时在原理图编辑器中选择相应的网络，可以激活网的高亮（见下文）。 当网络高亮激活时，高亮的网或网将以较亮的颜色显示，所有其他项目将以比正常颜色更暗的颜色显示。

有三种方法可以点击一个或多个网络在 PCB 编辑器中高亮：点击铜对象后使用热键 ` ，使用任何铜对象的上下文菜单，以及外观面板的网络选项卡的上下文菜单。当您按下高亮网络热键时，任何选定铜件的网络将被高亮。如果未选中铜项，则编辑器光标下的铜项的网络将高亮。如果光标下没有铜项目，则任何现有的高亮都将被清除。也可以使用清除高操作 (热键 ~) 清除高亮。

选择一个或多个网络进行高亮时，左侧工具栏上的切换网络高亮显示操作变为启用(也可通过热键 Ctrl+` 访问)。此操作将打开或关闭高亮，而无需选择要高亮的新网络。

KiCad 允许在原理图和 PCB 之间进行双向交叉探测。 有几种不同类型的交叉探测。

选择交叉探测 允许您在原理图中点击一个符号或引脚，在 PCB (如果存在) 中点击相应的封装或焊盘，反之亦然。 默认情况下，交叉探查将导致显示以交叉探查的项目为中心并缩放到合适的位置。 可以在偏好设置对话框的显示选项部分禁用此行为。

高亮交叉探测 允许您同时高亮原理图和 PCB 中的网络。 如果在偏好设置对话框的显示选项部分中启用了选项 "高亮交叉网络"， 则在原理图编辑器中高亮某个网络或总线将导致相应的一个或多个网络在 PCB 编辑器中高亮。

左侧工具栏提供了更改 Pcbnew 中项目显示的选项。

KiCad 中的印刷电路板通常由代表电子元件及其焊盘的 封装、定义这些焊盘如何彼此连接的 网络、形成每个网络中焊盘之间的铜连接的 布线、过孔 和 填充区 以及定义电路板边缘、丝印标记和任何其他所需信息的各种图形形状组成。

KiCad 通常会将 PCB 上的网络信息与相关的原理图保持同步，但也可以直接在 PCB 编辑器中创建和编辑网络。

KiCad 能够创建多达 32 个铜层、14 个技术层 (丝印、阻焊、元件粘合剂、焊膏等) 和 13 个通用绘图层的印刷电路板。

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

KiCad 目前支持每个工程/原理图一个电路板文件。

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

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

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

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

也可以创建没有匹配原理图的电路板，尽管此工作流程有一些限制，不建议大多数用户使用。为此，您必须独立启动 PCB 编辑器(而不是从 KiCad 工程管理器启动)。在开始设计之前，最好保存电路板文件，该文件还将创建一个工程文件来存储电路板设置。使用 "另存为…​" 从文件菜单选择保存电路板文件的位置。将在您选择保存电路板文件的相同位置创建一个同名的工程文件。

在开始您的线路板设计之前，使用电路板设置对话框来配置电路板的基本参数。要打开电路板设置，请单击顶部工具栏中的 图标或选择 "电路板设置…​" 从文件菜单中选择。

放置和绘图工具位于右边的工具栏中。 当一个工具被激活时，它将一直处于激活状态，直到选择了一个不同的工具或用 Esc 键取消该工具。 当任何其他工具被取消时，选择工具总是被激活。

某些工具栏按钮在调色板中有多个可用工具。这些工具由按钮右下角的小箭头表示：

要显示调色板，你可以在工具上点击并按住鼠标按钮，或者点击并拖动鼠标。 调色板关闭时将显示最近使用的工具。

移动、拖动和绘制电路板元素时，栅格、焊盘和其他元素可以具有捕捉点，具体取决于用户偏好设置中的设置。在复杂的设计中，捕捉点可能离得太近，这会使当前的工具操作变得困难。使用下表中的快捷键可以在移动鼠标时禁用栅格和对象捕捉。

所有对象都有可在对话框中编辑的属性。 使用热键 E 或从右键菜单中选择属性来编辑所选项目的属性。 只有当你选择的所有项目都是同一类型时，你才能打开属性对话框。 要想一次编辑不同类型的项目的属性，请参阅下面关于批量编辑工具的章节。

在属性对话框中，任何包含数字值的字段也可以接受一个基本的数学表达式，从而得到一个数字值。 例如，一个尺寸可以被输入为 2 * 2mm，结果是 4mm 的值。 支持基本算术运算符以及用于定义运算顺序的圆括号。

