KiCad 10 introduces new importers for Cadence Allegro, Mentor PADS, and gEDA/Lepton EDA. These tools make it possible to migrate existing schematic and PCB projects into KiCad while preserving important design data and allowing the projects to continue evolving in an open design environment.
Proprietary file formats can create vendor lock-in. Years of design work may become tied to formats that only specific tools can read, making it difficult to move to another EDA platform. The new KiCad 10 importers are intended to reduce that barrier by converting existing design data into KiCad projects that users can continue to edit and maintain.
Cadence Allegro Importer
The Allegro importer supports reading .brd files from Allegro versions 16 through 23. Schematic import is not currently supported.
Kicad Allegro uses a proprietary binary format whose documentation has not been publicly disclosed. The importer was developed through binary-structure reverse engineering and does not call any Allegro program or library. Hundreds of sample files were analyzed to identify patterns in the binary data and map them to documented Allegro functions and Gerber output.
This form of "blind" reverse engineering required the importer to handle linked-list block layouts, hash tables, and fields controlled by version-specific conditions across seven major Allegro releases.
After import, footprints retain their reference designators, values, positions, rotation angles, and layer assignments. Supported pad shapes include circles, squares, rectangles, obrounds, rounded rectangles, chamfered rectangles, octagons, and custom polygons. Drill diameters and thermal-relief parameters are also preserved.
Traces, arcs, and vias retain their widths and net assignments. Copper zones are reconstructed from their boundary shapes, while independent copper polygons can be imported directly. For boards created with Allegro 17.2 and later, teardrops are imported as zone objects.
Allegro physical constraint sets are converted into KiCad net classes. The conversion includes clearance rules, trace-width constraints, and differential-pair spacing parameters. Width overrides assigned to specific nets are also retained.
Board outlines, keepout areas, silkscreen graphics, assembly graphics, courtyard boundaries, and text objects are imported using their original positions and font-metric information.

Mentor PADS Importer
The PADS importer operates by reading .asc ASCII export files. It supports both schematics and PCB layouts, making it the most comprehensive of the three new importers in terms of supported design content.
Schematic Import
PADS schematic import includes symbols, wires, junctions, net labels, and connectivity. Multi-unit symbols are reconstructed, while power and ground symbols are mapped to their corresponding entries in the KiCad standard libraries. Hierarchical, multi-sheet structures are preserved, and title-block information is extracted from FIELDS.
Pin types can be converted directly, including passive, input, output, bidirectional, tri-state, open-collector, open-emitter, and power pins. Text annotations retain their height, width, alignment, and rotation. Basic drawing elements such as lines, rectangles, circles, and arcs preserve their fill and line styles.
PCB Import
Imported footprints retain their reference designators, values, positions, rotations, and layer placements. Supported pad shapes include circles, rectangles, ovals, rounded rectangles, and thermal pads. Drill definitions cover plated through-holes, non-plated through-holes, slots, and layer-specific dimensions.
Traces, arcs, and all major via types—including through vias, blind vias, buried vias, and microvias—retain their widths and net assignments. Copper zones preserve their priorities, thermal-relief settings, and net assignments. Keepout areas for traces, vias, copper pours, and component placement are also supported.
The importer supports board outlines, including curved segments, text annotations, dimension lines, graphic elements, test-point definitions, and reuse blocks. Reuse blocks are converted into KiCad groups.
Design rules for clearances, trace widths, via dimensions, hole spacing, and solder-mask expansion are extracted and applied to the board setup. Differential-pair rules are converted into DRC rules in the .kicad_dru file.

gEDA and Lepton EDA Importer
The gEDA importer supports schematics in .sch format, board files in .pcb format, and footprint libraries in .fp format. It is the only one of the three new importers that also supports a footprint-library browser.
Schematic Import
Component graphics are reconstructed from .sym symbol files, including lines, boxes, circles, arcs, and paths. Pin types are mapped to their corresponding KiCad types. When three or more wires intersect, junctions are placed automatically. Bus segments generate the appropriate bus entries.
Hierarchical sub-schematics use the source= attribute and support recursive loading and loop detection. Multi-slot components are reconstructed using the numslots, slot, and slotdef attributes.
Power symbols are identified through the net= attribute. gEDA overbar notation, written as _text\_, is converted into KiCad's ~{text} format. If the original .sym file is unavailable, built-in fallback symbols are provided for common parts such as resistors, capacitors, diodes, transistors, logic gates, and operational amplifiers.

PCB Import
Footprint import includes through-hole pins on both sides of the board, with round or square shapes, as well as surface-mount pads in rectangular, oval, and circular shapes. Pad spacing and solder-mask expansion are converted during import.
Copper traces, arcs, and polygons are imported on all supported layers together with through-hole vias. Net connectivity is reconstructed from the NetList block. Multilayer copper structures with up to 16 layers are supported.

Footprint-Library Browsing
The gEDA importer can browse footprint libraries directly. When an individual .fp file is loaded from a directory-based library, the importer includes its pin and pad definitions, shape and spacing parameters, and silkscreen graphics.
How to Use the New Importers
All three importers are accessible from KiCad's File menu. Create or open a project, select the import option corresponding to the source format, and point KiCad to the source file. Coordinate-system conversion, layer mapping, and unit conversion are handled automatically.
Because KiCad 10 is still under development, users evaluating these features should understand that nightly builds may contain incomplete or changing functionality. KiCad 10 file formats also differ slightly from those used by KiCad 9. A file saved by KiCad 10 cannot be opened by KiCad 9.
After importing a project, the converted design should still be reviewed carefully. Check component positions, layer assignments, pad and drill definitions, board outlines, net connectivity, design rules, and graphical objects before using the project for manufacturing or further release work. Importing preserves a large amount of source information, but verification remains an essential part of any EDA-tool migration.