PCB layout

Footprints and Placement

3 min read Updated Markdown
On this page

Footprints are the physical packages placed on the PCB — pads, drill holes, silkscreen graphics, and optional 3D models. This page covers how footprints reach the board, and how to move, rotate, flip, and remove them.


Where Footprints Come From#

Every footprint on a board belongs to a component of the project's schematic. The footprint itself is the one assigned to that symbol (see Symbols Library).

Data Description
Pads Number, position, shape, drill size, layers
Graphics Silkscreen, fabrication, and courtyard outlines; reference and value text
3D model Optional STEP or other 3D file with offset, scale, and rotation

Footprint sources are managed in View → Local Library Manager — KiCad footprint folders, single .kicad_mod files, and converted Altium libraries. Load Footprints... at the top of the PCB Footprints panel adds one .kicad_mod file to the library.

Free KiCad footprint libraries

The official KiCad libraries at https://www.kicad.org/libraries/ can be added as a footprint source.


Placing Footprints#

From the schematic (the normal way)#

With a schematic of the project active, run Tools → Update Schematic to PCB (choose the target board when the project has several PCBs). WireFrame then:

  1. collects every sheet of the design, starting from the top sheet;
  2. loads each component's footprint, assigning one from the library symbol when the field is empty, and lists components whose footprint cannot be found;
  3. keeps footprints that are already on the board — position, rotation, and side — when their footprint did not change;
  4. removes footprints whose component no longer exists in the schematic;
  5. places new footprints in a grid, 200 mil apart, starting at the board origin;
  6. updates the nets and saves the PCB.

Drag the new footprints from the grid to their places on the board. A project is required: a standalone schematic cannot be converted.

Placing an unplaced footprint again#

The Footprints panel (right side, with a PCB active) lists footprints that belong to the design but are not on the board — for example ones you removed with Del. It reads All components placed. when there are none.

  1. Type in Filter... to find the footprint.
  2. Drag its row onto the canvas. It lands at the drop point, at 0°, on the top side.

Moving, Rotating, and Flipping#

Action How
Select Click a footprint; drag a box over several
Move Drag the selection, or nudge with the arrow keys (5 mil per press)
Rotate Space — by the step set in Preferences → Editing (90° by default)
Flip to the other side F, or Flip Layer (F) in Properties
Exact position Properties → Footprint Properties → Transform: X, Y, Rotation

Connected traces and vias keep their endpoints on the pads while you move or rotate. All of these are undoable (Ctrl+Z).

Flipping (Front ↔ Back)#

Flipping moves a footprint to the opposite side of the board. Its copper and silkscreen move to the back-layer set (F.Cu → B.Cu, F.SilkS → B.SilkS, and so on), and the footprint is mirrored as seen from the top. Properties shows (Current: Top) or (Current: Bottom).

Visual feedback

Flipped footprints change color (e.g. red F.Cu → blue B.Cu) and the designator mirrors — this matches the physical reality of a bottom-side component.


Footprint Properties#

Select one footprint to see Footprint Properties:

Field Description
Reference Designator, e.g. R1
Value Value text, e.g. 10k
Library The footprint it was built from (read-only)
Transform X, Y (mil, with mm beside), Rotation
Flip Layer (F) Moves it to the other side

Adjusting Designator Text#

Each footprint has a designator label (e.g. "R1", "U3") that can be moved on its own:

Action How
Select only the text Click directly on the designator
Move Drag it
Rotate Space with the designator selected
Align several Select the designators, right-click → Align Designators ▸ (Align Left, Align Right, Align Center (H), Align Top, Align Bottom, Align Center (V)), or Shift+Y / Shift+X

Use this when the designator overlaps a trace or pad.


Removing a Footprint#

Select a footprint and press Del. The footprint leaves the board and goes back to the Footprints panel, so you can drag it in again. Its traces stay where they are. Removing it is undoable.

To remove a component from the design for good, delete it in the schematic and run Update Schematic to PCB again.


See Also#