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

图形对象 (直线、圆弧、矩形、圆、多边形和文本)可以存在于任何图层上，但不能分配给网络。矩形、圆和多边形可以在其属性对话框中设置为填充或轮廓。线宽属性将控制轮廓的宽度，即使是填充形状也是如此。填充形状的线宽可以设置为 "0" 以禁用轮廓。

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，但通常被添加到用户层之一。 KiCad 目前支持四种不同类型的标注：对齐、正交、中心和引线。

对齐 标注 () 表示两点之间距离的测量。 测量轴是连接这两个点的线，标注图形与该轴保持平行。

正交 标注 () 也测量两点之间的距离，但测量轴是 X 轴或 Y 轴。 换句话说，这些标注表示两点之间距离的水平或垂直分量。 创建正交标注时，在选择要测量的两个点后，可以根据放置标注的位置选择要用作测量轴的轴。

中心 标注 () 创建一个十字标记来指示一个点或圆或圆弧的圆心。

引线 标注 () 创建一个箭头，将一条引线连接到文本字段。 此文本字段可以包含任何文本以及文本周围的可选圆形或矩形框。 这种类型的标注通常用来提醒人们注意设计的某些部分，以便在制造说明中参考。

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

KiCad 具有交互式布线器的功能：

默认情况下，布线器在放置布线时尊重配置的设计规则：新布线的尺寸（宽度）将取自设计规则，在确定新布线和过孔的放置位置时，布线器将尊重设计规则中设置的铜间隙。 如果需要的话，可以通过使用高亮冲突布线器模式和打开布线器设置中的允许 DRC 违规选项来禁用这种行为（见下文）。

布线器有三种模式，可以随时选择。 布线器模式用于布线新布线，但也用于使用拖动（热键 D）命令拖动现有布线时。 这些模式是：

使用哪种模式是一个偏好问题。 对于大多数用户，我们建议使用推挤模式以获得最高效的布线体验，或者，如果您不希望布线器修改未被布线的线段，则建议使用绕走模式。请注意，推挤和绕走模式始终创建水平、垂直和 45 度 (H/V/45) 布线段。如果需要使用 H/V/45 以外的角度布线段，则必须使用高亮碰撞模式，并在交互布线器设置对话框中启用自由角度模式选项。

有五个主要的布线功能。单轨布线、差分对布线、调整单轨长度、调整差分对的长度和调整差分对的偏移 (相位)。 所有这些都存在于顶部工具栏上的路由菜单下拉菜单（单独）和绘图工具栏上的两个重载图标中，在右侧的绘图工具栏上。 上面介绍了重载图标的使用。 一个用于两个布线功能，一个用于三个调谐功能。 此外，布线菜单允许选择设置层对和交互式布线器设置。

要布线，请点击布线 图标（从绘图工具栏或从顶部工具栏 布线 下）或使用热键 X。 点击一个起始位置，选择要布线的网络，并开始布线。 被布线的网络会自动高亮显示，网络的允许间隙会在被布线的线端周围用灰色的轮廓表示。 可以通过改变 "偏好设置" 对话框中的 "间隙轮廓" 设置来禁用间隙轮廓。

当布线器处于活动状态时，将从布线起点到编辑器光标绘制新的线段。这些线段是未固定临时 (unfixed temporary) 对象，它们显示当您使用左击或 Enter 键来固定布线 (fix the route) 时将创建哪些线段。非固定布线段以比固定布线段更亮的颜色显示。当您使用 Esc 键或通过选择另一个工具退出布线器时，将只保存固定布线段。完成布线操作(热键 End) 将固定所有布线并退出布线器。

在布线时，可以使用撤消最后一个布线段命令 (热键 Backspace) 取消固定最近固定的布线。您可以重复使用此命令以后退已固定的布线。

在以前的 KiCad 版本中，使用鼠标左键或 Enter 来固定已布线的线段会固定所有线段，但不包括鼠标光标位置结束的线段。 在 KiCad 6 中，这种行为现在是可选的，默认情况下，所有的线段 包括 在鼠标光标位置结束的线段都会被固定。 通过在交互式布线器设置对话框中禁用 "点击后固定所有线段" 选项，可以恢复旧的行为。

