EasyEDA

Introduction

KiCad imports designs from two EasyEDA format families: EasyEDA Standard (also known as JLCEDA Standard / LCEDA Standard) and EasyEDA Pro (also known as JLCEDA Pro / LCEDA Pro). These formats have different file structures and use separate parsers. EasyEDA Standard stores design data as JSON with tilde-delimited shape strings. EasyEDA Pro stores design data as ZIP archives containing JSON Lines files.

EasyEDA Standard File Types

.json — single JSON document containing a schematic sheet, symbol, PCB, or footprint
.zip — archive containing one or more JSON documents

EasyEDA Pro File Types

.epro — project archive (renamed ZIP)
.zip — project archive
.elibz — library archive
.efoo — individual footprint file
.esym — individual symbol file

EasyEDA Standard does not support project-level import. EasyEDA Pro provides a project chooser when the archive contains multiple schematics or boards.

EasyEDA Standard Format

JSON Document Structure

Each EasyEDA Standard file is a JSON object with the following top-level fields:

Field Type Description

Field	Type	Description
`docType`	integer or string	Document type (may appear here or inside `head`)
`head`	object	Header with `docType`, `editorVersion`, `title`, `description`, origin `x`/`y`, and optional `c_para` component parameters
`canvas`	string	Canvas configuration data
`title`	string	Document title
`shape`	array of strings	Design elements as tilde-delimited shape strings
`dataStr`	object	Additional data (PCB layers, DRC rules, etc.)

docType

integer or string

Document type (may appear here or inside head)

head

object

Header with docType, editorVersion, title, description, origin x/y, and optional c_para component parameters

canvas

string

Canvas configuration data

title

string

Document title

shape

array of strings

Design elements as tilde-delimited shape strings

dataStr

object

Additional data (PCB layers, DRC rules, etc.)

The head.docType field determines what content the file contains. Its value may be encoded as either an integer or a string representation of an integer.

DOC_TYPE Values

Value Enum Name Description

Value	Enum Name	Description
1	SCHEMATIC_SHEET	Single schematic sheet
2	SYMBOL	Schematic symbol definition
3	PCB	PCB layout
4	PCB_COMPONENT	Footprint definition
5	SCHEMATIC_LIST	Container holding multiple schematic sheets in a `schematics` array
14	PCB_MODULE	PCB module (sub-board)

SCHEMATIC_SHEET

Single schematic sheet

SYMBOL

Schematic symbol definition

PCB

PCB layout

PCB_COMPONENT

Footprint definition

SCHEMATIC_LIST

Container holding multiple schematic sheets in a schematics array

PCB_MODULE

PCB module (sub-board)

For DOC_TYPE 5 (SCHEMATIC_LIST), the JSON object contains a schematics array where each element is a complete DOCUMENT object with its own head, shape, and other fields. KiCad imports each sheet and creates sub-sheets automatically.

Component Parameters (c_para)

The head.c_para object and the dataStr field carry component-level metadata. For symbols and footprints this includes package, pre (reference prefix), Contributor, link (datasheet URL), and Model_3D. For PCBs, dataStr contains a layers array, an optional uuid, and an optional DRCRULE object with track width, clearance, via diameter, and via drill constraints.

Shape Array Encoding

All design elements in the shape array use a common encoding. Each shape is a single tilde-delimited (~) string. The first field is a type prefix; remaining fields are positional parameters specific to that type.

Multi-line shapes use the delimiter @$ to join lines that were originally separate entries. When parsing, the importer replaces @$ with newline characters and splits on newlines.

Pin definitions within symbol shapes use the separator ^^ to delimit pin sub-parts (dot position, path/color, name, number, and optional decoration data).

Coordinate System and Scaling

EasyEDA Standard uses a coordinate system where values are in abstract units. The schematic parser converts these to KiCad internal units using:

ScaleSize(value) = round(MilsToIU(value * 10))

This multiplies the EasyEDA value by 10 to get mils, then converts mils to KiCad internal units (nanometers).

The PCB parser uses a different formula:

ScaleSize(value) = round((value * 254000.0) / 100.0) * 100

This converts from EasyEDA PCB units (which are 10 mil increments) to KiCad internal units with rounding to the nearest 100nm.

Both parsers support relative positioning through m_relOrigin, which is set to the document or component origin. Positions are computed as ScaleSize(value - origin).

Schematic Shape Types

Schematic documents and symbol definitions share many of the same shape types. When a shape appears at the schematic level (inside a LIB compound or at the top level), it is parsed in a schematic coordinate context. When it appears in a symbol definition, positions are relative to the symbol origin.

Top-Level Schematic Shapes

Prefix Parameter Layout

Prefix	Parameter Layout
`LIB`	`LIB_xy_paramsrotation_~importFlaglayer~…` followed by child shape lines joined with `#@$`. The `params` field is a backtick-delimited key-value list (e.g., `name``R1``package``0402`). Rotation is in degrees. The layer field (index 7) indicates front (1) or back (2) placement for PCB footprints.
`F`	`F_flagTypenamex_yangle~…` with pin sub-parts separated by `^^`. The third `^^`-segment contains the value text, position, angle, alignment, font, and size. Flag type names determine the power symbol style (e.g., `part_netLabel_gnD` for power ground, `part_netLabel_VCC` for VCC bar). The special flag type `part_netLabel_netPort` creates a global label instead of a power symbol.
`W`	`W_pointsstrokeColor_lineWidthstrokeStyle_fillColor~locked`. Points is a space-delimited list of x,y coordinate pairs. Creates wire segments between consecutive points.
`N`	`N_xy_angle_netname_haligntextX_textYfontname~fontSize`. Creates a net label at the specified position with the given rotation and text alignment.
`O`	`O_xy`. Creates a no-connect marker at the specified position.
`J`	`J_xy~diameter`. Creates a junction at the specified position.
`T`	`T_textTypex_yangle_colorfontname_fontSize_{~baselineAlign}_textvisible~halign`. Creates a text element. The `textType` field is unused at the schematic level. Text supports `\n` for newlines and HTML entity encoding. The `halign` field accepts `start`, `middle`, `end`, or `inherit`. The `baselineAlign` field controls vertical positioning relative to the text baseline (supports SVG values like `alphabetic`, `central`, `middle`, `hanging`, etc.).
`R`	`R_xy_rxry_widthheight_strokeColorlineWidth_strokeStylefillColor~~locked`. Creates a rectangle. The `rx`/`ry` fields specify corner radii but are not currently imported (rounded rectangles become sharp rectangles).
`I`	`I_xy_widthheight_angleimageUrl_~transformData`. Creates an image from a data URL (base64-encoded SVG or raster). The `transformData` field contains CSS-like transforms (`scale`, `translate`, `rotate`) applied in reverse order.

