Legacy PCB (pre 4.0)

This is is for the PCB file format before the sexpr format introduced in KiCad 4.0. This documentation is a mostly verbatim copy of what was written back then and the quality may be poor. This is only included as a reference and is not maintained.

Information about V1 version:

  • Board files ( *.brd files ) are in ASCII format.

  • Dimensions are in 1/10000 inch, except for the page size (in 1/1000 inch).

First line is something as: PCBNEW-BOARD Version 1 date 02/04/2011 15:04:20 All the following descriptions are like this:

$DESCRIPTION
some data
…
$endDESCRIPTION

when <DESCRIPTION> is an identifier which gives the meaning of the data between $DESCRIPTION and $endDESCRIPTION.

Example:

$GENERAL
encoding utf-8
LayerCount 2
Ly 1FFF8001
Links 66
NoConn 0
Di 24940 20675 73708 40323
Ndraw 16
Ntrack 267
Nzone 1929
Nmodule 29
Nnets 26
$EndGENERAL

$SHEETDESCR
Sheet A4 11700 8267
Title ""
Date "23 feb 2004"
Rev ""
Comp ""
Comment1 ""
Comment2 ""
Comment3 ""
Comment4 ""
$EndSHEETDESCR

Information about V2 version:

The file format is exactly the same format, and the extension is still .brd. However, dimensions are in mm (floating notation), except for the page size (in 1/1000 inch). Because the internal Pcbnew unit is now 1nm, the integer coordinates in 1/10000 inch cannot be used in files. Of course, the Pcbnew versions which are in nm are able to read the V1 version files, but can only write files in V2 version. The V2 version should be seen as a temporary way to store boards without loss of resolution.

First line is something as:

PCBNEW-BOARD Version 2 date 22/02/2013 15:04:20

All the following descriptions are like this:

$DESCRIPTION
some data
…
$endDESCRIPTION

Example:

PCBNEW-BOARD Version 2 date 22/02/2013 10:33:30

# Created by Pcbnew(2013-02-20 BZR 3963)-testing

$GENERAL
encoding utf-8
Units mm
LayerCount 2
EnabledLayers 1FFF8001
Links 200
NoConn 0
Di 69.241669 24.89454 202.336401 196.2404
Ndraw 19
Ntrack 779
Nzone 0
BoardThickness 1.6002
Nmodule 25
Nnets 111
$EndGENERAL

Information about new “S expression” version:

For Pcbnew versions in nanometers, the default file format is now using “S expressions”. This new format uses mm for coordinates, fixes issues (like spaces in names) in V1 and V2 versions, and is more human readable than the older format. The new file extension is .kicad_pcb Here is a sample:

(kicad_pcb (version 3) (host pcbnew "(2013-01-12 BZR 3902)-testing")

  (general
    (links 200)
    (no_connects 0)
    (area 69.241669 24.89454 202.336401 196.2404)
    (thickness 1.6002)
    (drawings 19)
    (tracks 779)
    (zones 0)
    (modules 25)
    (nets 111)
  )

  (page A4)
  (title_block
    (title Demo)
    (rev 2.C)
    (company Kicad)
  )

Layer numbering:

Tracks and other items (texts, drawings …​) use one layer. Pads and vias use several layers. There are 16 copper layers and 13 technical layers. The layer parameter used in descriptions has the value:

value

layer name

0

Copper layer

"Copper" layers

1 to 14

Inner layers

15

Component layer

16

Copper side adhesive layer

"Technical" layers

17

Component side adhesive layer

18

Copper side Solder paste layer

19

Component Solder paste layer

20

Copper side Silk screen layer

21

Component Silk screen layer

22

Copper side Solder mask layer

23

Component Solder mask layer

24

Draw layer (Used for general drawings)

25

Comment layer (Other layer used for general drawings)

26

ECO1 layer (Other layer used for general drawings)

27

ECO2 layer (Other layer used for general drawings)

28

Edge layer. Items on Edge layer are seen on all layers

29

Not yet used

30

Not yet used

31

Not yet used

Mask layer: Sometimes, a mask layer parameter is used. It is a 32 bits mask used to indicate a layer group usage (0 up to 32 layers). A mask layer parameter is given in hexadecimal form. Bit 0 is the copper layer, bit 1 is the inner 1 layer, and so on…​(Bit 27 is the Edge layer). Mask layer is the ORed mask of the used layers

First line of description:

Format:

PCBNEW-BOARD Version <version number> date <date>-<time>

Date and time are useful only for information (not used by pcbnew).

