The main toolbar is at the top of the main window. It has buttons for the undo/redo commands, zoom commands, footprint/pad properties dialogs, and layer/grid management controls.

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

Placement and drawing tools are located in the right toolbar.

The footprint name, description, and keywords describe the footprint itself. Together they are intended to describe the footprint and help you select an appropriate footprint for each component. They are also used when searching for footprints in the Footprint Editor and the Add Footprint dialog.

The footprint name contains the name of the footprint. This is the same as the footprint’s filename on disk, and is also initially the same as the footprint’s Value field. However, the Value field can be edited in the footprint editor, and when a footprint is added to a board, its Value field will be updated with the value of the footprint’s corresponding symbol.

The description is a description of the footprint. It should be human readable, but it is also used when searching for a footprint.

The keywords are space-separated words related to the footprint. They are used when searching for a footprint.

Footprints contain multiple fields, which are named values containing information related to the footprint. Fields can be visible and shown on any board layer, or they can be hidden and only shown in the footprint’s properties. Some fields have special meaning to KiCad: Reference and Footprint are both both used by KiCad to identify schematic symbols and PCB footprints, for example. Other fields may contain information that is important for a design but is not interpreted by KiCad, like pricing or stock information for a part.

Any fields defined in a library footprint will be included in the footprint when it is added to a board. You can also add new fields to footprints in the board. Whether they are in the library footprint or not, these fields can then be edited on a per-footprint basis in the board. Symbol fields are also transferred to the board and added as fields in the corresponding footprint.

All library footprints are defined with five default fields which correspond to the five default fields in library symbols: Reference, Value, Footprint, Datasheet, and Description. These default fields cannot be deleted. The Reference field initially has the value REF**, while the Footprint and Value fields are initially set to the name of the footprint. In the board, the values of the five default fields will be set to the values of the matching fields in the footprint’s corresponding symbol.

Fields each have an associated layer, which determines which board layer the field will be placed on. Fields can also be visible or hidden.

To edit an existing footprint field, double-click the field, select it or hover and press E, or right-click on the field text and select Properties…​.

To add new fields, delete optional fields, or edit existing fields, use the icon on the main tool bar to open the Footprint Properties dialog. Fields can be arbitrarily named, but names starting with ki_, e.g. ki_description, are reserved by KiCad and should not be used for user fields.

Fields have a number of properties, each of which is shown as a column in the properties grid. Not all columns are shown by default; columns can be shown or hidden by right clicking on the grid header and selecting or deselecting columns from the menu.

Footprints have several attributes, which are properties of the footprint that affect how it is handled by other parts of KiCad.

Every footprint has a component type: SMD, Through hole, or Unspecified. A footprint’s type affects KiCad’s behavior in a few ways:

If not in schematic is checked, KiCad will not expect the footprint to correspond to a symbol in the schematic. When updating a PCB from the schematic, KiCad will ordinarily remove footprints that don’t have corresponding symbols according to the delete footprints with no symbols setting. However, such footprints will not be deleted when they have not in schematic set.

If exclude from POS files is checked, KiCad will not include the footprint in component placement file exports.

If exclude from bill of materials is checked, the component will not be included in bill of materials exports in either the schematic or PCB editors. This attribute is synced to and from the footprint’s corresponding schematic symbol.

If exempt from courtyard requirement is checked, the footprint will not trigger a DRC violation if it does not contain a courtyard. Without this attribute set, a footprint without graphics on the F.Courtyard or B.Courtyard layer will cause a "Footprint has no courtyard defined" DRC violation.

The do not populate attribute is primarily a schematic symbol attribute, and is synced to and from the footprint’s corresponding schematic symbol. Footprints with this attribute set can optionally be excluded from component placement file exports and some other types of outputs. These footprints can also be hidden in the 3D viewer.

Footprints can have private footprint layers, which are layers that can be viewed and edited in the Footprint Editor but are not shown in the footprint when it is added to a board. Therefore any objects that are on private layers will not be visible in the PCB Editor or included in PCB fabrication outputs. This may be useful, for example, for notes or graphics that are of interest when drawing or editing a footprint but not needed at the board level.

Any of the existing User.* layers (User.Drawings, User.Comments, User.Eco1, User.1, etc.) can optionally be a private layer. To make a layer private, add a private layer in the General tab of the footprint properties dialog, then select the desired layer. Any objects on that layer will not be shown on the board.

The Clearance Overrides and Settings tab holds settings for footprint-specific overrides to board clearance and mask/paste expansion, pad-to-zone connections, and net tie settings for allowing pads within the footprint to short different nets.

