Display and selection controls

Board layers

Layers in Pcbnew represent physical copper layers on a board, as well as graphical layers used for defining things such as silkscreen, solder mask, and the board edge. There is always one layer that is active in the editor. The active layer is drawn on top of other layers and will be the layer assigned to newly-created objects. The active layer is indicated in the layer selector drop-down box in the top toolbar and is also highlighted in the appearance panel. To change the active layer, you can left-click a layer name in the appearance panel, use the drop-down layer selector in the top toolbar, or use a hotkey. Layers can be hidden to simplify the board view. You can hide a layer even if it is the active layer.

Display order for board layers

The appearance panel

The appearance panel provides controls to manage the visibility, color, and opacity of objects in the Pcbnew drawing canvas. It has three tabs: the Layers tab contains controls for the board layers, the Objects tab contains controls for different types of graphical objects, and the Nets tab contains controls for the appearance of the ratsnest and copper items.

Layer controls

In the Layers tab of the appearance panel, each board layer is shown with its color and visibility state. The active layer is shown highlighted with an arrow indicator to the left of the color swatch. Left-click on a layer to choose it as the active layer. Left-click on the corresponding visibility icon to toggle the layer between visible and hidden. Double-click or middle-click on the color swatch to change the layer’s color.

Below the list of layers is an expandable panel that contains layer display options. The first setting controls how non-active layers are displayed: normal, dimmed, or hidden. The layer display mode can be used to simplify the view and focus on a single layer. Items on inactive layers cannot be selected when the non-active layer display mode is “Dim” or “Hide”. You can use the hotkey Ctrl+H to cycle through these display modes quickly.

Flip board view will show the board as if you are looking from the bottom (that is, mirrored around the Y-axis). This option is also available in the View menu.

Object controls

The Objects tab of the appearance panel is similar to the Layers tab. The main differences are that some objects have no color setting and that four types of objects (tracks, vias, pads, and zones) have opacity control sliders. The opacity setting here will be multiplied with any opacity set in the layer colors. By default, all objects are fully opaque except for zones, which are set to translucent in order to make it easier to see objects through filled zone areas.

Layer presets

Layer presets store which layers and objects are visible and hidden for easy recall. There are several built-in layer presets and you can save your own custom presets. Custom presets are stored in the project settings for a board, as presets may be specific to a certain board stackup.

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

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.

Net and net class controls

The Nets tab of the appearance panel shows a list of all nets and net classes in the board. Each net has a visibility control that controls the visibility of that net in the ratsnest. Hiding nets in the ratsnest does not change the connectivity of the board and will not impact the design rule checker; it only is intended to make the ratsnest easier to understand.

Each net and net class can also have a color assigned. By default, this color applies to the ratsnest lines for the net (or for all the nets in the net class). Nets have no color by default; this is indicated by a checkerboard pattern in the color swatch. Double-click or right-click a net or net class color swatch to set the color.

You can also select and highlight nets and net classes via the appearance panel: right-click on a net or net class to show these options in a menu.

Below the list of net classes is an expandable panel that contains net display options. The first option controls how net colors are applied. When “All” is selected, all copper items (pads, tracks, vias, and zones) belonging to a net or net class will take on the chosen color. When “Ratsnest” is selected (the default value), only the ratsnest is affected by net and net class colors. When “None” is selected, net and net class colors are ignored.

The second option controls how ratsnest lines are drawn. “All layers” means that ratsnest lines will be drawn between all unconnected items. “Visible layers” means that no ratsnest lines will be drawn to items that are on hidden layers, even when those items are unconnected.

Selection and the selection filter

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 and a right-to-left selection box is drawn in blue.

The selection action can be modified by holding modifier keys while clicking or dragging. The following modifier keys apply when clicking to select single items:

The following modifier keys apply when dragging to perform a box selection:

The selection filter panel in the lower right corner of the Pcbnew window controls which types of objects can be selected with the mouse. Turning off selection of unwanted object types makes it easier to select items in a dense board. The “All items” checkbox is a shortcut to turn the other items on and off. The “Locked items” checkbox is independent of the rest, and controls whether or not items that have been locked can be selected. You can right-click any object type in the selection filter to quickly change the filter to only allow selecting that type of object.

When a connected copper item is selected, you can expand the selection to other copper items of the same net using the Expand Selection command in the right-click context menu or with the hotkey U. The first time you run this command, the selection will be expanded to the nearest pad. The second time, the selection will be expanded to all connected items on all layers.

Pressing Esc will always cancel the current tool or operation and return to the selection tool. Pressing Esc while the selection tool is active will clear the current selection.

Net highlighting

An electrical net (or set of nets) can be highlighted in the PCB editor to visualize how the net is routed across the PCB. Net highlighting can be activated by selecting the net to highlight in the PCB editor or by selecting the corresponding net in the schematic editor when cross-probe highlighting is enabled (see below). When net highlighting is active, the highlighted net or nets will be shown in a brighter color and all other items will be shown in a dimmer color than normal.

There are three ways to select a net or nets to highlight in the PCB editor: by using the hotkey ` after selecting a copper object, by using the context menu of any copper object, and the context menu of the Nets tab of the Appearance panel. When you press the Highlight Net hotkey, the nets of any selected copper items will be highlighted. If no copper items are selected, the net of the copper item under the editor cursor will be highlighted. If there is no copper item under the cursor, any existing highlighting will be cleared. The highlighting can also be cleared by using the Clear Highlight action (hotkey ~).

When a net or nets have been selected for highlighting, the Toggle Net Highlighting action becomes enabled on the left toolbar (also accessible by hotkey, Ctrl+`). This action will turn the highlighting display on or off without choosing a new net to highlight.

Cross-probing from the schematic

KiCad allows bi-directional cross-probing between the schematic and the PCB. There are several different types of cross-probing.

Selection cross-probing allows you to select a symbol or pin in the schematic to select the corresponding footprint or pad in the PCB (if one exists) and vice-versa. By default, cross-probing will result in the display centering on the cross-probed item and zooming to fit. This behavior can be disabled in the Display Options section of the Preferences dialog.

Highlight cross-probing allows you to highlight a net in the schematic and PCB at the same time. If the option “Highlight cross-probed nets” is enabled in the Display Options section of the Preferences dialog, highlighting a net or bus in the schematic editor will cause the corresponding net or nets to be highlighted in the PCB editor.

Left toolbar display controls

The left toolbar provides options to change the display of items in Pcbnew.