The display order for board layers is dynamic and depends on which layer is selected as the active layer. The active layer is always drawn on top of other layers. In addition, layers that are related to the active layer are drawn on top of layers that are unrelated. For example, if you make B.Silkscreen the active layer, then all of the other back layers (B.Cu, B.Adhesive, B.Paste, B.Mask, B.Fab, and B.Courtyard) will be drawn on top of the front, user, and inner copper layers, with B.Silkscreen topmost. If you make Edge.Cuts active, then it will be drawn on top, and the User.* layers and Margin will also be be brought to the front.

在外观面板的 “层” 选项卡中，每个电路板层都显示了其颜色和可见性状态。 活动层在色块的左边有一个箭头指示器。 左键点击一个图层来选择它作为活动图层。 左键单击相应的可见性图标，在可见和隐藏之间切换该图层。 双击或中击色块来改变该图层的颜色。

在图层列表下方是一个包含图层显示选项的可展开面板。第一个设置控制非活动图层的显示方式：正常、暗显或隐藏。层显示模式可用于简化视图并聚焦于单个层。当非活动层显示模式为 "暗显" 或 "隐藏" 时，不能选择非活动层上的对象。您可以使用快捷键 Ctrl+H 快速切换这些显示模式。

翻转电路板视图 将显示电路板，就像从底部看一样(即绕 Y 轴镜像)。 此选项也可在视图菜单中使用。

外观面板的 "对象" 选项卡与 "图层" 选项卡类似。 主要区别在于，有些对象没有颜色设置，而四种类型的对象（布线、过孔、焊盘和敷铜）有不透明度控制滑块。 这里的不透明度设置将与图层颜色中设置的任何不透明度相乘。 默认情况下，所有对象都是完全不透明的，除了敷铜，敷铜被设置为半透明，以便通过敷铜区域更容易看到对象。

图层预设存储了哪些图层和对象是可见和隐藏的，以便于调用。 有几个内置的图层预设，您也可以保存您自己的自定义预设。 自定义预设存储在一个电路板的工程设置中，因为预设可能是特定于某个电路板的层叠。

要加载一个预设，请从外观面板底部的预设下拉菜单中选择它，或者通过按住 Ctrl 并按 Tab 来使用快速切换器。 一旦快速切换器窗口出现，你可以按 Tab 和 Shift+Tab 来循环浏览可用的预设。 当你放开 Ctrl 键时，高亮显示的预设将被加载。

To save a custom preset, first use the visibility controls to choose which layers you want visible, then choose Save preset…​ from the Presets drop-down menu. Give your preset a name and it will now be available via the drop-down menu and the quick switcher. To modify a custom preset, follow the same process and save the modified version with the same name to overwrite the existing version. To delete a custom preset, choose the Delete preset…​ option from the drop-down menu and select the preset to be deleted from the list.

Viewports store the current view location and zoom level so you can quickly switch back to it later, or switch between several saved views.

To load a viewport, choose it from the Viewports drop-down menu at the bottom of the appearance panel or use the quick switcher by holding down Shift and pressing Tab. Once the quick switcher window appears, you can press Tab to cycle through the stored viewports. When you let go of the Shift key, the highlighted viewport will be loaded.

To save a new viewport, scroll and zoom to show the desired area of the board, then choose Save viewport…​ from the Viewports drop-down menu. Give your viewport a name and it will now be available via the drop-down menu and the quick switcher. To modify an existing viewport, save a new viewport with the same name to overwrite the existing version. To delete a viewport, choose the Delete viewport…​ option from the drop-down menu and select the preset to be deleted from the list.

外观面板的网络选项卡显示电路板中所有网络和网络类的列表。每个网络都有一个可见性控件，用于控制该网络在飞线中的可见性。在飞线中隐藏网络不会改变电路板的连接性，也不会影响设计规则检查器；这只是为了使飞线更容易理解。

每个网络和网络类还可以指定一种颜色。默认情况下，此颜色适用于网络 (或网络类中的所有网络) 的飞线。默认情况下，网络没有颜色；这由色样中的棋盘格图案指示。双击或右键单击网络或网络类颜色样本以设置颜色。

您还可以通过外观面板选择并高亮网络和网络类：右击网络或网络类以在菜单中显示这些选项。

网络类列表下面是一个包含网络显示选项的可扩展面板。第一个选项控制如何应用网络颜色。当选择了 “所有” 时，属于网络或网络类的所有铜对象 (焊盘、布线、过孔和敷铜) 都将呈现所选的颜色。当选中 “飞线” (默认值)时，只有飞线受网络和网络类颜色的影响。 当选择 “无” 时，网络和网络类颜色被忽略。

第二个选项控制如何绘制飞线。“所有图层” 表示将在所有未连接的项目之间绘制飞线。“可见层” 意味着不会向隐藏层上的项目绘制任何最新的飞线，即使这些项目是未连接的。

在 "电路板设置" 中，有两个部分用于配置电路板的层叠和层。 "电路板编辑器层" 部分用于启用或禁用技术层（非铜层），如果需要的话，还可以给各层自定义名称。 物理层叠部分用于配置铜层的数量，以及铜层和电介质层的物理参数，如厚度和材料类型。介电层、阻焊层和丝印层可以被分配颜色，这将影响电路板在 3D 查看器中的外观。

要配置电路板的层叠，从物理层叠部分开始：

Set the number of copper layers in the upper left corner and then enter the physical parameters of the stackup if desired. These parameters may be left at their default values, but note that the board thickness value will be used when exporting a 3D model of the board, and layer thicknesses will be included in net length calculations for any nets that include vias. If you plan to use these features, it is a good idea to ensure that the stackup thickness is correct.

