Footprint editor · SoftForge Electronics Designer

.kicad_mod files open in the footprint editor (or use Edit footprint in the Libraries tab, Electronics Designer: New footprint…, or Ctrl+E on a board to edit the selected footprint in place). It shares undo/redo, save, revert and hot exit with the other editors and writes with a minimal diff: footprints you do not touch stay byte-identical.

Library tab (left): the footprints of the .pretty folder with a search box; a click opens one. New, Wizard, Duplicate, Rename and Delete act on the folder.
Footprint tab (right): with a pad selected, every pad field (number, type, shape, position, angle, size, corner and chamfer ratios, trapezoid delta, hole and slot, layers, clearance / mask / paste overrides, zone connection and thermal reliefs, pin function and type, die length and delay, fabrication property, custom shape anchor and primitives); with a graphic or text selected its layer, width, style, points or text settings; with a text box selected its text (several lines), position, size, angle, layer, font (size, thickness, bold, italic, mirrored), horizontal and vertical justification, border (on / off, width, line style), the four margins (empty for KiCad’s default) and knockout. Below: description, keywords, fields, attributes (SMD / through-hole, not in schematic, exclude from position files and BOM, DNP, courtyard exemption), private layers, clearance overrides, net tie groups and the 3D models (path with a found / not-found check, offset, scale, rotation, opacity) with a 3D preview of the footprint and its models.
Private layers (Footprint tab): tick the user layers (Dwgs.User, Cmts.User, Eco1/Eco2.User, User.1 …) whose graphics belong to this footprint only, KiCad’s (private_layers …); the count of graphics on each private layer is shown next to it.
Pad array (Footprint tab or tool bar): a grid (columns, rows, pitch, stagger, numbering along rows or columns, snake) or a circle (count, centre, angle, rotated pads) of copies of the selected pad, numbered 1 2 3, A B C or BGA style (A1 … AA1, skipping I O Q S X Z). The dialog previews the pads it will create, with their numbers, over the footprint’s other pads (the template outlined) and warns when a number is already used.
Footprint wizard: SOIC / SOP, QFP, QFN (exposed pad, thermal vias), BGA, DIP, SIP, chip resistors and capacitors 0402 to 2512, through-hole two-pin parts, pin headers and mounting holes, with IPC-7351 courtyards and KiCad’s library names and 3D model paths; create a new footprint or replace the one on screen.
Tools: Add Pad, Renumber Pads (click pads in order), lines, rectangles, circles, arcs, polygons, Bézier curves, text and text boxes; move, rotate, flip, duplicate and delete as on the board.
Board footprints opened with Ctrl+E save back into the board as one undoable edit of the board (position, nets and fields kept, and the uuids of the footprint’s pads, graphics, texts and fields too, so groups, DRC exclusions and comments that refer to them still do; new objects get new uuids); Electronics Designer: Save footprint to another library… and Electronics Designer: Import footprint from board into a library… copy them into a .pretty.