LIB

LIB_xy_paramsrotation_~importFlaglayer~… followed by child shape lines joined with #@$. The params field is a backtick-delimited key-value list (e.g., name`R1``package``0402`). Rotation is in degrees. The layer field (index 7) indicates front (1) or back (2) placement for PCB footprints.

F

F_flagTypenamex_yangle~… with pin sub-parts separated by ^^. The third ^^-segment contains the value text, position, angle, alignment, font, and size. Flag type names determine the power symbol style (e.g., part_netLabel_gnD for power ground, part_netLabel_VCC for VCC bar). The special flag type part_netLabel_netPort creates a global label instead of a power symbol.

W

W_pointsstrokeColor_lineWidthstrokeStyle_fillColor~locked. Points is a space-delimited list of x,y coordinate pairs. Creates wire segments between consecutive points.

N

N_xy_angle_netname_haligntextX_textYfontname~fontSize. Creates a net label at the specified position with the given rotation and text alignment.

O

O_xy. Creates a no-connect marker at the specified position.

J

J_xy~diameter. Creates a junction at the specified position.

T

T_textTypex_yangle_colorfontname_fontSize_{~baselineAlign}_textvisible~halign. Creates a text element. The textType field is unused at the schematic level. Text supports \n for newlines and HTML entity encoding. The halign field accepts start, middle, end, or inherit. The baselineAlign field controls vertical positioning relative to the text baseline (supports SVG values like alphabetic, central, middle, hanging, etc.).

R

R_xy_rxry_widthheight_strokeColorlineWidth_strokeStylefillColor~~locked. Creates a rectangle. The rx/ry fields specify corner radii but are not currently imported (rounded rectangles become sharp rectangles).

I

I_xy_widthheight_angleimageUrl_~transformData. Creates an image from a data URL (base64-encoded SVG or raster). The transformData field contains CSS-like transforms (scale, translate, rotate) applied in reverse order.

Symbol Shape Types

These shapes appear inside symbol definitions (within LIB compound shapes or standalone symbol files).

Prefix Parameter Layout

Prefix	Parameter Layout
`PL`	`PL_pointsstrokeColor_lineWidthstrokeStyle_fillColor~locked`. Polyline drawn through space-delimited x,y coordinate pairs.
`PG`	`PG_pointsstrokeColor_lineWidthstrokeStyle_fillColor~locked`. Closed polygon using the same point format as `PL`.
`PT`	`PT_pathDatastrokeColor_lineWidthstrokeStyle_fillColor~locked`. Freedraw shape using SVG-like path commands (M, L, A, C, Z).
`Pimage`	`Pimage_~_angle_xy_widthheight~dataUrl`. Embedded image within a symbol, using a base64 data URL. Supports SVG and raster formats.
`A`	`A_pathData_strokeColorlineWidth_strokeStylefillColor~~locked`. Arc shape using SVG path data containing M and A commands.
`R`	`R_xy_rxry_widthheight_strokeColorlineWidth_strokeStylefillColor~~locked`. Rectangle within a symbol. Corner radii are parsed but not applied.
`E`	`E_cxcy_rxry_strokeColorlineWidth_strokeStylefillColor~~locked`. Ellipse defined by center and radii. Only the X radius is used (treated as a circle).
`P`	Pin definition using `^^` separators between five or seven sub-parts. Sub-part 0: `P_showelecType_pinNumberx_yrotation`. Sub-part 1: `dotX~dotY` (pin dot position). Sub-part 2: `pathData_color…` (pin line path, parsed as `M x,y h length` or `M x,y v length`). Sub-part 3: `nameVisible_~~pinName` (pin name and visibility). Sub-part 4: `numVisible_~~pinNumber` (pin number and visibility). Optional sub-parts 5-6: `hasDot_dotXdotY` and `hasClock~clockPath` for inverted and clock pin decorations.
`T`	`T_textTypex_yangle_colorfontname_fontSize_{~baselineAlign}_textvisible~halign`. Text element within a symbol. The `textType` field determines the field role: `P` maps to the reference field, `N` maps to the value field, any other value creates a plain text item.

PL

PL_pointsstrokeColor_lineWidthstrokeStyle_fillColor~locked. Polyline drawn through space-delimited x,y coordinate pairs.

PG

PG_pointsstrokeColor_lineWidthstrokeStyle_fillColor~locked. Closed polygon using the same point format as PL.

PT

PT_pathDatastrokeColor_lineWidthstrokeStyle_fillColor~locked. Freedraw shape using SVG-like path commands (M, L, A, C, Z).

Pimage

Pimage_~_angle_xy_widthheight~dataUrl. Embedded image within a symbol, using a base64 data URL. Supports SVG and raster formats.

A

A_pathData_strokeColorlineWidth_strokeStylefillColor~~locked. Arc shape using SVG path data containing M and A commands.

R

R_xy_rxry_widthheight_strokeColorlineWidth_strokeStylefillColor~~locked. Rectangle within a symbol. Corner radii are parsed but not applied.