接下来，如果需要，可以使用电路板编辑器层部分重命名或隐藏您不会在设计中使用的非铜层。例如，如果您不打算在设计中使用底层丝印，请取消选中 B.Silkcreen 层旁边的复选框。

在电路板编辑器对话框的电路板表面处理(Board Finish)和阻焊/锡膏部分可以找到一些其他的电路板层叠设置。电路板表面处理部分包含用于定义铜的表面处理和特殊功能 (如刻痕或边缘电镀) 的设置。请注意，这些设置目前只影响作为 Gerber 文件一部分的电路板属性输出。

阻焊/锡膏部分允许全局调整电路板上焊盘的铜形和阻焊/锡膏形之间的间隙（正或负）。 这些值将被添加到在个别封装或焊盘上设置的任何间隙覆盖。 正的间隙值将导致阻焊层或锡膏开口的形状比铜的形状 更大。 负的间隙值将导致开口比铜的形状 更小。

电路板设置对话框的文本和图形默认值部分可用于配置将用于放置在电路板上的新文本和图形形状的属性。

可以为对话框中显示的六种不同类别的图层配置线粗细、文本大小和文本外观。此外，可以为所有图层配置标注对象的特性。有关标注属性的更多详细信息，请参阅下面的标注部分。

虚线的外观是在 "格式化" 部分控制的。虚线长度 控制虚线的长度，而 间隔长度 控制虚线和圆点之间的间距。虚线和间隔的长度是相对于行宽而言的：间隔长度为 2 意味着是行宽的两倍。

文本替换变量可以在文本变量部分创建。 这些变量允许你将变量名称替换为任何文本字符串。 这种替换发生在变量名称在 ${VARIABLENAME} 的变量替换语法内的任何地方。

例如，您可以创建一个名为 VERSION 的变量，并将文本替换设置为 1.0。 现在，在 PCB 上的任何文本对象中，你可以输入 ${VERSION}，KiCad 将替代 1.0。 如果你把变量改为 2.0，每个包括 ${VERSION} 的文本对象都会自动更新。 你也可以混合使用普通文本和变量。 例如，你可以创建一个文本对象，内容为 版本：${VERSION}，它将被替换为 版本：1.0。

文本变量也可以在 原理图设置 中创建。 文本变量是项目范围内的；在原理图编辑器中创建的变量在电路板编辑器中也可用，反之亦然。

还有一些 内置系统文本变量。

设计规则控制交互式布线器的行为、敷铜和设计规则检查器。设计规则可以随时修改，但我们建议您在电路板设计过程开始时建立所有已知的设计规则。

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). Note that footprints added in this way will not be automatically associated with a symbol or have nets assigned to their pads, and subsequent updates from the schematic will remove these unassociated footprints unless the footprint is locked or the Delete footprints with no symbols option is unchecked in the Update PCB From Schematic dialog. For these reasons, it is usually recommended to avoid manually adding footprints to the board. Manually adding footprints is necessary for PCB-only workflows, and can also be useful for adding logos or other footprints that do not need a corresponding schematic symbol.

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.

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. Only one footprint at a time can be dragged.

Flip a footprint to the opposite side of the board with the F hotkey. Any parts of the footprint on a front layer will be swapped to the corresponding back layer, and vice versa.

Rotate a footprint 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.

右侧工具栏可以用来创建直线（, 默认快捷键 Ctrl+Shift+L）、弧线（, 默认快捷键 Ctrl+Shift+A）、矩形（），圆（，默认快捷键 Ctrl+Shift+C），和多边形（，默认快捷键 Ctrl+Shift+P）。

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。

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 使用 Edge.Cuts 层上的图形对象来定义电路板的边框。 边框必须是一个连续（封闭）的形状，但可以由不同类型的图形对象组成，如直线和弧，或者是一个单一的对象，如矩形或多边形。 如果没有定义电路板的边框，或者电路板的边框无效，那么一些功能，如 3D 查看器和一些设计规则的检查将无法发挥作用。

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.

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

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）。

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.

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。

间隙和约束解析工具允许你检查哪些间隙和设计约束规则应用于选定的项目。 当设计具有复杂设计规则的 PCB 时，这些工具可以提供帮助，因为在这种情况下并不总是清楚哪些规则适用于哪些对象。

要检查两个对象之间适用的间隙规则，选择这两个对象并从 检查 菜单中选择 间隙解析。 间隙报告对话框将显示每个铜层上的对象之间所需的间隙，以及产生该间隙的设计规则。

要检查适用于单一对象的设计约束，选择它并从 检查 菜单中选择 约束解析。 约束报告对话框将显示适用于该对象的所有约束。

用鼠标左键拖动将旋转 3D 视图。 默认情况下，这是电路板的中心，但可以通过将光标移动到所需点上并按 Space 将轴心点重置为电路板上的新点。 滚动鼠标滚轮将放大或缩小视图。 按住 Ctrl 滚动可左右平移视图，按住 Shift 滚动可上下平移视图。 使用鼠标中键拖动也可以平移视图。

Different sized 3D grids can be set using the View → 3D Grid menu. Bounding boxes for each component can be enabled with Preferences → Show Model Bounding Boxes.