Pad clearance controls the minimum clearance between the footprint’s pads 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 the board’s design rules and netclass rules. This value can be overridden for individual pads by setting the pad’s clearance to a nonzero value.

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 here. These values can be overridden for individual pads by setting the pad’s expansion or clearance to a nonzero value.

Solder mask expansion 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 expansion 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.

Pad connection to zones controls whether the footprint’s pads will have solid, thermal relief, or no connection to zones. 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 zone setting, which uses the connection mode specified in the connection zones' properties. This setting can be overridden for individual pads by setting the pad’s connection mode to a value other than From parent footprint.

The 3D Models tab allows you to attach external 3D model files to a footprint and view the footprint in three dimensions along with any attached models.

The main part of the window is a 3D preview of the footprint and any attached models. The buttons to the right of the preview let you enable or disable an orthographic projection (), show or hide the PCB model (), align the view to one of the six face-aligned perspectives (), and refresh the view (). The bottom button () lets you set the thickness of the PCB in the preview.

The top of the dialog lets you attach external models. Each added model will be shown in the footprint preview as well as in the full PCB 3D view when the footprint is added to a board. Footprint models can be in STEP, VRML, or IDF format. The models are specified as paths to the model files, which can contain path variables such as ${KIPRJMOD} or ${KICAD8_3DMODEL_DIR}. Click the Configure Paths button to configure path variables. If there is a problem loading a model file from the specified path, an icon in the leftmost column will indicate an error.

By default, models are added with their origin placed at the footprint’s origin, with no offset, scaling, or rotation. Offset, scaling, and rotation can be applied to a model using the controls to the left of the preview canvas. The model’s opacity can be adjusted using the opacity slider, and the model can be completely hidden by deselecting the show checkbox in the rightmost column of the model table.

You can edit a pad after adding it by opening the pad’s properties dialog (E). These properties are also editable using the properties manager.

When you place a new pad, the new pad’s properties are copied from the default pad properties. Each time any pad is edited, the pad’s updated properties are stored as the default pad properties, so that new pads will match the properties of the most recently edited pad.

You can directly edit the default pad properties by selecting Edit → Default Pad Properties…​, or choose an existing pad to represent the default by right clicking the pad and choosing Copy Pad Properties to Default. New pads will use that pad’s properties as their defaults until a new default is selected, either by editing another pad, editing the default pad properties, or manually copying a different pad’s properties to the default.

There are several ways to update existing pads with the properties of other pads. You can apply the default pad properties to an explicit selection of pads by selecting the desired target pads, right clicking, and choosing Paste Default Pad Properties to Selected from the right click context menu. You can also update other pads with a selected pad’s properties using Push Default Pad Properties to Other Pads…​, also in the right click context menu.

This tool has several options to filter which pads are targeted.

If do not modify pads having a different shape is selected, only pads with the exact same shape properties as the selected pad will be updated.

If do not modify pads having different layers is selected, only pads on the same layer(s) as the selected pad will be updated.

If do not modify pads having a different orientation is selected, only pads with the same orientation as the selected pad will be updated.

If do not modify pads pads having a different type is selected, only pads with the same pad type as the selected pad will be updated.

If no options are selected, all pads in the footprint will be updated.

You can create an array of pads from a source pad by right clicking the source pad and selecting Create from Selection → Create Array…​ (Ctrl+T). The basic functionality of this tool is described in the PCB Editor documentation. For pads, however, there are additional options for controlling pad numbering.

For grid arrays, you can select a numbering direction, either horizontal, then vertical or vertical, then horizontal. If reverse numbering on alternate rows/columns is selected, the direction of increasing pad numbers will alternate from one row/column to the next.

The initial pad number in the array can either be the first unused pad number in the footprint (use first free number) or the specified pad numbering start value. After the first number, the pad numbering can either be continuous (1, 2, 3, …​) or coordinate based, in other words, dependent on both the row and column (A1, A2, …​, B1, …​). In addition to the initial pad number (pad numbering start), you can specify a numbering step (pad numbering skip). For coordinate-based numbering, you can configure separate starting numbers and steps for each axis. You can select whether pad numbers use decimal digits (0-9), hexadecimal digits (0-F), the full alphabet, or the alphabet excepting certain ambiguous letters (I, O, S, Q, X, and Z).

Finally, you can quickly renumber existing pads using the Renumber Pads tool (Edit → Renumber Pads…​).