布线时，可以按住 Ctrl 键禁用网格捕捉，按住 Shift 键禁用对焊盘和过孔等对象的捕捉。

大多数对象可以通过其属性对话框、右键上下文菜单或使用 "切换锁定" 热键（L）来锁定。 被锁定的对象不能被选择，除非选择过滤器中的 "被锁定的项目" 复选框被启用。 试图移动锁定的项目将导致一个警告对话框：

在这个对话框中选择 "覆盖锁定" 将允许移动锁定的项目。 选择 "确定" 将允许你在选择中移动任何未上锁的项目；留下锁定的项目。 选择 "不再显示" 将使你在剩下的会话中记住你的选择。

测量工具允许你在 PCB 上的各点之间进行距离和角度测量。 要激活该工具，请点击右侧工具栏的 图标，或使用热键 Ctrl+Shift+M。 一旦该工具被激活，点击一次以设置测量起点，然后再点击一次以完成测量。

设计规则检查器用于验证 PCB 是否符合电路板设置对话框中建立的所有要求，以及所有焊盘是否按照网表或原理图连接。 KiCad 可以在布线线段时自动防止一些违反设计规则的行为，但许多其他的行为是无法自动防止的。 这意味着在为 PCB 创建制造文件之前，必须使用设计规则检查器。

要使用设计规则检查器，请点击顶部工具栏的 图标，或者从检查菜单中选择设计规则检查器。

DRC 控制窗口的顶部部分包含一些控制设计规则检查器的选项：

重新填充所有敷铜后再执行 DRC： 启用后，每次运行设计规则检查器时都会重新填充敷铜。 如果未手动重新填充敷铜，禁用此选项可能会导致错误的 DRC 结果。

报告每个布线的所有错误： 启用后，将报告每个线段的所有间隙错误。 禁用时，将只报告第一个错误。 启用此选项将导致设计规则检查器运行速度变慢。

测试 PCB 和原理图之间的奇偶校验： 启用后，设计规则检查器除了测试 PCB 设计规则外，还将测试原理图和 PCB 之间的差异。 在独立模式下运行 PCB 编辑器时，该选项不起作用。

运行 DRC 后，任何违规行为都会显示在 DRC 控制窗口的中间部分。 违反规则、未连接的项目以及原理图和 PCB 之间的差异会显示在三个不同的标签中。 违规列表下面的控件可以用来显示或隐藏违规，这取决于其严重程度。 在运行 DRC 后，可以使用保存按钮创建一个纯文本格式的报告文件。

每项违规行为涉及 PCB 上的一个或多个对象。 在违章列表中，涉及的对象列在违章下面。 点击列表中的违规行为将移动 PCB 编辑器的视图，使受影响的区域居中。 点击违章所涉及的对象之一将突出显示该对象。

右键单击列表视图中的违规行为将打开一个上下文菜单，其中包括排除所选违规行为的额外操作。 除非 DRC 控制窗口底部的 "排除" 复选框被激活，否则排除的违反行为会被隐藏。 被排除的违规行为在设计规则检查器运行期间会被记住。

The Find tool searches for text in the PCB, including reference designators, footprint fields, and graphic text. When the tool finds a match, the canvas is zoomed and centered on the match and the text is highlighted. Launch the tool using the () button in the top toolbar.

The Find tool has several options:

Match case: Selects whether the search is case-sensitive.

Words: When selected, the search will only match the search term with complete words in the PCB. When unselected, the search will match if the search term is part of a larger word in the PCB.

Wildcards: When selected, wildcards can be used in the search terms. ? matches any single character, and * matches any number of characters. Note that when this option is selected, partial matches are not returned: searching for abc* will match the string abcd, but searching for abc will not.

Wrap: When selected, search results will return to the first hit after reaching the last hit.

Search footprint reference designators: Selects whether the search should apply to footprint reference designators.

Search footprint values: Selects whether the search should apply to footprint value fields.

Search other text items: Selects whether the search should apply to other text items, including graphical text and footprint fields other than value and reference.

Search DRC markers: Selects whether the search should apply to the violation descriptions of DRC markers shown on the board.

The 3D Viewer shows a 3-dimensional view of the board and the components on the board. You can view the board from different perspectives, show or hide different types of components, cross-probe from the PCB Editor to the 3D viewer, and generate raytraced renders of the board.