当 PCB 编辑器和 3D 查看器同时打开时，在 PCB 编辑器中选择一个封装也会在 3D 查看器中高亮显示该元件。高亮显示的颜色可以在 偏好设置 → 偏好设置…​ → 3D 查看器 → 实时渲染器 → 选择颜色 中调整。

The appearance manager is a panel at the right of the viewer which provides controls to manage the visibility, color, and opacity of different types of objects and board layers in the 3D view.

Each layer or type of object in the list can be individually shown or hidden by clicking its corresponding visibility icon. PCB layers can have their colors customized; double-click on the color swatch next to the item type to edit the item’s color and opacity. To use the colors selected in the Board Setup dialog’s Physical Stackup editor, enable the use board stackup colors option.

You can save an appearance configuration as a preset, or load a configuration from a preset, using the Preset selector at the bottom. The Ctrl+Tab hotkey cycles through presets; press Tab repeatedly while holding Ctrl to cycle through multiple presets. Several built-in presets are available: "Follow PCB Editor" matches the visibility settings in the PCB editor, "Follow PCB Plot Settings" matches the visibility settings selected in the Plot dialog, and "legacy colors" matches the default 3D Viewer color settings from older versions of KiCad.

Finally, you can save a viewport for later retrieval using the Viewports selector at the bottom. You can quickly cycle between saved viewports using Shift+Tab; pressing Tab repeatedly while holding Shift will cycle through multiple viewports.

当前的 3D 视图可以用 文件 → 将当前视图导出为 PNG…​ 或 将当前视图导出为 JPG…​，根据所需的图像格式，将其保存为一个图像。也可以用 按钮，或 编辑 → 复制 3D 图像 将当前视图复制到剪贴板上。

3D 查看器有一个光线跟踪渲染模式，它使用比默认渲染模式更精确的物理渲染模型来显示电路板。 光线追踪比默认渲染模式慢，但当需要最吸引人的视觉效果时，可以使用它。使用 按钮，或者使用 偏好设置→光线追踪 来启用光线追踪模式。在光线追踪模式下，3D 网格和选择高亮不会显示。

颜色和其他渲染选项，包括光线跟踪和非光线跟踪模式，都可以在 偏好设置 → 偏好设置…​ → 3D查看器 中调整。

许多查看选项是通过顶部的工具栏控制的。

The Net Inspector may report different net lengths than the length tuner, because the two tools have different purposes and calculate track/net lengths differently. In short, the Net Inspector sums up the total length of each track segment and via on a net, while the length tuner calculates the effective electrical length of a path between two points on a net. The specific differences are as follows:

包含层： 检查电路板上使用的每一个层在列表中是否被启用。 被禁用的图层将不会被绘制出来。

Plot on All Layers: Selected layers will be included in the plot for each layer selected in the include layers list. The additional layers are plotted on top of the base layer. You can reorder these layers using the arrow buttons at the bottom; items that are lower in the list are plotted after (on top of) items that are higher in the list.

输出目录： 指定打印文件的保存位置。 如果这是相对路径，则它是相对于工程目录创建的。

Plot drawing sheet: If enabled, the drawing sheet border and title block will be plotted on each layer. This should usually be disabled when plotting Gerber files.

绘制封装值： 如果启用，每个封装的值字段将绘制在其所在的任何层上 (除非特定封装的字段可见性被禁用)。

绘制位号： 如果启用，每个封装的位号字段将绘制在其所在的任何层上 (除非特定封装的字段可见性被禁用)。

Plot footprint text: If enabled, text fields in footprints will be plotted on whatever layers they exist on (unless the field visibility is disabled for a specific footprint). Disabling this option also disables the plot footprint values and plot reference designators options.

强制绘制不可见值/位号： 如果启用，将绘制所有封装值和位号，即使其中一些字段可见性被禁用。

在所有图层上绘制板边（Edge.Cuts）： 如果启用，Edge.Cuts(电路板边框) 图层将添加到所有其他层。 请向您的制造商咨询，了解此设置对于其制造过程的正确值是多少。

制造层上的草图焊盘： 如果启用，制造 (F.Fab，B.Fab) 层上的封装焊盘将绘制为未填充的边框，而不是填充的形状。

绘制前检查敷铜区域： 启用后，将在生成输出之前检查敷铜 (如果过期则重新敷铜)。 如果禁用此选项，绘制输出可能不正确！

钻孔标记： 对于 Gerber 以外的绘图格式，可以在所有钻孔的位置绘制标记。 钻孔标记可以按成品孔的实际尺寸 (直径) 创建，也可以按较小的尺寸创建。

缩放： 对于支持非 1:1 缩放的打印格式，可以设置打印比例。 自动缩放设置将缩放绘图以适合指定的页面大小。

绘图模式： 对于某些绘图格式，填充的形状可能只被绘制成边框（草图模式）。

使用钻孔/拾放文件原点： 启用后，绘制文件的坐标原点将是电路板编辑器中设置的钻孔/拾放文件原点。 禁用时，坐标原点将是绝对原点 (图框的左上角)。

镜像绘图： 对于某些绘图格式，设置此选项后输出会水平镜像。

负片绘图： 对于某些绘制格式，可能会将输出设置为负片模式。 在此模式下，将为电路板边框内的空白区域绘制图形，并在 PCB 中存在对象的位置留下空白区域。

不允许过孔盖油： 如果启用，过孔将在阻焊层 (F.Mask、B.Mask) 上不会被覆盖。 如果禁用，过孔将被阻焊层 (绿油) 覆盖。

使用 Protel 文件扩展名： 启用后，绘制的 Gerber 文件将使用基于 Protel (.GBL、.GTL 等) 的文件扩展名命名。 当禁用时，文件将有 .gbr 的扩展名。

生成 Gerber 作业文件： 开启后，Gerber 作业文件 (.gbrjob) 将与任何 Gerber 文件一起生成。 Gerber 作业文件是 Gerber 格式的扩展，包括有关 PCB 层叠、材料和表面处理的信息。 有关 Gerber 工作文件的更多信息，请访问链接：Ucamco 网站。

Subtract soldermask from silkscreen: When enabled, silkscreen will be automatically removed from board areas that aren’t covered by soldermask.