$GENERAL

This data is useful only when loading file. It is used by Pcbnew for displaying activity when loading data.

$GENERAL

Start description

Ly 1FFF8001

Obsolete (used for old pcbnew compatibility)

Links 66

Total number of connections

NoConn 0

Remaining connections

Di 24940 20675 73708 40323

Bounding box coordinates:
X_start Y_start X_end Y_end

Ndraw 16

Number of draw items like eged segments, texts…​

Ntrack 267

Number of track segments

Nzone 1929

Number of zone segments

Nmodule 29

Number of modulss

Nnets 26

Number of nets

$SHEETDESCR

This the page size and texts.

$SHEETDESCR

Start description

Sheet A4 11700 8267

<Page size> X_size Y_size in mils (1/1000 inch)

Title ""

Title text

Date "23 feb 2004"

Date text

Rev ""

Revision text

Comp ""

Company name text

Comment1 ""

Comment text, line 1

Comment2 ""

Comment text, line 2

Comment3 ""

Comment text, line 3

Comment4 ""

Comment text, line 4

$EndSHEETDESCR

End description

$SETUP block:

This data bock is used for design settings This is useful only for board edition. Example:

$SETUP
InternalUnit 0.000100 INCH
Layers 2
Layer[0] Cuivre signal
Layer[15] Composant signal
TrackWidth 250
TrackWidthHistory 25
TrackWidthHistory 170
TrackWidthHistory 250
TrackClearence 110
ZoneClearence 150
DrawSegmWidth 150
EdgeSegmWidth 50
ViaSize 600
ViaDrill 250
ViaSizeHistory 600
MicroViaSize 200
MicroViaDrill 80
MicroViasAllowed 0
TextPcbWidth 170
TextPcbSize 600 800
EdgeModWidth 150
TextModSize 600 600
TextModWidth 120
PadSize 1500 2500
PadDrill 1200
AuxiliaryAxisOrg 29500 55500
$EndSETUP

$SETUP

Start block "SETUP"

InternalUnit 0.000100 INCH

Internal unit for Pcbnew, all coordinates are in this unit

Layers 2

Number of layers (2 = double sided board) must be 1 to 16

Layer[0] Cuivre signal

layer name and type
name = name given to the layer by the user (here: "cuivre"
type = signal (not current used in Pcbnew)

Layer[15] Composant signal

TrackWidth 250

Current track width

TrackWidthHistory 170

Last used track widths

TrackWidthHistory 250

TrackWidthHistory 400

TrackClearence 100

Isolation for DRC (Design rules check)

ZoneClearence 200

Isolation used in zone filling

DrawSegmWidth 120

Current segment width for drawings on technical layers

EdgeSegmWidth 120

Current segment width for drawings on "edge layer"

ViaSize 700

Current via size

ViaDrill 250

Via drill for this board

ViaSizeHistory 450

Last used via sizes

ViaSizeHistory 650

ViaSizeHistory 700

TextPcbWidth 120

Current text width for texts on copper or technical layers. This is not for text on footprints

TextPcbSize 600 600

Current text X Y size

EdgeModWidth 120

Current Segment width for footprint edition

TextModSize 120 600

Current text XY size for texts for footprint edition

TextModWidth 120

Current text width for texts for footprint edition

PadSize 700 700

Current X Y pad size (footprint edition)

PadDrill 320

Current pad drill

AuxiliaryAxisOrg 0 0

Auxiliary axis position
(Auxiliary axis is the reference coordinate (0 0 coordinate) for EXCELLON drilling files

$EndSETUP

End block "SETUP"

$EQUIPOT

$EQUIPOT describes a net name.