网络检查器允许你查看电路板中所有网络的统计数据。 要打开检查器，请点击外观面板中的网络部分顶部的 图标，或者从检查菜单中选择网络检查器。

点击网络列表中的一个网络会在电路板上高亮显示该网络。 单击列标题允许您按该列对网络列表进行排序。

分组依据字段允许您将不同的网络组合在一起，并查看组合的网络的总长度。 例如，如果您有两个名为 DATA0 和 DATA0_EXT 的网络，则使用值为 DATA0* 的分组依据将创建一个包含这两个网络的组。 通过将分组依据模式从通配符更改为 RegEx (正则表达式)，可以创建更复杂的分组。 分组依据模式的子字符串 (Substr) 变体将为以不同方式匹配该模式的每组网络创建组。

例如，如果您有 U1D+，U1D-，U2D+ 和 U2D-，分组模式 U*D 将在通配符模式下匹配所有四个网络，创建一个单一的组 U*D。 在通配符子串模式下，它将匹配所有四个网络，但创建两个不同的组：U1D 和 U2D。

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

KiCad 使用 Gerber 文件作为其 PCB 制造的主要绘图格式。 要创建 Gerber 文件，请从文件菜单中打开绘图对话框，或从文件菜单的制造输出部分选择 Gerbers。 绘图对话框将打开，允许你配置和生成 Gerber 文件。

KiCad 可以生成大多数 PCB 制造工艺所需的 Excellon 或 Gerber X2 格式的数控钻孔文件。 KiCad 还可以生成钻孔图：一个显示钻孔位置的电路板图形图。 从 "制造输出" 菜单中选择 "生成钻孔文件" 选项来打开该对话框：

输出文件夹： 选择要保存生成的钻孔和映射文件的文件夹。 如果输入相对路径，则它将相对于工程目录。

钻孔文件格式： 选择是生成 Excellon 钻孔文件 (大多数 PCB 制造商都需要)还是 Gerber X2 文件。

镜像 Y 轴： 对于卓越文件，选择是否镜像 Y 轴坐标。 当由第三方制造 PCB 时，通常不应使用该选项，并且是为了方便自己制造 PCB 的用户而提供的。

最小钻头： 对于 Excellon 文件，选择是否输出最小钻头，而不是完整的文件钻头。 除非制造商要求，否则不应启用此选项。

PTH (电镀孔) 和 NPTH (非电镀孔) 为单文件： 默认情况下，会在两个不同的 Excellon 文件中生成电镀孔和非电镀孔。 启用此选项后，这两个文件将合并为单个文件。 除非制造商要求，否则不应启用此选项。

椭圆孔钻孔模式： 控制椭圆孔在 Excellon 钻孔文件中的表示方式。 默认设置 使用布线命令 对于大多数制造商都是正确的。 如果制造商要求，请仅选择 使用备用钻孔模式 设置。

映射文件格式： 选择绘制钻孔映射的输出格式。

钻孔原点： 选择钻孔文件的坐标原点。 绝对 将使用左上角的页面原点。 钻孔/放置文件原点 将使用电路板设计中指定的原点。

钻孔单位： 选择钻孔坐标和尺寸的单位。

零的格式 控制 Excellon 钻孔文件中数字的格式。 请根据制造商的建议在此处选择一个选项。

元件放置文件是一种文本文件，它列出了电路板上的每个元件（封装）以及其中心位置和方向。 这些文件通常用于对取放机进行编程，如果你订购的是完全组装的 PCB，你的制造商可能需要这些文件。

格式： 选择生成纯文本 (ASCII)、逗号分隔文本 (CSV) 或 Gerber 放置文件格式。

单位： 在放置文件中选择元件位置的单位。

文件： 选择是为电路板正面和背面的封装生成单独的文件，还是生成一个合并两面的文件。

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

使用通孔焊盘排除所有封装： 启用时，如果封装包含任何通孔焊盘，即使其制造类型设置为 SMD，也将从放置文件中排除封装。

包括电路板边缘层： 对于 Gerber 放置文件，控制电路板轮廓是否包含在封装放置数据中。

使用钻孔/放置文件原点： 启用后，元件位置将相对于电路板设计中设置的钻孔/放置文件原点。 禁用时，位置将相对于页面原点 (左上角)。

KiCad 还可以从电路板设计生成封装报告文件、IPC-D-356 网表文件和物料清单 (BOM)。 这些输出格式没有可配置的选项。

KiCad 可以使用文件菜单中的打印操作将电路板视图打印到标准打印机上。

包含层： 选择要包含在打印输出中的层。未选中的层将不可见。

输出模式： 选择以黑白或全彩方式打印。

打印边框和标题块： 启用后，将打印页面边框和标题块。

根据外观管理器的对象选项卡打印： 启用后，任何隐藏在外观面板的对象选项卡中的对象都将隐藏在打印输出中。 禁用时，如果在包含的图层区域中选择了这些对象所在的图层，则将打印这些对象。