坐标格式： 配置坐标在绘制的 Gerber 文件中的存储方式。 请咨询您的制造商，了解他们对此选项的推荐设置。

使用扩展的 X2 格式： 启用后，绘制的 Gerber 文件将使用 X2 格式，其中包括有关网表和其他扩展属性的信息。 此格式可能与某些制造商使用的旧版 CAM 软件不兼容。

包含网表属性： 启用后，绘制的 Gerber 文件将包含可用于在 CAM 软件中检查设计的网表信息。 禁用 X2 格式模式时，此信息将作为注释包含在 Gerber 文件中。

禁用孔径宏： 启用后，所有形状都将绘制为图元，而不是使用孔径宏。 此设置仅应在您的制造商要求时用于与旧的或有缺陷的 CAM 软件兼容。

缩放系数： 控制电路板文件中的坐标将如何被缩放到 PostScript 文件中的坐标。 使用不同的 X 和 Y 比例因子的值将导致输出的拉伸/扭曲。 这些系数可以用来纠正 PostScript 输出设备中的缩放比例，以实现精确的输出比例。

布线宽度校正： 在绘制 PostScript 文件时，从布线、过孔和焊盘的尺寸中添加（或减去，如果是负的）一个全局系数。 这个系数可用于纠正 PostScript 输出设备中的错误，以实现精确的比例输出。

强制 A4 输出： 启用后，生成的 PostScript 文件将为 A4 大小，即使 KiCad 电路板文件大小不同。

精度： 控制将使用多少个有效数字来存储坐标。

Output mode: Controls whether the generated SVG file is in color or black and white.

使用图形项目的轮廓线绘图： DXF 文件中的图形形状没有宽度。 此选项控制如何将 KiCad 电路板中具有宽度 (厚度) 的图形绘制到 DXF 文件。 启用此选项后，将绘制图形的外边框。 禁用此选项时，将绘制图形的中心线 (并且形状的厚度在生成的 DXF 文件中不可见)。

使用 KiCad 字体绘制文本： 启用后，KiCad设计中的文本将被绘制成使用KiCad字体的图形。 禁用时，文本将作为 DXF 文本对象绘制，它将使用不同的字体，并且不会以与 KiCad 电路板编辑器中显示的完全相同的位置和大小显示。

导出单位： 控制将在 DXF 文件中使用的单位。 由于DXF格式没有指定的单位系统，你必须使用与你想在其他软件中使用的相同的单位设置来输出。

默认笔尺寸： 控制用于创建图形的绘图仪笔尺寸。

Output mode: Controls whether the generated PDF file is in color or black and white.

Generate property popups for front footprints: When enabled, interactive popups will be added to the generated PDF containing part information for each footprint on the front of the board.

Generate property popups for back footprints: When enabled, interactive popups will be added to the generated PDF containing part information for each footprint on the back of the board.

The Specctra DSN exporter creates a file suitable for importing into certain third-party autorouter software. This exporter has no configurable options.

The GenCAD exporter creates a GenCAD file for fabrication, testing, or importing into other software.

The GenCAD exporter has several options.

Flip bottom footprint padstacks: If enabled, separate flipped padstack definitions will be added for bottom-side footprints. This may be necessary for importing into some third-party software.

Generate unique pin names: If enabled, a suffix will be added to each pin name so that no footprint in the generated file will have two pins with the same name.

Generate a new shape for each footprint instance: If enabled, a unique footprint will be output for every footprint instance, even if two footprints are identical.

Use drill/place file origin as origin: If enabled, coordinates in the generated file will be relative to the drill/place file origin.

Save the origin coordinates in the file: If enabled, the selected origin coordinates will be included in the generated file. If not enabled, the origin in the generated file will be set to (0,0).

The VRML exporter creates a VRML (.wrl) 3D model file containing the PCB and any VRML files specified in footprints. VRML models are suitable for use in applications where visual appearance is important and dimensional accuracy is not critical.

The VRML exporter has several options.

Coordinate origin options: Selects the origin for the generated model. If user defined origin is selected, you can manually specify the origin point.

VRML units for output files: Selects the unit system for the generated model. Dimensions in the generated model will be scaled appropriately.

Copy 3D model files to 3D model path: If enabled, VRML files referenced in footprints will be copied into a subdirectory of the directory containing the generated board VRML model, and the generated model will reference the copied files. The subdirectory name is set by the footprint 3D model path field. If disabled, VRML files referenced in footprints will be embedded in the generated VRML files.

Use relative paths to model files in board VRML file: If enabled, references to external models will use paths relative to the generated board VRML file. If disabled, the references will use absolute paths. This option is only available when the copy 3D model files to 3D model path option is enabled.