$EQUIPOT

Start block

Na 2 "N-000026"

Na <internal net number> « net name »

St ~

$EndEQUIPOT

End block

Note1: Internal net number is an arbitrary number. It is computed by Pcbnew when compiling netlist. Note2: Net 0 is not a real net. Net 0 is the net number used internally by Pcbnew for all the no connected pads.

Example:

$EQUIPOT;
Na 0 ""
St ~
$EndEQUIPOT
$EQUIPOT
Na 1 "DONE"
St ~
$EndEQUIPOT
$EQUIPOT
Na 2 "N-000026"
St ~
$EndEQUIPOT
$EQUIPOT
Na 3 "TD0/PROG"
St ~
$EndEQUIPOT

$MODULE

Description start by: $MODULE <module name>`

And ends with $EndMODULE <module name>`

Module description has four sections:

  1. General description (fixed size)

  2. Field description (variable size)

  3. Drawing description (variable size)

  4. Pad description. (variable size)

  5. 3D shape informations.

Note: All coordinates are relative to the module position. Its means the coordinates of segments, pads, texts …​ are given for a module in position 0, rotation 0. If a module is rotated or mirrored, real coordinates must be computed according to the real position and rotation.

General description:

$MODULE bornier6

$MODULE <module lib name>

Po 62000 30500 2700 15 3EC0C28A 3EBF830C ~~

Po Xpos Ypos Orientation(0.1deg) Layer TimeStamp Attribut1Attribut2
Attribut1 = ~or 'F' for autoplace (F = Fixed, ~= moveable)
Attribut2 = ~or 'P' for autoplace (P = autoplaced)

Li bornier6

Li <module lib name>

Cd Bornier d’alimentation 4 pins

Cd comment description (displayed when browsing libraries)

Kw DEV

Kw Keyword1 Keyword2 …​ (for footprint selection by keywords)

Sc 3EBF830C

Sc TimeStampOp

Op 0 0 0

Op <rotation cost 90 deg> <rotation cost 180 deg> for auto place.
rotation cost = 0 (no rotation allowed) to 10 (null cost)

Note: Usually, components are on layer 15 (component layer) or 0 (copper layer). If the component is on layer 0, it is"mirrored". The "mirror axis is the X axis

Field Description:

There are 2 to 12 fields

Field 0 = component reference (U1, R5 …​) (required) Field 1 = component value (10K, 74LS02 …​) (required) Other fields (optional) are comments. Format:

T<field number> <Xpos> <Ypos> <Xsize> <Ysize> <rotation> <penWidth> N <visible> <layer> "text"`

Field

Units

Meaning

field number

enumeration

0⇒reference, 1⇒value, etc.

Xpos

tenths of mils (.0001 inches)

The horizontal offset relative to the module’s overall position

Ypos

tenths of mils (.0001 inches)

The vertical offset relative to the module’s overall position

Xsize

tenths of mils (.0001 inches)

The horizontal size of the character 'M'

Ysize

tenths of mils (.0001 inches)

The vertical size of the character 'M'

rotation

tenths of degrees

Angular rotation from horizontal, counterclockwise

penWidth

tenths of mils (.0001 inches)

Width of the pen used to draw characters

N

none

flag for the parser?

visible

boolean

I⇒ invisible, V⇒ visible

layer

enumeration

see layer numbers above

Examples:

T0 500 -3000 1030 629 2700 120 N V 21 "P1"

T0 ⇒ reference

T1 0 3000 1201 825 2700 120 N V 21 "CONN_6"

T1 ⇒ value

Drawings:

Tells how to draw module shape. They cannot be on a copper layer (DRC ignore them) Drawings are segment, circle, arc, polygon.