E

E_cxcy_rxry_strokeColorlineWidth_strokeStylefillColor~~locked. Ellipse defined by center and radii. Only the X radius is used (treated as a circle).

P

Pin definition using ^^ separators between five or seven sub-parts. Sub-part 0: P_showelecType_pinNumberx_yrotation. Sub-part 1: dotX~dotY (pin dot position). Sub-part 2: pathData_color… (pin line path, parsed as M x,y h length or M x,y v length). Sub-part 3: nameVisible_~~pinName (pin name and visibility). Sub-part 4: numVisible_~~pinNumber (pin number and visibility). Optional sub-parts 5-6: hasDot_dotXdotY and hasClock~clockPath for inverted and clock pin decorations.

T

T_textTypex_yangle_colorfontname_fontSize_{~baselineAlign}_textvisible~halign. Text element within a symbol. The textType field determines the field role: P maps to the reference field, N maps to the value field, any other value creates a plain text item.

Pin Electrical Types

Pin electrical types are encoded as single-character numeric strings in the elecType field of pin definitions.

Value KiCad Mapping

Value	KiCad Mapping
`0`	Unspecified
`1`	Input
`2`	Output
`3`	Bidirectional
`4`	Passive

0

Unspecified

1

Input

2

Output

3

Bidirectional

4

Passive

Stroke Styles

Line stroke styles are encoded as numeric strings.

Value Style

Value	Style
`0`	Solid
`1`	Dash
`2`	Dot

0

Solid

1

Dash

2

Dot

Power Flag Styles

Power symbols use a numeric style identifier that determines the generated KiCad symbol graphics.

Value Style Name Flag Type Name

Value	Style Name	Flag Type Name
0	Circle	`part_netLabel_Bar` (flipped)
1	Arrow	(generic)
2	Bar	`part_netLabel_gNd`, `part_netLabel_VCC` (flipped), `part_netLabel_+5V` (flipped), `part_netLabel_VEE`, `part_netLabel_-5V`
3	Wave	(generic)
4	Power Ground	`part_netLabel_gnD`
5	Signal Ground	`part_netLabel_GNd`
6	Earth	`part_netLabel_GnD`
7	GOST Arrow	(generic)
8	GOST Power Ground	(generic)
9	GOST Earth	(generic)
10	GOST Bar	(generic)

Circle

part_netLabel_Bar (flipped)

Arrow

(generic)

Bar

part_netLabel_gNd, part_netLabel_VCC (flipped), part_netLabel_+5V (flipped), part_netLabel_VEE, part_netLabel_-5V

Wave

(generic)

Power Ground

part_netLabel_gnD

Signal Ground

part_netLabel_GNd

Earth

part_netLabel_GnD

GOST Arrow

(generic)

GOST Power Ground

(generic)

GOST Earth

(generic)

GOST Bar

(generic)

PCB Shape Types

PCB documents use the same tilde-delimited shape encoding. Shapes appear at the board level or within LIB compound shapes representing footprints.

Prefix Parameter Layout

Prefix	Parameter Layout
`LIB`	`LIB_xy_paramsrotation_~importFlaglayer~…` followed by child shapes joined with `#@$`. The `params` field uses backtick-delimited key-value pairs. Layer 1 is front, layer 2 is back.
`TRACK`	`TRACK_widthlayer_netnamepoints`. Points is a space-delimited coordinate list. Creates PCB track segments between consecutive coordinate pairs. On non-copper layers, segments are created as graphical shapes instead.
`CIRCLE`	`CIRCLE_cxcy_radiuswidth_layer~~netname`. Creates a circle with the given center, radius, and stroke width on the specified layer.
`RECT`	`RECT_xy_widthheight_layer_~strokeWidthfillColor~~netname`. Creates a filled or unfilled rectangle.
`ARC`	`ARC_strokeWidthlayer_netnamepathData`. The path data uses SVG-style M and A commands to define the arc geometry. Arc center is computed from start, end, radius, far-flag, and direction-flag using the standard SVG arc algorithm.
`DIMENSION`	`DIMENSION_layershapeData_~textHeight_~lineWidth`. The shape data contains SVG path commands defining dimension lines. These are imported as grouped line segments, not native KiCad dimension objects.
`SOLIDREGION`	`SOLIDREGION_layernetname_pathDatatype`. Creates either a board cutout (when layer is `11`) or a filled zone. The `type` field may be `cutout` (rule area preventing zone fills) or empty (solid fill with full pad connection).
`COPPERAREA`	`COPPERAREA_strokeWidthlayer_netnamepathData_clearancefillStyle_~thermal keepIsland_fillData_~fillOrder_~_{improveFabrication}spokeWidth`. Creates a copper zone with fill data. The `fillData` field is a JSON array of polygon contour arrays. `thermal` may be `direct` (full pad connection). `keepIsland` may be `yes` (never remove islands). `fillOrder` controls zone priority (higher values have lower priority). `spokeWidth` sets thermal relief spoke width.
`SVGNODE`	`SVGNODE~jsonData`. The JSON payload has `nodeType` (1 for element nodes), `layerid`, and `attrs`. On layer 19 with `c_etype=outline3D`, this defines a 3D model reference with `uuid`, `title`, `c_origin`, `c_rotation`, `c_width`, `c_height`, and `z` offset. On other layers, the `d` attribute contains SVG path data defining filled polygon outlines.
`TEXT`	`TEXT_textTypex_ystrokeWidth_rotation_layer_fontSizetext_geometry~ display~font`. The `textType` field maps to footprint fields: `P` for reference, `N` for value. The `display` field set to `none` creates a hidden field.
`VIA`	`VIA_xy_diameter_netnamedrillRadius`. Creates a through-hole via. Inside footprints, creates a PTH pad instead.
`HOLE`	`HOLE_xy_radiusuuid`. Creates an NPTH (non-plated through-hole) drill. At the board level, a standalone footprint is created to contain the hole.
`PAD`	`PAD_shapex_ywidth_heightlayer_netnamenumber_holeDiapolyPoints_rotation uuid_holeLength_plated_{~pasteExpansion}maskExpansion`. Pad shape types: `ELLIPSE` (oval), `RECT` (rectangle), `OVAL` (circle if equal dimensions, oval otherwise), `POLYGON` (custom shape from point data). Layer `11` indicates through-hole; the `plated` field (`Y`/`N`) determines PTH vs. NPTH. Layer 1 is front SMD, layer 2 is back SMD.

