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。