Draw segment:

DS -6000 -1500 -6000 1500 120 21

DS is a Draw Segment
DS Xstart Ystart Xend Yend Width Layer

DS 6000 1500 6000 -1500 120 21

An other Draw Segment

Circle:

DC Xcentre Ycentre Xpoint Ypoint Width Layer

DC is a Draw Circle
Xpoint, Ypoint is a point on the circle.

Arc:

DA Xcentre Ycentre Xstart_point Ystart_point angle width layer

DA is a Draw Arc
angle is the arc angle in 0.1 degrees

Polygon:

DP 0 0 0 0 corners_count width layer

Draw Polygon
First line of a polygon.
The polygon should be closed, otherwise this is a poly-line.
width is the thickness of outlines.

Dl corner_posx corner_posy

Corner coordinate
( corners_count lines like this)

Pad Descriptions:

All the pads of this footprint are listed here (Many $PAD/$EndPAD sections here).. See $PAD description.

$SHAPE3D

3D shape informations: The real shape description is a vrml file, build by Wings3d. This shape can be scaled, moved and rotated. This is because a single 3D shape can be used for many footprints (for instance, we use the shape resistor.wrl for several resistor footprints, by tuning the X, Y, Z scale of the 3D shape according to the different size of resistor footprints). Some smd footprints are using this feature. For the same reasons, the 3D shape can be moved (by the move factor) and/or rotated. Real shape unit is 0.1 inch (1 unit vrml = 0.1 inch = 2.54 millimeter). An other reason exists: when a footprint is very big ( a big connector) or very small (a small SMD resistor) we must create a 3D shape small or bigger than real size, in order to use easily the 3D modeler.

$SHAPE3D

Start description

Na "device/bornier_6.wrl"

FileName (default path is kicad/modules/packages3d/)

Sc 1.000000 1.000000 1.000000

X Y Z scale factor

Of 0.000000 0.000000 0.000000

X Y Z offset (move vector, in 3D units (0.1 inch))

Ro 0.000000 0.000000 0.000000

X Y Z rotation (in degree)

$EndSHAPE3D

End description

The 3D shape coordinates are relative to the footprint coordinates. The 3D shape must be scale, moved and rotated according to the parameters Sc Of and Ro, and after moved and rotated according to the footprint coordinates and rotation. If the footprint is « inverted » (that is, located on copper side) the 3D shape must be « inverted » too. Note: A footprint may have several 3D shapes (for instance an integrated circuit and his socket).

$PAD

Pads have different shapes and attributes. Pad shapes are: * Circle. * Oblong(or oval). * Rectangular (Square is like a rectangle). * Trapeze.

Pad attributes are:

  • Normal (Has usually a hole)

  • Smd (used for Surface Mounted Devices). Has no hole.

  • Connector (used for connectors like a PC Board Bus connector)

  • Mechanical. (Like a hole for mechanical use)

And shape can be draw with an offset related to the drilling hole. The hole shale is round or oblong

$PAD

Start description

Sh "2" C 1500 1500 0 0 2700

Shape: <pad name> shape Xsize Ysize Xdelta Ydelta Orientation

Dr 600 0 0
or (oblong hole)
Dr 600 0 0 O 600 650

Drill <Pad drill> Xoffset Yoffset (round hole)
or (oblong hole)
Drill <Pad drill.x> Xoffset Yoffset <Hole shape> <Pad drill.x> <Pad drill.y>

At STD N 00E0FFFF

Attributs: <Pad type> N <layer mask>

Ne 8 "GND"

Net reference of the pad: <netnumber> <net name>

Po -3000 0

X_pos Y_pos (relative to the module position)

$EndPAD

End description

Note: <Pad type> is the Pad Attribute. It is one of: "STD" "SMD" "CONN" "HOLE" "MECA". Shape is one of:

  • C (circle)

  • R (Rectangular).