LIB

LIB_xy_paramsrotation_~importFlaglayer~… followed by child shapes joined with #@$. The params field uses backtick-delimited key-value pairs. Layer 1 is front, layer 2 is back.

TRACK

TRACK_widthlayer_netnamepoints. Points is a space-delimited coordinate list. Creates PCB track segments between consecutive coordinate pairs. On non-copper layers, segments are created as graphical shapes instead.

CIRCLE

CIRCLE_cxcy_radiuswidth_layer~~netname. Creates a circle with the given center, radius, and stroke width on the specified layer.

RECT

RECT_xy_widthheight_layer_~strokeWidthfillColor~~netname. Creates a filled or unfilled rectangle.

ARC

ARC_strokeWidthlayer_netnamepathData. The path data uses SVG-style M and A commands to define the arc geometry. Arc center is computed from start, end, radius, far-flag, and direction-flag using the standard SVG arc algorithm.

DIMENSION

DIMENSION_layershapeData_~textHeight_~lineWidth. The shape data contains SVG path commands defining dimension lines. These are imported as grouped line segments, not native KiCad dimension objects.

SOLIDREGION

SOLIDREGION_layernetname_pathDatatype. Creates either a board cutout (when layer is 11) or a filled zone. The type field may be cutout (rule area preventing zone fills) or empty (solid fill with full pad connection).

COPPERAREA

COPPERAREA_strokeWidthlayer_netnamepathData_clearancefillStyle_~thermal keepIsland_fillData_~fillOrder_~_{improveFabrication}spokeWidth. Creates a copper zone with fill data. The fillData field is a JSON array of polygon contour arrays. thermal may be direct (full pad connection). keepIsland may be yes (never remove islands). fillOrder controls zone priority (higher values have lower priority). spokeWidth sets thermal relief spoke width.

SVGNODE

SVGNODE~jsonData. The JSON payload has nodeType (1 for element nodes), layerid, and attrs. On layer 19 with c_etype=outline3D, this defines a 3D model reference with uuid, title, c_origin, c_rotation, c_width, c_height, and z offset. On other layers, the d attribute contains SVG path data defining filled polygon outlines.

TEXT

TEXT_textTypex_ystrokeWidth_rotation_layer_fontSizetext_geometry~ display~font. The textType field maps to footprint fields: P for reference, N for value. The display field set to none creates a hidden field.

VIA

VIA_xy_diameter_netnamedrillRadius. Creates a through-hole via. Inside footprints, creates a PTH pad instead.

HOLE

HOLE_xy_radiusuuid. Creates an NPTH (non-plated through-hole) drill. At the board level, a standalone footprint is created to contain the hole.

PAD

PAD_shapex_ywidth_heightlayer_netnamenumber_holeDiapolyPoints_rotation uuid_holeLength_plated_{~pasteExpansion}maskExpansion. Pad shape types: ELLIPSE (oval), RECT (rectangle), OVAL (circle if equal dimensions, oval otherwise), POLYGON (custom shape from point data). Layer 11 indicates through-hole; the plated field (Y/N) determines PTH vs. NPTH. Layer 1 is front SMD, layer 2 is back SMD.

Layer Mapping

EasyEDA Standard uses numeric layer identifiers that map to KiCad layers.

EasyEDA Layer	KiCad Layer	Description
1	F.Cu	Front copper
2	B.Cu	Back copper
3	F.SilkS	Front silkscreen
4	B.SilkS	Back silkscreen
5	F.Paste	Front solder paste
6	B.Paste	Back solder paste
7	F.Mask	Front solder mask
8	B.Mask	Back solder mask
10	Edge.Cuts	Board outline
11	Eco1.User	Multi-layer / board cutout
12	Dwgs.User	Document layer
13	F.Fab	Front fabrication
14	B.Fab	Back fabrication
15	Eco2.User	Eco2 user layer
19	F.Fab	3D model layer
21-50	In1.Cu-In30.Cu	Inner copper layers

EasyEDA Layer

KiCad Layer

Description

F.Cu

Front copper

B.Cu

Back copper

F.SilkS

Front silkscreen

B.SilkS

Back silkscreen

F.Paste

Front solder paste

B.Paste

Back solder paste

F.Mask

Front solder mask

B.Mask

Back solder mask

Edge.Cuts

Board outline

Eco1.User

Multi-layer / board cutout

Dwgs.User

Document layer

F.Fab

Front fabrication

B.Fab

Back fabrication

Eco2.User

Eco2 user layer

F.Fab

3D model layer

21-50

In1.Cu-In30.Cu

Inner copper layers

EasyEDA Pro Format

ZIP Archive Structure

EasyEDA Pro files are ZIP archives with the following internal structure:

File Description

File	Description
`project.json`	Project manifest with schematics, boards, PCBs, devices, symbols, footprints, and their relationships
`device.json`	Device library manifest (in `.elibz` archives)
`footprint.json`	Footprint library manifest (in `.elibz` archives)
`symbol.json`	Symbol library manifest (in `.elibz` archives)
`*.esch`	Schematic sheet (JSON Lines format)
`*.epcb`	PCB layout (JSON Lines format)
`*.esym`	Symbol definition (JSON Lines format)
`*.efoo`	Footprint definition (JSON Lines format)
`*.eblob`	Binary blob data (embedded images)
`*.ecop`	Poured copper data (JSON Lines format)

project.json

Project manifest with schematics, boards, PCBs, devices, symbols, footprints, and their relationships

device.json

Device library manifest (in .elibz archives)

footprint.json

Footprint library manifest (in .elibz archives)

symbol.json

Symbol library manifest (in .elibz archives)