打印背景色： 全彩色打印时，该选项控制是否打印视图背景色。

使用不同的颜色主题进行打印： 当以全色打印时，此选项允许使用不同的颜色主题进行打印。 禁用时，电路板编辑器使用的颜色主题将用于打印。

钻孔标记： 控制是以实际大小显示钻孔，还是以较小的尺寸显示钻孔，还是将其隐藏在打印输出中。

打印镜像： 启用后，打印输出将被水平镜像。

每层打印一页： 启用后，在包含图层区域中选择的每一图层都将打印到单独一页。 如果启用此选项，在所有页面上打印电路板边缘 选项控制是否将 Edge.Cuts 层添加到每个打印页面。

比例： 控制打印输出相对于页面设置中配置的页面大小的比例。

KiCad 可以将电路板设计导出为各种第三方格式，以便与外部软件一起使用。 这些功能可以在文件菜单的导出部分找到。

Specctra .DSN： 创建适合导入到某些第三方自动布线软件中的文件。 此导出器没有可配置的选项。

KiCad’s footprint library management system allows directly using several types of footprint libraries:

KiCad uses a table of footprint libraries to map footprint libraries of any supported library type to a library nickname. KiCad uses a global footprint library table as well as a table specific to each project. To edit either footprint library table, use Preferences → Manage Footprint Libraries…​.

The global footprint library table contains the list of libraries that are always available regardless of the currently loaded project. The table is saved in the file fp-lib-table in the KiCad configuration folder. The location of this folder depends on the operating system being used.

The project specific footprint library table contains the list of libraries that are available specifically for the currently loaded project. If there are any project-specific footprint libraries, the table is saved in the file fp-lib-table in the project folder.

Pcbnew 有各种偏好设置，可以通过偏好设置对话框进行配置。与 KiCad 的所有部分一样，Pcbnew 的偏好设置存储在用户配置目录中，并且在 KiCad 次要版本之间相互独立，从而允许多个版本与独立的偏好设置并行运行。

偏好设置对话框的第一部分 (通用、鼠标和触摸板以及快捷键) 在所有 KiCad 程序之间共享。KiCad 手册中“通用偏好设置”部分详细介绍了这些部分。请注意，尽管快捷键部分在所有程序之间共享，但有许多特定于 Pcbnew 的快捷键只有在 Pcbnew 运行时才会出现在列表中。

KiCad’s custom design rule system allows creating design rules that are more specific than the generic rules available in the Constraints page of the Board Setup dialog. Custom design rules have many applications, but in general they are used to apply certain rules to a portion of the board, such as a specific net or netclass, a specific area, or a specific footprint.

自定义设计规则存储在一个扩展名为 kicad_dra 的单独文件中。当您开始向项目添加自定义规则时，会自动创建此文件。如果您在项目中使用自定义规则，请在备份或提交到版本控制系统时，确保将 kicad_dra 文件与 kicad_pcb 和 kicad_pro 文件一起保存。

脚本允许您使用 Python 语言自动执行 KiCad 中的任务。可以通过 Python "操作插件" 向 KiCad 添加功能，这些插件可以添加到顶部工具栏。也可以编写与 KiCad 文件交互的独立脚本，例如，从电路板文件自动生成制造输出。

本手册涵盖了一般脚本编写概念。希望编写或修改脚本的用户还应使用 https://docs.kicad.org/doxygen-python/namespaces.html 上的 Doxygen 文档。

KiCad 6 或更新版本需要 Python 3 来支持脚本。Python 2 已不再被支持。

KiCad can export an IDF representation of the board for use in mechanical CAD software. Below is some guidance on attaching IDF component outlines to footprints, creating new IDF component outlines, and a description of the IDF utilities included with KiCad.

The actions below are available in Pcbnew. Hotkeys can be assigned to any of these actions in the Hotkeys section of the preferences.

The actions below are available in the 3D Viewer. Hotkeys can be assigned to any of these actions in the Hotkeys section of the preferences.

The actions below are available across KiCad, including in Pcbnew. Hotkeys can be assigned to any of these actions in the Hotkeys section of the preferences.