  • O (Oblong)

  • T (Trapèze) Hole shape = O (O for Oblong)

Example:

$PAD
Sh "3" C 1500 1500 0 0 2700
Dr 600 0 0
At STD N 00E0FFFF
Ne 10 "TD0_1"
Po -1000 0
$EndPAD

Graphic items:

There are drawing items like segments, circles, texts, targets and cotations.

$DRAWSEGMENT

Draw segments are:

  • segments (strait line)

  • circles

  • arcs

Line:

$DRAWSEGMENT

Start description

Po 0 67500 39000 65500 39000 120

Position shape Xstart Ystart Xend Yend width

De 28 0 900 0 0

Description layer type angle timestamp status

$EndDRAWSEGMENT

End description

Note:

  • shape = 0

  • Angle is used only for arc segments (unused for line, left for compatibility).

Circle:

$DRAWSEGMENT

Start description

Po 1 67500 39000 65500 39000 120

Position shape Xcentre Ycentre Xend Yend width

De 28 0 900 0 0

Description layer type angle timestamp status

$EndDRAWSEGMENT

End description

Note: * shape = 1 * Angle is used only for arc segments (unused for circle, left for compatibility). * End is a point of this circle. (If Xend or Yend is 0, the other coordinate is the radius)

Arc:

$DRAWSEGMENT

Start description

Po 2 67500 39000 65500 39000 120

Position shape Xstart Ystart Xend Yend width

De 28 0 900 0 0

Description layer type angle timestamp status

$EndDRAWSEGMENT

End description

Note:

  • shape = 2

  • start and end are the 2 points of the arc. angle is the arc angle (in 0.1 degree). Center coordinates are computed by pcbnew from start, end and angle. Currently, only 90 degrees arcs are supported.(thereby, angle = 900)

Example:

$DRAWSEGMENT
Po 0 67500 34000 67500 39000 120
De 28 0 900 0
$EndDRAWSEGMENT

$TEXTPCB

$TEXTPCB

Start description

Te "TDI"

Text "string"

Po 57250 35750 600 600 150 0

Position Xstart Ystart Xsize Ysize Width rotation

De 15 1 B98C Normal

Description layer normal timestamp style
normal = 0 : text is mirrored.
normal = 1 : text is normal.
style = Normal or Italic

$EndTEXTPCB

End description

Example:

$TEXTPCB
Te "TCK"
Po 57250 33500 600 600 150 0
De 15 1 B98C Normal
$EndTEXTPCB

$MIRE

 shape 1
shape 0

$MIREPCB

Start description

Po 0 28 28000 51000 5000 150 00000000

Position shape Xpos Ypos size width timestamp

$EndMIREPCB

End description

$COTATION

$COTATION

Start description

Ge 0 24 0

General shape layer timestamp
currently, shape = 0.

Te "4,5500''"

Text "string"
string is the cotation value in inches or millimeters

Po 50250 5791 600 800 170 0 1

Position (for text) Xpos Ypos Xsize Ysize width orient normal

Sb 0 27500 6501 73000 6501 150

Coordinates of segments (axis, arrows…​)

Sd 0 73000 9000 73000 5081 150

Sg 0 27500 9000 27500 5081 150

S1 0 73000 6501 72557 6731 150

S2 0 73000 6501 72557 6271 150

S3 0 27500 6501 27943 6731 150

S4 0 27500 6501 27943 6271 150

$EndCOTATION

End description

Track, vias and Zone section:

$TRACK

Track section decribes tracks and vias on copper layers. Each track (or via) has a two line description: For a track segment:

Position shape Xstart Ystart Xend Yend width
Description layer 0 netcode timestamp status Shape parameter is set to 0 (reserved for future changes).

For a via: Position shape Xstart Ystart Xend Yend diameter
Description layer 1 netcode timestamp status

For a via, layer parameter gives : On the 4 less significant bits: the starting layer of the via
On the 4 next bits: the ending layer.

For instance, a via starting at copper kayer (layer 0) end ending at component layer (layer 15 has the layer parametre set to F0 hexadecimal or 240 decimal.
Shape parameter is the via type (through = 3, blind = 2, buried = 1)
Timestamp parameters are set to 0 (reserved for future changes).
Status parameter can be set to 0 (Used internally for routing infos)..