*.esch

Schematic sheet (JSON Lines format)

*.epcb

PCB layout (JSON Lines format)

*.esym

Symbol definition (JSON Lines format)

*.efoo

Footprint definition (JSON Lines format)

*.eblob

Binary blob data (embedded images)

*.ecop

Poured copper data (JSON Lines format)

project.json Structure

The project manifest is a standard JSON object with the following top-level keys:

schematics — map of schematic UUIDs to objects with name and sheets (each sheet has id, name, uuid)
boards — map of board UUIDs to objects with schematic and pcb UUID references
pcbs — map of PCB UUIDs to PCB names or objects with title
devices — map of device UUIDs to objects with source, description, title, version, tags, custom_tags, and attributes (containing Symbol, Footprint, 3D Model, 3D Model Title, 3D Model Transform, and custom attributes)
symbols — map of symbol UUIDs to objects with source, title, version, type (symbol type integer), desc, tags, and custom_tags
footprints — map of footprint UUIDs to objects with source, title, version, type, desc, tags, and custom_tags

Symbol Types

Value	Enum Name	Description
2	NORMAL	Standard schematic symbol
18	POWER_PORT	Power port (creates global power label)
19	NETPORT	Net port (creates global label)
20	SHEET_SYMBOL	Sheet symbol for hierarchy
22	SHORT	Short symbol

Value

Enum Name

Description

NORMAL

Standard schematic symbol

POWER_PORT

Power port (creates global power label)

NETPORT

Net port (creates global label)

SHEET_SYMBOL

Sheet symbol for hierarchy

SHORT

Short symbol

JSON Lines Format

Internal design files (.esch, .epcb, .esym, .efoo) use the JSON Lines format where each line is a standalone JSON array. The first element of each array is a string type identifier that determines how the remaining elements are interpreted.

Empty lines serve as section separators. In .efoo files, an empty line separates footprint data from PCB data, allowing both to coexist in a single file.

Coordinate System and Scaling

EasyEDA Pro uses a different coordinate system from Standard. The Y axis is inverted relative to KiCad (EasyEDA Pro Y increases downward; KiCad schematic Y increases upward).

The schematic parser scales values as:

ScaleSize(value) = round(MilsToIU(value * 10))
ScalePos(x, y) = (ScaleSize(x), -ScaleSize(y))

The PCB parser uses a different scale factor:

ScaleSize(value) = round(value * 25400.0 / 500.0) * 500
ScalePos(x, y) = (ScaleSize(x), -ScaleSize(y))

Both include Y-axis inversion in position calculations. The PCB scale formula converts from EasyEDA Pro units to nanometers with rounding to the nearest 500nm.

Schematic Line Types

Type Identifier Array Layout

Type Identifier	Array Layout
`HEAD`	`["HEAD", config]` where `config` is an object with `originX`, `originY`, `maxId`, `version`, and `symbolType` (integer matching the SYMBOL_TYPE enum).
`COMPONENT`	`["COMPONENT", id, name, x, y, rotation, mirror, customProps, unk]`. Places a component instance. Attributes for this component (Device, Symbol, Designator, etc.) are linked via ATTR lines with matching `parentId`.
`WIRE`	`["WIRE", id, geometry, lineStyle]`. The `geometry` field is an array of coordinate arrays, where each sub-array defines a polyline segment as `[x1, y1, x2, y2, …]`.
`ATTR`	`["ATTR", id, parentId, key, value, keyVisible, valVisible, x, y, rotation, fontStyle]`. Attributes attach to their parent by `parentId`. When `parentId` is empty, the attribute belongs to the document root. Standard keys include `Device`, `Symbol`, `Designator`, `Name`, `Value`, `Global Net Name`, `Description`, `Footprint`, and `Unique ID`.
`RECT`	`["RECT", id, x1, y1, x2, y2, …, lineStyleId]`. Rectangle with start and end corners.
`CIRCLE`	`["CIRCLE", id, cx, cy, radius, lineStyleId]`. Circle with center and radius.
`ARC`	`["ARC", id, startX, startY, midX, midY, endX, endY, lineStyleId]`. Arc defined by start, midpoint, and end.
`POLY`	`["POLY", id, [x1, y1, x2, y2, …], closed, lineStyleId]`. Polyline or polygon with coordinate array.
`BEZIER`	`["BEZIER", id, [x1, y1, cx1, cy1, cx2, cy2, x2, y2], lineStyleId]`. Cubic bezier curve with start, two control points, and end.
`TEXT`	`["TEXT", id, x, y, angle, text, fontStyleId]`. Text element with position, rotation, and named font style reference.
`OBJ`	`["OBJ", id, unk, …]`. Embedded image object. Two variants exist depending on whether element 3 is a number (inline format with x, y, w, h, angle, flipped, dataUrl) or a string (mime-prefixed format with mimeType, x, y, w, h, angle, data). Images may reference `blob:objectId` URLs that resolve through the blob map.
`PIN`	`["PIN", id, unk1, unk2, x, y, length, rotation, unk3, invertedFlag]`. Pin definition within a symbol. `invertedFlag` value of 2 indicates an inverted (bubble) pin. Pin attributes (Pin Name, Pin Number, Pin Type, NO_CONNECT) are linked via ATTR lines.
`PART`	`["PART", partId]`. Marks the beginning of a new unit in a multi-unit symbol.
`LINESTYLE`	`["LINESTYLE", id, …]`. Named line style definition with color, dash pattern, and thickness.
`FONTSTYLE`	`["FONTSTYLE", id, unk1, unk2, color, fontName, fontSize, …, valign, halign]`. Named font style definition. Font size is scaled by 0.62 during import. Alignment values: 0=top/left, 1=center, 2=bottom/right.