IDF 导出器导出一个 IDFv3 兼容的板（.emn）和库（.emp）文件，用于向机械 CAD 软件传递机械尺寸。导出器导出板子的边框和切口，所有的焊盘和安装孔，包括开槽孔，以及元件的边框；这是与机械设计师互动所需的最基本的机械数据集。IDFv3 规范中描述的所有其他实体目前都没有导出。

一旦为所有需要的元件指定了模型，就可以导出电路板的模型。在 PCB 编辑器中，选择文件 → 导出 → IDFv3…​。

网格参考点： 选择导出的模型参考点的位置。如果选择了 自动调整 选项，KiCad 将把参考点设置为 PCB 的中心点。否则，参考点将相对于显示原点设置。

输出单位： 选择输出模型的单位是毫米还是mil。

输出结果可以直接在机械 CAD 应用程序中查看，或使用 idf2vrml 工具 转换为 VRML。

The STEP exporter creates a STEP (.step) 3D model file containing the PCB and any STEP files specified in footprints. STEP models are suitable for use in mechanical CAD applications.

The STEP exporter can also export a binary GLTF (.glb) model file by changing the output file’s format to Binary GLTF.

Coordinates: Selects the origin for the generated model. If user defined origin is selected, you can manually specify the origin point.

Ignore 'Do not populate' components: If enabled, components with the DNP attribute set will not be included in the exported STEP model.

Ignore 'Unspecified' components: If enabled, components with the Unspecified footprint type will not be included in the exported STEP model.

Substitute similarly named models: VRML models cannot be used for STEP exports, but if this option is enabled the exporter will look for an identically named STEP model to include in the export instead of a footprint’s specified VRML model. Note that footprints in KiCad’s footprint library specify VRML models, but suitably named STEP models are included for each VRML model. Therefore this option must be enabled in order to export STEP models for footprints from KiCad’s library.

Overwrite old file: If enabled, the exported STEP model will overwrite an existing file with the same name.

Optimize STEP file: If enabled, parametric curves will be disabled in the exported STEP model. This reduces the file size, but may reduce compatibility with some software.

Export tracks, pads and vias: If enabled, tracks, pads, and vias on outer layers will be modeled in the exported STEP model. This option may increase the export time.

Export zones: If enabled, zones on outer layers will be modeled in the exported STEP model. This option may increase the export time.

Board outline chaining tolerance: Controls the minimum distance between two points for the points to be considered coincident. If the board outline in the exported STEP model is not contiguous, try increasing this tolerance.

The SVG exporter creates a vector graphics image of the board.

Layers: The selected layers will be included in the generated SVG.

Print mode: Controls whether the generated SVG file is in color or black and white.

Color theme: Controls the color theme used for the generated SVG file. If the use current board theme option is selected, the theme that is selected in the board editor will be used.

SVG page size: Controls the size of the generated SVG drawing. If page with frame and title block is selected, the drawing will match the board’s sheet size and will include the drawing sheet and title block. If current page size is selected, the drawing will match the board’s sheet size but will not include the drawing sheet. If board area only is selected, the drawing will be just big enough to fit the board itself.

Print mirrored: When selected, layers will be horizontally mirrored.

Print one page per layer: When selected, a separate SVG file will be generated for each selected layer. If the print board edges on all pages option is selected, the Edge.Cuts layer will be included in all generated SVGs, even if it is not selected as a layer.

CMP files are used to sync footprint assignments and some other footprint fields between the PCB and the schematic. You can import CMP files into the schematic using the schematic editor’s File → Import → Footprint Assignments menu item. This provides a very limited form of back annotation. It is recommended to use the Update Schematic from PCB tool instead.

This exporter has no configurable options.

The Hyperlynx exporter creates a file suitable for importing into Mentor Graphics (Siemens) HyperLynx simulation and analysis software. This exporter has no configurable options.

当 PCB 编辑器（或任何其他使用封装的 KiCad 工具）第一次运行时，如果没有找到全局封装表文件 fp-lib-table，KiCad 将引导用户设置一个新的封装库表。该过程在 上文 中描述。

封装库只有在被添加到全局或工程专用的封装库表中时才能被使用。

通过点击 按钮并选择一个库或点击 按钮并输入库文件的路径来添加一个库。选定的库将被添加到当前打开的库表中（全局或工程专用）。可以通过选择所需的库条目并点击 按钮来删除库。

点击 和 按钮在库表中上下移动所选库。这并不影响在 "封装库浏览器"、"封装编辑器 "或 "添加封装工具 "中显示库的顺序。

通过取消选中第一列中的 活动 复选框，可以使库处于非活动状态。 非活动库仍在库表中，但不会出现在任何库浏览器中，也不会从磁盘加载，这样可以减少加载时间。

点击范围内的第一个库，然后 Shift 点击范围内的最后一个库，可以选择一系列库。

每个库必须有一个独特的昵称：在同一个表中不允许有重复的库昵称。然而，昵称可以在全局和工程库表中重复。工程表中的库比全局表中的同名库更有优先权。

库的昵称不一定要与库的文件名或路径有关。冒号字符 （:） 不能用于库昵称或封装名称，因为它被用作昵称和封装之间的分隔符。

每个库条目必须有一个有效的路径。路径可以定义为绝对的、相对的，或者通过 环境变量替换 来定义。

The appropriate library format must be selected in order for the library to be properly read. The supported formats are listed above. Only KiCad format libraries (.pretty folders containing .kicad_mod files) can be saved. Other footprint library formats are read-only and must be converted to KiCad format before you can modify them.

