Three New Importers in KiCad 10: Allegro, PADS, and GEDA

PADS schematics import with symbols, wire segments, junction dots, net labels, and connectivity. Multi-unit symbols from multi-gate part types are reconstructed, and power and ground symbols map to their KiCad standard library equivalents. Hierarchical multi-sheet structures are preserved, and title block information is pulled from the FIELDS section.

Pin types translate directly: passive, input, output, bidirectional, tristate, open collector, open emitter, and power. Text annotations keep their height, width, justification, and rotation. Graphic primitives (lines, rectangles, circles, arcs) retain their fill and line styles.

Footprints import with reference designators, values, positions, rotation, and layer placement. Pad shapes include circles, rectangles, ovals, rounded rectangles, and thermals. Drill definitions cover plated and non-plated holes, slotted holes, and per-layer dimensions.

Tracks, arcs, and all via types (through-hole, blind, buried, and microvias) import with width and net assignments. Copper zones keep their priority ordering, thermal relief settings, and net assignment. Keepout areas for routing, vias, copper, and component placement are handled.

Board outlines (with arc support), text annotations, dimension lines, graphic elements, test point definitions, and reuse blocks are all imported. Reuse blocks become KiCad groups. Design rules for clearances, track widths, via sizes, hole spacing, and mask expansions are extracted and applied to the board settings. Differential pairs are converted to DRC rules in the .kicad_dru file.

Component graphics are reconstructed from .sym symbol files, including lines, boxes, circles, arcs, and paths. Pin types (input, output, bidirectional, open collector, open emitter, passive, tristate, power, no-connect) map to KiCad equivalents. Net wires import with automatic junction placement at three-way and greater intersections, and bus segments generate proper bus entries.

Hierarchical sub-schematics work through the source= attribute, with recursive loading and loop detection. Multi-slot components are reconstructed using the numslots, slot, and slotdef attributes. Power symbols are identified from the net= attribute, and gEDA’s overbar notation (_text\_) converts to KiCad’s ~{text} format. A built-in symbol library provides fallback symbols for common parts like resistors, capacitors, diodes, transistors, logic gates, and op-amps when the original .sym files are not available.

Footprints import with through-hole pins (circle or square shapes) and surface-mount pads (rectangle, oval, circle) on front or back layers. Pad clearance and solder mask margins are converted. Copper traces, arcs, and polygons import on all layers, along with through-hole vias. Net connectivity is reconstructed from the NetList block, and the importer handles multi-layer copper configurations up to 16 layers.

The gEDA importer can also browse footprint libraries directly. Individual .fp files from directory-based libraries load with pin and pad definitions, shape and clearance parameters, and silkscreen graphics.