HEAD

["HEAD", config] where config is an object with originX, originY, maxId, version, and symbolType (integer matching the SYMBOL_TYPE enum).

COMPONENT

["COMPONENT", id, name, x, y, rotation, mirror, customProps, unk]. Places a component instance. Attributes for this component (Device, Symbol, Designator, etc.) are linked via ATTR lines with matching parentId.

WIRE

["WIRE", id, geometry, lineStyle]. The geometry field is an array of coordinate arrays, where each sub-array defines a polyline segment as [x1, y1, x2, y2, …].

ATTR

["ATTR", id, parentId, key, value, keyVisible, valVisible, x, y, rotation, fontStyle]. Attributes attach to their parent by parentId. When parentId is empty, the attribute belongs to the document root. Standard keys include Device, Symbol, Designator, Name, Value, Global Net Name, Description, Footprint, and Unique ID.

RECT

["RECT", id, x1, y1, x2, y2, …, lineStyleId]. Rectangle with start and end corners.

CIRCLE

["CIRCLE", id, cx, cy, radius, lineStyleId]. Circle with center and radius.

ARC

["ARC", id, startX, startY, midX, midY, endX, endY, lineStyleId]. Arc defined by start, midpoint, and end.

POLY

["POLY", id, [x1, y1, x2, y2, …], closed, lineStyleId]. Polyline or polygon with coordinate array.

BEZIER

["BEZIER", id, [x1, y1, cx1, cy1, cx2, cy2, x2, y2], lineStyleId]. Cubic bezier curve with start, two control points, and end.

TEXT

["TEXT", id, x, y, angle, text, fontStyleId]. Text element with position, rotation, and named font style reference.

OBJ

["OBJ", id, unk, …]. Embedded image object. Two variants exist depending on whether element 3 is a number (inline format with x, y, w, h, angle, flipped, dataUrl) or a string (mime-prefixed format with mimeType, x, y, w, h, angle, data). Images may reference blob:objectId URLs that resolve through the blob map.

PIN

["PIN", id, unk1, unk2, x, y, length, rotation, unk3, invertedFlag]. Pin definition within a symbol. invertedFlag value of 2 indicates an inverted (bubble) pin. Pin attributes (Pin Name, Pin Number, Pin Type, NO_CONNECT) are linked via ATTR lines.

PART

["PART", partId]. Marks the beginning of a new unit in a multi-unit symbol.

LINESTYLE

["LINESTYLE", id, …]. Named line style definition with color, dash pattern, and thickness.

FONTSTYLE

["FONTSTYLE", id, unk1, unk2, color, fontName, fontSize, …, valign, halign]. Named font style definition. Font size is scaled by 0.62 during import. Alignment values: 0=top/left, 1=center, 2=bottom/right.

PCB Line Types

Type Identifier Array Layout

Type Identifier	Array Layout
`LAYER`	`["LAYER", layerId, layerType, layerName, enableFlag]`. Layer configuration. When `enableFlag` is non-zero, the layer is added to the board’s enabled layer set.
`NET`	`["NET", netname]`. Net declaration. All nets must be declared before they are referenced by other elements.
`RULE`	`["RULE", ruleType, ruleName, isDefault, ruleData]`. Design rule. Rule type `3` is track width (data: `[units, min, opt, max]`). Rule type `1` is clearance (data: `[units, clearanceTable]`).
`VIA`	`["VIA", id, unk, netname, unk2, x, y, drill, diameter]`. Through-hole via placement.
`LINE`	`["LINE", id, unk, netname, layer, startX, startY, endX, endY, width]`. Single track segment.
`ARC`	`["ARC", id, unk, netname, layer, startX, startY, endX, endY, angle, width]`. Arc track segment. The `angle` field is the included arc angle in degrees; arc center is computed from start, end, and angle using perpendicular bisector geometry.
`POLY`	`["POLY", id, unk, netname, layer, thickness, polyData]`. Graphical polyline. The `polyData` field is a JSON array using the Pro polygon encoding (see below).
`FILL`	`["FILL", id, unk, netname, layer, width, unk2, polyDataList]`. Solid copper fill. Creates a zone with the fill polygon as pre-poured data. Angles in fill poly data are scaled by 10x.
`POUR`	`["POUR", id, unk, netname, layer, lineWidth, pourName, fillOrder, polyDataList]`. Copper pour zone outline. `fillOrder` determines zone priority. Poured copper data is provided separately through POURED lines or `.ecop` files.
`POURED`	`["POURED", pouredId, parentPourId, unk, isPoly, polyData]`. Poured copper fill data linked to a POUR by `parentPourId`. The `isPoly` flag distinguishes between solid fill contours and thermal relief spoke geometry.
`TEARDROP`	`["TEARDROP", id, netname, layer, polyData]`. Teardrop shape imported as a pre-filled zone with unspecified teardrop type.
`REGION`	`["REGION", id, unk, layer, width, flags, polyDataList]`. Rule area or board outline. The `flags` set determines restrictions: flag 2 = no footprints, flag 5 = no tracks, flag 6/8 = no zone fills, flag 7 = no copper at all (tracks, vias, pads, fills).
`PAD`	`["PAD", id, unk, netname, layer, padNumber, x, y, orientation, holeData, shapeData, …, drillDirection]`. The `holeData` array is `[holeType, width, height]` where holeType is `ROUND` or `SLOT`. A hole with zero dimensions creates an SMD pad. The `shapeData` array is `[shapeName, …]` where shapeName is `RECT` (`[w, h, cornerRadiusPct]`), `ELLIPSE` (`[w, h]`), `OVAL` (`[w, h]`), or `POLY`/`POLYGON` (`[polyData]`).
`IMAGE`	`["IMAGE", id, unk, layer, x, y, width, height, angle, mirror, polyDataList]`. Reference image defined by polygon outlines scaled to the specified dimensions.
`OBJ`	`["OBJ", id, unk, layer, unk2, x, y, width, height, angle, flipped, imageUrl]`. Bitmap image with support for blob URLs.
`STRING`	`["STRING", id, unk, layer, x, y, text, font, height, strokeWidth, …, align, angle, inverted, unk, mirror]`. PCB text element. The `align` field uses a 1-9 grid (1=top-left through 9=bottom-right).
`COMPONENT`	`["COMPONENT", compId, unk, layer, x, y, orientation, localAttribs]`. Places a footprint instance. The `localAttribs` field is a map of attribute overrides. Component attributes (Device, Footprint, Designator) and pad nets are linked via ATTR and PAD_NET lines with matching component ID.
`ATTR`	`["ATTR", id, unk, parentId, layer, x, y, key, value, keyVisible, valVisible, fontName, height, strokeWidth, …, textOrigin, rotation, inverted]`. PCB attribute attached to a component or standalone. The `textOrigin` field uses the same 1-9 alignment grid as STRING.
`PAD_NET`	`["PAD_NET", compId, padNumber, netname]`. Assigns a net to a specific pad within a component.
`DOCTYPE`	Document type identifier line (appears in some file formats).
`HEAD`	Header configuration line.