有一个可选的描述字段，用于添加库条目的描述。选项字段目前不使用，所以添加选项在加载库时不会有任何影响。

封装库表支持环境变量替换，允许你定义环境变量，其中包含库存储位置的自定义路径。环境变量替换是通过在封装库路径中使用 ${ENV_VAR_NAME} 的语法来支持的。

默认情况下，KiCad定义了几个环境变量，这些变量在 工程管理文档 中描述。 环境变量可以在 偏好 → 配置路径…​ 对话框中进行配置。

在封装库表中使用环境变量，可以在不破坏封装库表的情况下重新定位库，只要在库的位置改变时更新环境变量即可。

${KIPRJMOD} 是一个特殊的环境变量，总是展开为当前工程目录的绝对路径。${KIPRJMOD} 允许将库存储在工程文件夹中，而不必在项目库表中使用绝对路径。这使得移动项目位置而不破坏其项目库表成为可能。

Non-KiCad format libraries, including legacy libraries (.mod files), are read-only. They need to be converted to KiCad format (.kicad_mod files in a .pretty folder) before you can save changes to them.

Libraries in other formats can be converted to KiCad libraries by selecting them in the footprint library table and clicking the Migrate Libraries button. Multiple libraries can be selected and migrated at once by Ctrl-clicking or shift-clicking.

Libraries can also be converted one at a time by opening them in the Footprint Editor and saving them as a new library.

有关创建新的封装向导的更多信息，请参阅高级主题章节的脚本部分。

渲染引擎： 控制是否使用硬件加速图形或备用图形加速。

网格样式： 控制对齐网格的绘制方式。

网格粗细： 控制网格线或网格点的粗细。

最小网格间距： 控制两条网格线之间的最小距离 (以像素为单位)。无论当前的网格设置如何，如果网格线 违反这个最小间距，将不会被绘制。

捕捉到网格： 控制绘图和编辑操作何时会被捕捉到活动网格上的坐标。 总是 "将启用捕捉功能，即使网格被隐藏； "当网格显示时" 将只在网格可见时启用捕捉功能。

光标形状： 控制编辑光标是画成一个小十字线还是全屏十字线（一组覆盖整个画布的线条）。 编辑光标显示下一个绘图或编辑操作将发生的位置，如果启用了捕捉，则会捕捉到网格位置。

始终显示十字准线： 控制是始终显示编辑光标， 还是仅在编辑或绘图工具处于活动状态时才显示编辑光标。

网络名称： 控制是否在铜对象上绘制网络名称标签。 这些标签仅作为编辑指南，不会出现在制造输出中。

显示焊盘编号：控制是否在封装焊盘上绘制焊盘编号标签。

显示焊盘 <无网络> 指示器： 控制是否用特殊标记指示没有网络的焊盘。

布线间隙： 控制是否显示布线和过孔周围的间隙边界。 间隙边界显示为对象周围的细长形状，表示与其他对象之间的最小间隙， 如约束和设计规则所定义。

显示焊盘间隙： 控制是否显示焊盘周围的间隙边界。

交叉探测项目的中心视图： 当原理图和 PCB 编辑器同时运行时，控制在原理图中点击一个元件或引脚是否会将 PCB 编辑器的视图集中在相应的封装或焊盘上。

缩放以适合交叉探测对象： 控制是否缩放视图以显示交叉探测的 封装或焊盘。

高亮交叉探测网络： 控制当高亮工具在两个工具中激活时，原理图中高亮的网络是否会在 PCB 编辑器中高亮。

翻转电路板项目 L/R： 控制电路板对象在顶层和底层之间移动时的翻转方向。 选中时，项目从左向右翻转(垂直轴)； 取消选中时，项目从上向下翻转(水平轴)。

旋转命令的步长： 控制每次使用旋转命令时选定对象将旋转多远。

允许自由焊盘： 控制封装焊盘是否可以解锁并与封装分开编辑或移动。

吸附点： 这部分控制对象捕捉，也叫吸附点。 启用对象捕捉后，对象捕捉优先于网格捕捉。 对象捕捉只对活动层上的对象起作用。按住 Shift 可以暂时关闭对象捕捉功能。

捕捉焊盘： 控制编辑光标何时捕捉焊盘原点。

捕捉到布线： 控制编辑光标何时捕捉到布线端点。

对齐图形： 控制编辑光标何时对齐图形形状点。

始终显示选定的飞线：启用后，即使全局飞线被隐藏， 选定封装的飞线也将始终显示。

用曲线显示飞线：控制飞线是直线绘制还是曲线绘制。

鼠标拖动布线行为： 控制使用鼠标拖动布线线段时将发生的操作："移动" 将独立于任何其他布线线段移动布线。 "拖动(45 度模式)" 将调用推挤布线器拖动布线，遵守设计规则并保持其他布线段的连接。 "拖动(自由角度)" 将移动布线段最近的角点，高亮显示与其他对象的碰撞，但不会将其移开。

将操作限制在从起点开始的45度： 控制使用图形绘制工具绘制的布线是否可以采用任何角度。 请注意，这仅影响绘制新的布线：布线可以被编辑成任何角度。

显示页面限制： 控制页面边界是否绘制为矩形。

敷铜属性对话框关闭后重新敷铜： 控制编辑任何敷铜属性后是否自动重新敷铜。 可以在复杂的设计或速度较慢的计算机上禁用此功能，以提高响应速度。

KiCad supports switching between different color themes to match your preferences. Kicad 8.0 comes with two built-in color themes: "KiCad Default" is a new theme designed to have good contrast and balance for most cases and is the default for new installations. "KiCad Classic" is the default theme from KiCad 5.1 and earlier versions. Neither of these built-in themes can be modified, but you can create new themes to customize the look of KiCad as well as install themes made by other users.