The tool has several options. Pads will be renumbered starting at the selected first pad number, and each subsequent pad will have its number incremented by the numbering step. You can also choose an optional pad name prefix which will be inserted before of the incrementing part of each pad number.

Once you click OK, you will be prompted to click on a pad, which will be assigned a new pad number based on the selected initial pad number and prefix. You can keep clicking on pads to assign them the next number in the sequence based on the selected numbering step. Double click on a pad to renumber that pad and end the sequence, or press Esc to discard the changes.

For some footprints, the built-in pad shapes (round, rectangular, etc.) may not be sufficient. In these cases you can construct custom pads with arbitrary shapes using Pad Edit Mode. This mode lets you combine a basic pad with graphic shapes to build a new pad out of the compound shape.

To build a custom pad, first add a regular pad using the pad tool ( button). This base pad will become the custom pad’s anchor or snapping point, so be sure to place the pad in the exact location where you want tracks to attach to the pad. The shape and size of the pad do not matter, but the hole, if any, will remain in the final custom pad. In other words, a surface mount base pad will result in a surface mount custom pad, and a through hole base pad will result in a through hole custom pad. The custom pad’s number will be inherited from the base pad.

Next, enter Pad Edit Mode by selecting the base pad, right-clicking, and selecting Edit Pad as Graphic Shapes (Ctrl+E). Add graphic shapes as appropriate to create the desired pad shape. Shapes touching the base pad will be unioned together with the base pad to create the final pad shape.

You can exit Pad Edit Mode by right-clicking and selecting Finish Pad Edit, or pressing Ctrl+E again. When you exit pad edit mode, all shapes that touch the base pad will be combined with the pad. For example, when editing a surface mount pad on F.Cu, any shapes that are on F.Cu and touch the base pad will become part of the custom pad. Any shapes that do not overlap the base pad, or that are on a different layer, will remain separate. If the base pad is a through hole pad, overlapping shapes on F.Cu will be combined in the custom pad. Because through hole pads have the same pad shape on all copper layers, this shape will become part of the custom pad on all copper layers, not just F.Cu. For convenience, Pad Edit Mode dims the color of other pads and all shapes that are not contiguous with the base pad so that you can see which shapes will be included in the custom pad and which will not.

Custom pads can only contain a single base pad. Any additional pads that touch the base pad or the contiguous graphics, whether they have the same or different pad numbers as the base pad, will remain separate pads after the shapes are combined into the custom pad.

To modify an existing custom pad, select it and enter Pad Edit Mode again. You can then continue to edit the component shapes to adjust the pad shape, or change the position of the base pad to adjust the pad anchor.

KiCad automatically chooses a size and location for showing the pad number over the pad. Particularly for unusually shaped pads, the automatically determined size and location may not be optimal. In these cases, you can manually specify a region in which KiCad should draw the pad number by adding a pad number box primitive. To add a number box, enter Pad Edit Mode and add a rectangular shape. In the properties manager for the rectangle, check the Number Box checkbox. The rectangle will then be shown as a wireframe, and when you exit Pad Edit Mode it will be used to draw the pad number.

In the board, KiCad will automatically add thermal spokes when connecting the pad to a zone. The thermal spoke settings are determined by the pad, footprint, and zone settings, and the thermal spokes by default connect to the pad anchor. You can override the default thermal spoke placement by adding thermal relief templates to the custom pad. To add a thermal relief template, enter Pad Edit Mode and add a line shape. In the properties manager for the line, check the Thermal Relief Template checkbox. In Pad Edit Mode, the line will then be shown as a wireframe, and it will not be shown outside of pad edit mode. If any thermal relief templates are present in the pad, KiCad will not automatically add additional spokes when filling zones; spokes will only be placed where there are thermal relief templates defined in the pad. Thermal relief templates only determine the spoke location: spoke width and relief gap are still defined in the pad, footprint, and/or zone properties, as normal.

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

This dialog is described in more detail in the PCB Editor documentation.

There is a dedicated tool for performing common cleanup operations on graphics, which is run via Tools → Cleanup Graphics…​.

The following cleanup actions are available and will be performed when selected:

Merge lines into rectangles: combines individual graphic lines that together form a rectangle into a single rectangle shape object.

Delete redundant graphics: deletes graphics objects that are duplicated or degenerate.

Merge overlapping graphics into pads: merges graphic copper shapes that overlap pads into a custom pad.

Any changes that will be applied to the footprint are displayed at the bottom of the dialog. They are not applied until you press the Update Footprint button.