LAYER

["LAYER", layerId, layerType, layerName, enableFlag]. Layer configuration. When enableFlag is non-zero, the layer is added to the board’s enabled layer set.

NET

["NET", netname]. Net declaration. All nets must be declared before they are referenced by other elements.

RULE

["RULE", ruleType, ruleName, isDefault, ruleData]. Design rule. Rule type 3 is track width (data: [units, min, opt, max]). Rule type 1 is clearance (data: [units, clearanceTable]).

VIA

["VIA", id, unk, netname, unk2, x, y, drill, diameter]. Through-hole via placement.

LINE

["LINE", id, unk, netname, layer, startX, startY, endX, endY, width]. Single track segment.

ARC

["ARC", id, unk, netname, layer, startX, startY, endX, endY, angle, width]. Arc track segment. The angle field is the included arc angle in degrees; arc center is computed from start, end, and angle using perpendicular bisector geometry.

POLY

["POLY", id, unk, netname, layer, thickness, polyData]. Graphical polyline. The polyData field is a JSON array using the Pro polygon encoding (see below).

FILL

["FILL", id, unk, netname, layer, width, unk2, polyDataList]. Solid copper fill. Creates a zone with the fill polygon as pre-poured data. Angles in fill poly data are scaled by 10x.

POUR

["POUR", id, unk, netname, layer, lineWidth, pourName, fillOrder, polyDataList]. Copper pour zone outline. fillOrder determines zone priority. Poured copper data is provided separately through POURED lines or .ecop files.

POURED

["POURED", pouredId, parentPourId, unk, isPoly, polyData]. Poured copper fill data linked to a POUR by parentPourId. The isPoly flag distinguishes between solid fill contours and thermal relief spoke geometry.

TEARDROP

["TEARDROP", id, netname, layer, polyData]. Teardrop shape imported as a pre-filled zone with unspecified teardrop type.

REGION

["REGION", id, unk, layer, width, flags, polyDataList]. Rule area or board outline. The flags set determines restrictions: flag 2 = no footprints, flag 5 = no tracks, flag 6/8 = no zone fills, flag 7 = no copper at all (tracks, vias, pads, fills).

PAD

["PAD", id, unk, netname, layer, padNumber, x, y, orientation, holeData, shapeData, …, drillDirection]. The holeData array is [holeType, width, height] where holeType is ROUND or SLOT. A hole with zero dimensions creates an SMD pad. The shapeData array is [shapeName, …] where shapeName is RECT ([w, h, cornerRadiusPct]), ELLIPSE ([w, h]), OVAL ([w, h]), or POLY/POLYGON ([polyData]).

IMAGE

["IMAGE", id, unk, layer, x, y, width, height, angle, mirror, polyDataList]. Reference image defined by polygon outlines scaled to the specified dimensions.

OBJ

["OBJ", id, unk, layer, unk2, x, y, width, height, angle, flipped, imageUrl]. Bitmap image with support for blob URLs.

STRING

["STRING", id, unk, layer, x, y, text, font, height, strokeWidth, …, align, angle, inverted, unk, mirror]. PCB text element. The align field uses a 1-9 grid (1=top-left through 9=bottom-right).

COMPONENT

["COMPONENT", compId, unk, layer, x, y, orientation, localAttribs]. Places a footprint instance. The localAttribs field is a map of attribute overrides. Component attributes (Device, Footprint, Designator) and pad nets are linked via ATTR and PAD_NET lines with matching component ID.

ATTR

["ATTR", id, unk, parentId, layer, x, y, key, value, keyVisible, valVisible, fontName, height, strokeWidth, …, textOrigin, rotation, inverted]. PCB attribute attached to a component or standalone. The textOrigin field uses the same 1-9 alignment grid as STRING.

PAD_NET

["PAD_NET", compId, padNumber, netname]. Assigns a net to a specific pad within a component.

DOCTYPE

Document type identifier line (appears in some file formats).

HEAD

Header configuration line.

Pro Polygon Encoding

EasyEDA Pro uses a JSON array encoding for polygon contour data, distinct from the SVG-like path strings in Standard. Elements alternate between coordinate pairs and command strings:

Command Parameters

Command	Parameters
(numbers)	`x, y` — sets the current point
`L`	followed by `x, y` pairs — line-to commands
`ARC`	`angle, endX, endY` — arc from current point to end with given angle
`CARC`	`angle, endX, endY` — same as ARC (alternate name)
`C`	`cx1, cy1, cx2, cy2, x, y` — cubic bezier curve
`CIRCLE`	`cx, cy, radius` — standalone circle
`R`	`x, y, width, height, angle [, cornerRadius]` — rectangle with optional rounded corners and rotation

(numbers)

x, y — sets the current point

L

followed by x, y pairs — line-to commands

ARC

angle, endX, endY — arc from current point to end with given angle

CARC

angle, endX, endY — same as ARC (alternate name)

C

cx1, cy1, cx2, cy2, x, y — cubic bezier curve

CIRCLE

cx, cy, radius — standalone circle

R

x, y, width, height, angle [, cornerRadius] — rectangle with optional rounded corners and rotation

In fill data from .epcb files, arc angles are multiplied by 10 and must be divided during import.