颜色主题存储在位于 KiCad 配置目录的 Colors 子目录中的 JSON 文件中。“打开主题文件夹” 按钮将在您的系统文件管理器中打开此位置，使您可以轻松地管理已安装的主题。要安装新主题，请将其放在此文件夹中，然后重新启动 KiCad。如果文件是有效的颜色主题文件，则从颜色主题下拉列表中可以看到新主题。

要创建一个新的颜色主题，从颜色主题的下拉列表中选择 “新主题…​”。 为你的主题输入一个名称，然后开始编辑颜色。 新主题中的颜色将从你创建新主题之前选择的任何主题中复制。

要更改颜色，请双击或中键单击列表中的色样。“重置为默认值” 按钮会将该颜色重置为 “KiCad 默认” 颜色主题中的相应条目。

颜色主题会自动保存；当您关闭 "偏好设置" 对话框时，所有更改都会立即反映出来。对话框右侧的窗口显示所选主题外观的预览。

KiCad PCB 编辑器支持用 Python 编写的插件，对正在编辑的电路板进行操作。 这些插件可以使用内置的 “插件和内容管理器” 来安装（详见 KiCad 章节），或者将插件文件放在用户的插件目录中。 详见下面的脚本部分。

每个被检测到的插件都会在这个偏好设置上显示一排。 插件可以在 “PCB 编辑器” 的顶部工具栏上显示一个按钮。 如果一个插件的 "显示按钮" 控制没有被选中，它仍然可以从 "工具" > "外部插件" 菜单中访问。

列表底部的箭头控制允许改变插件在工具栏和菜单中的显示顺序。 文件夹按钮将启动一个文件资源管理器到插件文件夹，以使安装新的插件更容易。 刷新按钮将扫描插件文件夹中的任何新的或删除的插件，并更新列表。

显示原点： 决定在编辑画布中坐标显示使用哪个坐标原点。 页面原点固定在页面的角落。 用户可以移动钻孔/拾放文件原点和网格原点。

X 轴： 控制 X 坐标向右还是向左增加。

Y 轴： 控制 Y 坐标是向上还是向下增加。

自定义规则编辑器位于电路板设置对话框中，它提供了一个用于输入自定义规则的文本编辑器，一个语法检查器将测试你的自定义规则并指出任何错误，还有一个语法帮助对话框，其中包含了对自定义规则语言的快速参考和一些规则示例。

The custom rules editor also provides context-sensitive autocomplete to suggest valid keywords and properties. The autocomplete suggestion menu appears automatically, but it can also be opened manually by pressing Ctrl+Space.

在编辑自定义规则后，最好使用 检查规则语法 按钮，确保没有语法错误。 自定义规则中的任何错误将阻止设计规则检查器的运行。

The custom design rule language is based on s-expressions and allows you to create design constraints that are not possible with the built-in constraints. Each design rule generally contains a condition defining what objects to match and a constraint defining the rule to be applied to the matched objects.

该语言使用圆括号 (( 和 )) 来定义相关标记和值的子句。括号必须始终匹配：对于每个 ( 必须有匹配的 )。在子句中，标记和值之间用空格分隔。按照惯例，使用单个空格，但是可以在标记之间使用任意数量的空格字符。在文本字符串有效的地方，没有任何空格的字符串可以用 " 或 ' 引起来，也可以不加引号。包含空格的字符串必须始终用引号引起来。在需要嵌套引号的地方，可以使用 " 作为外引号字符，使用 ' 作为内引号字符 (反之亦然)，从而实现单层嵌套。换行符不是必需的，但为清楚起见，通常在示例中使用。

在下面的语法描述中，<三角括号> 中的项目代表必须存在的标记，[方括号] 中的项目代表可选的或只是有时需要的标记。

The Custom Rules file must start with a version header defining the version of the rules language. As of KiCad 8.0, the version is 1. The syntax of the version header is (version <number>). So in KiCad 8.0 the header should read:

在版本头之后，您可以输入任何数量的规则。 规则的评估顺序是相反的，也就是说，文件中的最后一条规则首先被检查。 一旦为一个给定的被测对象找到一个匹配的规则，将不再检查其他规则。在实践中，这意味着更具体的规则应该在文件的后面，以便它们在更通用的规则之前被评估。

例如，如果您创建一条规则来限制 HV 网络的布线与任何其他网络的布线之间的最小间距，然后又创建第二条规则来限制特定规则区域内所有对象的最小间距，请确保第一条规则在自定义规则文件中的出现时间比第二条规则晚，否则，如果 HV 网络中的布线落在规则区域内，可能会有错误的间距。

Each rule must have a name and one or more constraint clauses. The name can be any string and is used to refer to the rule in DRC reports. The constraint defines the behavior of the rule. Rules may also have a condition clause that determines which objects should have the rule applied, an optional layer clause which specifies which board layers the rule applies to, and an optional severity clause which specifies the severity of the resulting DRC violation.

The custom rules file may also include comments to describe rules. Comments are denoted by any line that begins with the # character (not including whitespace). You can press Ctrl+/ to comment or uncomment lines automatically.