$TRACK

Start description

Po 0 36750 37000 36550 37000 250

Position shape Xstart Ystart Xend Yend width width = diameter for a via

De 15 0 1 0 400

Description layer type netcode timestamp status
type = 0 for a track segment.
type = 1 for a via

Po 0 39000 36750 38750 37000 250

An other track

De 15 0 1 0 0

Po 3 53500 27000 53500 27000 650

This is a via (via "through") from layer 15 (component) to layer 0 (copper)

De 15 1 14 0 0

$EndTRACK

End description

$ZONE

Zone section is like track section. (There is no via in Zone section). It is used to handle a zone filling, from a zone outline.

$ZONE

Start description

Po 0 67100 33700 67100 38600 100

Same as track description

De 0 0 2 3EDDB09D 0

$EndZONE

End description

$CZONE_OUTLINE

Describes the main outlines of a zone and the outlines of filled areas (solid polygons) inside the zone main outlines. Outlines of filled areas can be missing (if the zone is not currently filled) Because a zone handles thermal reliefs, there are options to describe pads in zones options and thermal reliefs parameters. Example:

$CZONE_OUTLINE
ZInfo 47868246 1 "GND"
ZLayer 0
ZAux 4 E
ZClearance 150 T
ZMinThickness 190
ZOptions 0 32 F 200 200
ZCorner 74750 51750 0
ZCorner 74750 13250 0
ZCorner 29750 13250 0
ZCorner 29750 51750 1
....
$POLYSCORNERS
74655 51655 0 0
74655 13345 0 0
...
$endPOLYSCORNERS
$endCZONE_OUTLINE

$CZONE_OUTLINE

Start description

ZInfo 478E3FC8 1 "/aux_sheet/INPUT" <Time stamp> <internal netcode> "net name"

ZLayer 0 Layer (0 = copper, 15 = component, 1 ..14 = inner layers)

ZAux 4 E <corners count> <zone hatching option>

zone hatching option = N (none), E (edge hatching) or F (full hatching)

ZClearance 200 T <Zone clearance> <pads option = I, T or X>

I = pads in zone

T = Thermal reliefs

X = pads not in zone.

ZMinThickness 190 <Zone min thickness (for copper zone)>

ZOptions 0 32 F 200 200 <fill mode> <arc approx> <antipad thickness> <thermal stubs width>

fill mode = 0 (use solid polygons) or 1 (use segments)

arc approx = 16 or 32 (segments count to approximate a 360 arc)

ZCorner 49450 19150 0 First corner (external outline)

ZCorner 40600 19150 0 Next corner

ZCorner 40600 22850 0

ZCorner 49450 22850 1 End corner (flag = 1)

$POLYSCORNERS Start of filled areas outlines

74655 51655 0 0 First corner (first filled area outline)

74655 13345 0 0 Next corner

$endPOLYSCORNERS

Other example:

$CZONE_OUTLINE	Start description of an other outline
ZInfo 47B3E800 3 "VCC"
ZLayer 1
ZAux 8 F
ZClearance 200 T
ZMinThickness 190	Zone min thickness (for copper zone)
ZOptions 0 32 F 200 200
ZCorner 49704 23032 0	First corner (external outline)
ZCorner 49704 18940 0
ZCorner 46140 19024 0
ZCorner 46148 20000 0
ZCorner 45250 20000 0
ZCorner 44750 21250 0
ZCorner 43750 22250 0
ZCorner 46176 23068 1	End corner (flag = 1)
ZCorner 48450 19900 0	First corner (this is a hole)
ZCorner 48450 20800 0
ZCorner 47350 20800 0
ZCorner 47250 19900 1	End corner (flag = 1)
$endCZONE_OUTLINE	End description

$EndBOARD

$EndBOARD terminates the whole board description. Must be the last line.

Last Modified