Symbol and Footprint Line Types

Symbol files (.esym) use the same line types as schematic files (HEAD, PIN, ATTR, PART, RECT, CIRCLE, ARC, POLY, BEZIER, TEXT, OBJ, LINESTYLE, FONTSTYLE).

Footprint files (.efoo) use the same line types as PCB files (POLY, PAD, FILL, ATTR, REGION). An empty line in a .efoo file separates the footprint data from additional PCB-level data.

Pro Layer Mapping

EasyEDA Pro uses a different layer numbering scheme from Standard.

EasyEDA Pro Layer	KiCad Layer	Description
1	F.Cu	Front copper
2	B.Cu	Back copper
3	F.SilkS	Front silkscreen
4	B.SilkS	Back silkscreen
5	F.Mask	Front solder mask
6	B.Mask	Back solder mask
7	F.Paste	Front solder paste
8	B.Paste	Back solder paste
9	F.Fab	Front fabrication
10	B.Fab	Back fabrication
11	Edge.Cuts	Board outline
12	Edge.Cuts	Multi-layer (also maps to Edge.Cuts)
13	Dwgs.User	Document layer
14	Eco2.User	Eco2 user layer
15-44	In1.Cu-In30.Cu	Inner copper layers
48	F.Fab	Component shape layer
49	F.Fab	Component marking
53	User.4	3D shell outline
54	User.5	3D shell top
55	User.6	3D shell bottom
56	User.7	Drill drawing

EasyEDA Pro Layer

KiCad Layer

Description

F.Cu

Front copper

B.Cu

Back copper

F.SilkS

Front silkscreen

B.SilkS

Back silkscreen

F.Mask

Front solder mask

B.Mask

Back solder mask

F.Paste

Front solder paste

B.Paste

Back solder paste

F.Fab

Front fabrication

B.Fab

Back fabrication

Edge.Cuts

Board outline

Edge.Cuts

Multi-layer (also maps to Edge.Cuts)

Dwgs.User

Document layer

Eco2.User

Eco2 user layer

15-44

In1.Cu-In30.Cu

Inner copper layers

F.Fab

Component shape layer

F.Fab

Component marking

User.4

3D shell outline

User.5

3D shell top

User.6

3D shell bottom

User.7

Drill drawing

Note that the solder mask and paste layer numbering differs between Standard and Pro. In Standard, paste is layers 5/6 and mask is 7/8. In Pro, mask is layers 5/6 and paste is 7/8.

Schematic

Imported Elements

Symbol instances with reference, value, and custom fields
Multi-sheet schematics (Standard creates sub-sheets automatically; Pro supports sheet hierarchy)
Wires, net labels, junctions, and no-connect markers
Power symbols with multiple flag styles (circle, arrow, bar, wave, power ground, signal ground, earth, and GOST variants)
Global labels (net ports)
Text elements with font, size, rotation, and alignment
Rectangles and images (SVG and raster, both inline and blob-referenced)
Pin electrical types and visibility control
Multi-unit symbols (Pro)
Components with symbol references and device attribute mapping (Pro)
Named font and line style lookups (Pro)

Limitations

Rounded rectangles are not supported; corner radius values are ignored.
Ellipses are treated as circles using only the X radius.
Image and bitmap rotation is not applied in Pro.
Per-unit symbol attributes are limited to unit 1 in Pro.
Standalone .esym file import is partially disabled.

Layout

Imported Elements

Board outline with automatic shape healing (segments within 1.5mm are joined)
Tracks, vias, and arcs with width, layer, and net assignment
Pads with multiple shape types:
- Standard: ellipse (oval), rectangle, oval, polygon (custom)
- Pro: rectangle (with optional corner radius percentage for rounded rect), ellipse, oval, polygon
Pad attributes (SMD, PTH, NPTH) with front/back/through-hole layer configuration
Copper zones with fill data, thermal relief, island removal, and priority
Solid regions including board cutouts
Copper pours with pre-poured data (Pro)
Teardrops converted to zones (Pro)
Rule areas with configurable restrictions (no copper, no tracks, no fills, no footprints)
Circles, rectangles, arcs, dimensions, and text
SVG node shapes with filled polygon outlines (Standard)
3D model references with offset, rotation, and fit dimensions
Footprints with auto-generated courtyard if missing
Layer mapping for up to 30 inner copper layers
DRC rules (track width, clearance, via diameter, via drill)
Solder paste and mask expansion per pad
Reference images (Pro)
Net assignment from project data (Pro)

Limitations

Dimensions are imported as grouped line segments, not native dimension objects (Standard).
3D model paths are hardcoded to ${KIPRJMOD}/EASYEDA_MODELS/.
Component rotation is limited to 90-degree increments in some cases (Pro).
Poured copper from .ecop files is disabled by default (Pro).
The importer is read-only.

Undocumented Areas

The following aspects of the EasyEDA formats are not fully understood or documented:

The complete set of canvas field parameters in Standard format documents.
Exact behavior of all stroke style and fill mode combinations.
The full range of SVGNODE node types beyond type 1 (element nodes).
Image transform concatenation edge cases in Standard format.
The complete set of REGION flags in Pro format beyond flags 2, 5, 6, 7, and 8.
Differences between JLCEDA V2 and V3 attribute naming (Pro uses both NAME/NUMBER and Pin Name/Pin Number depending on the editor version).
The unk fields present in many Pro line types, which appear to be reserved or format-version-dependent.