可以在自定义规则表达式中测试以下属性：

PCB 编辑器带有一个内置的 Python 控制台，可以用来检查并与电路板互动。 要启动控制台，使用顶部工具栏中的 按钮。PCB 编辑器的 Python API 不会自动加载，所以要加载它，在控制台中输入 import pcbnew。然后 pcbnew.GetBoard() 命令将返回当前在 PCB 编辑器中加载的电路板的引用，可以通过控制台进行检查和修改。

Plugin scripts (PCB action plugins and footprint wizards) can be installed automatically using the Plugin and Content Manager (PCM), or manually by copying the plugin to a folder. Manually installed plugins should each be in their own folder within the plugins folder. The location of the plugins folder is by default:

The scripting API reflects the internal object structure inside KiCad’s Board Editor. It is provided by the pcbnew module in Python.

Scripts, action plugins, and interactive scripting sessions often start with a call to GetBoard(), which returns a BOARD object representing the currently open board and its contents.

BOARD has a set of properties and a set for each type of object in the board: footprints, zones, tracks, vias, text, etc. Each type of object has its own properties and holds its own objects: a footprint will likely have at least one pad, for example.

The objects in the BOARD can be accessed using methods that each return an iterable list of the corresponding object type. A selection of these methods are listed below. Other methods are listed in the doxygen documentation.

Boards can be loaded and saved from disk using the following functions:

Action plugin associate a script with a button in the PCB Editor GUI. Clicking the button runs the script. Action plugins are shown in the Tools → External plugins menu, and can also be shown in the toolbar if enabled in the Action Plugins page of the Preferences dialog.

The example below is an action plugin that uses KiCad’s pcbnew API to replace the string $date$ with the current date in any text item.

Footprint wizards are Python scripts that can be accessed from the Footprint Editor. Each footprint wizard presents a selection of parameters defined in the Python script, and creates a footprint based on the parameter values.

There are 3 minimum steps required to create a footprint wizard, which are described below. For examples of how to create footprint wizards, see the footprint wizards included with KiCad.

The GetName(), GetDescription(), and GetValue() functions are there to provide strings to the UI. The only functionality needed is to return an appropriate string.

The GenerateParameterList() function defines the parameters needed for the footprint. Parameters are grouped into a page + name format. For example, calling self.AddParam("demo", "radius", self.uMM, 5) would add a parameter named radius into the page named demo. Retrieving that parameter data would be done with a call such as self.footprint_radius = self.parameters["demo"]["radius"].

The CheckParameters() function is available to perform any data validation on the parameters defined in GenerateParameterList(). This function is also where the self.footprint_radius = self.parameters["demo"]["radius"] calls reside.

The BuildThisFootprint() function is where the footprint building steps are called. This function is where one creates the footprint.

The required {your_class_name}().register() call can either be at the end of the Python file, or in an __init__.py file. Both styles are supported by KiCad.

IDF 元件模型使用 [封装属性，封装的 3D 模型属性] 附加到封装上。IDF 导出器使用的文件类型与 3D 查看器和其他 3D 模型导出器不同，因此为 IDF 导出器添加 3D 模型不会与为其他目的添加到封装的 3D 模型发生冲突。

要在封装或 PCB 编辑器中把 IDF 模型添加到封装中，编辑封装的属性并点击 3D 模型标签。

点击 按钮，选择 IDF(*.idf;*.IDF) 文件类型筛选器。浏览到所需的边框文件。

一旦选择了所需的元件边框文件，输入任何必要的偏移和旋转值。偏移量必须使用 IDF 板的输出单位（毫米或mil）并在 IDF 坐标系中指定，这是一个右手坐标系，+Z 指向观察者，+X 指向观察者的右边，+Y 指向屏幕的上边缘。旋转必须以度为单位；正向旋转是逆时针旋转，如 IDF v3 规范中所述。

多个边框可以与适当的偏移量结合起来，以表示简单的装配，如插座中的 DIP 封装。

元件边框文件（*.idf）包括一个单一的 .ELECTRICAL 或 .MECHANICAL 部分，如规范文件中所述。该部分前面可以有任何数量的注释行；注释行由导出器复制到库文件中，可以用来跟踪元数据，如用于确定元件边框和尺寸的文件的参考。

元件边框部分包含字符串，整数或浮点数字段。 字符串是可包含空格的字符组合; 如果字符串包含空格，则必须引用它。 引号不得出现在字符串中。 浮点数可以使用十进制或指数表示法表示，但十进制表示法是人类可读性的首选。 小数点必须是点而不是逗号。 IDF 文件必须只包含7位 ASCII 字符; 使用8位字符将导致未定义的行为。

IDF 文件由 SECTIONS 组成，SECTIONS 由 RECORDS(记录) 组成，RECORDS 由 FIELDS(字段) 组成。对于 IDF 边框文件，只有一种类型的部分可以存在，并且必须是 .ELECTRICAL 或 .MECHANICAL 中的一种。一个记录是一行文本，可能包含一个或多个字段。字段是由一个或多个空格分隔的字符序列，不在引号之间出现。一条记录的所有字段必须出现在单行上；记录不能跨行。

Section的标题（.ELECTRICAL 或 .MECHANICAL）被认为是该节的第一条记录（记录 1）。记录 1 后面必须有记录 2，该记录有四个字段：

记录 2 后面必须跟有许多记录 3 条目，这些条目指定了元件的边框。 记录 3 包含四个字段：

只允许一个闭环，并且无法指定切口。 指定的最后一个点必须与第一个点相同，除非边框是圆形。

示例 IDF 文件 1：

示例 IDF 文件 2：

在创建边框时，特别是在与他人共享工作时，文件的设计和命名的一致性可以帮助人们更快地找到文件并以最小的麻烦放置元件。

许多命令行工具可用于帮助生成 IDF 元件边框。 工具是：