gEDA / Lepton EDA

Every file begins with a version line:

YYYYMMDD is a release date (e.g., 20130925) that identifies the minimum gEDA version required to read the file. N is the file format version number (typically 1 or 2). The version number is optional in very early format files.

The KiCad importer validates that the date is a plausible value (>= 19700101) and uses it for version-aware parsing decisions.

Each object begins with a single-character type identifier as the first non-whitespace character on a line. The parameters follow on the same line, separated by spaces.

Component lines are typically followed by an attribute block ({ }) containing attribute text objects that override or extend the symbol’s default attributes. Common attributes include:

Draws a net segment from (x1, y1) to (x2, y2). The color field is the gEDA color index (typically 4 for nets). The importer ignores color and maps all nets to KiCad wire objects.

Draws a bus segment. The ripperdir field (-1, 0, or 1) indicates which direction bus entry stubs should extend. The importer creates KiCad bus wire objects and generates bus entry objects where net endpoints touch bus segments.

Defines a pin on a symbol. The first coordinate pair is the connection point (the end that connects to nets) and the second is the other end. The whichend field (0 or 1) specifies which endpoint is the active connection point.

Pin attributes are defined in a { } block following the P line:

When a text object appears inside a { } block and contains an = character, it is parsed as an attribute with a name=value pair. Floating text objects (outside attribute blocks) are imported as KiCad SCH_TEXT objects.

Attribute blocks begin with { on its own line and end with } on its own line. They can follow any object type but are most commonly found after C (component) and P (pin) lines. Each entry inside the block is a T (text) object whose content is a name=value pair.

Components can be defined inline rather than loaded from external .sym files. An embedded component begins with [ on its own line after the C line and its attribute block, and ends with ]. The content between [ and ] is a complete symbol definition using the same object types (P, L, B, V, A, T, H).

When a C line references a symbol basename (e.g., resistor-1.sym), the symbol is resolved through the following search order:

The built-in symbol library includes common passives (resistors, capacitors, inductors), semiconductors (diodes, LEDs, BJTs, MOSFETs), op-amps, logic gates (7400 series), power symbols (GND, Vcc, Vdd, etc.), and I/O port symbols.

gEDA identifies power symbols by a net= attribute on the symbol definition (not on the schematic instance). The format is net=NETNAME:PINNUMBER. Symbols with this attribute become KiCad power symbols with a global label at the pin position.

Examples: net=GND:1, net=Vcc:1, net=+5V:1.

gEDA supports hierarchical designs through the source= attribute on component instances. A component with a source= attribute naming another .sch file becomes a KiCad SCH_SHEET, and the sub-schematic is loaded recursively. The import call stack is tracked to detect circular references.

gEDA schematic coordinates are integers in mils (thousandths of an inch) with the Y axis pointing upward. KiCad schematic coordinates use 100-nanometer internal units (IU) with the Y axis pointing downward.

Conversion formula:

The importer runs two passes: first it parses all objects and tracks the maximum Y coordinate, then it flips all Y coordinates during post-processing. This preserves relative positioning despite the axis inversion.

The gEDA PCB format has three unit conventions determined by both file age and syntax:

The bracket type after each keyword determines the unit convention. [ means centimils (100000 per inch). Values with an explicit mm or mil suffix are converted to centimils before further processing:

All values are then converted to KiCad internal units (nanometers):

A PCB file begins with an optional comment block (lines starting with #), a file version declaration, and a board header:

The PCB header declares the board name and dimensions. It is followed by global settings:

Elements define footprints placed on the board. Multiple syntax variants exist depending on format version:

An Element contains sub-objects enclosed between ( and ):

A Pad is defined by a line segment from (X1,Y1) to (X2,Y2) with a given thickness. The resulting pad shape is the line segment swept by a circle (or square) of the specified thickness.

The pad shape depends on the square flag:

The onsolder flag (bit 0x0080) places the pad on the back copper layer instead of the front.

These define silkscreen graphics within an Element. ElementLine draws a simple line segment. ElementArc draws an arc (or circle when DeltaAngle is 360 degrees).

gEDA PCB does not directly support circles as a primitive. Full circles are represented as arcs with a DeltaAngle of 360.

Arc angles use gEDA’s convention:

All vias are imported as through-hole vias spanning all copper layers (F.Cu to B.Cu). The gEDA format does not support blind or buried vias.

Layer blocks contain the board-level copper traces, shapes, arcs, and copper polygons. Layer numbering is 1-based:

Lines on copper layers are imported as PCB_TRACK objects. Lines on non-copper layers become PCB_SHAPE objects. Arcs on copper layers become PCB_ARC objects. Polygons become ZONE objects.

The NetList block at the end of the file defines the electrical connectivity. Each Net contains Connect entries that reference component pads using the format refdes-padnumber (e.g., R1-1, C1-2).

gEDA PCB objects use two flag formats:

Key flag values:

Layer mapping uses both the numeric index and the layer name string. Name-based matching takes precedence when the name contains a recognized keyword.