Rubriques:
Tracks and other items (texts,
drawings ...) use one layer.
Pads and vias use several
layers.
There are 16 copper layers and 12 technical layers.
The
layer parametre used in descriptions has the value:
value |
layer name |
"Copper" layers |
0 |
Copper layer |
|
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) |
|
26 |
ECO2 layer (Other layer used for general drawings) |
|
27 |
Edge layer. Items on Edge layer are seen on all layers |
$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 |
|
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 |
$EndGENERAL |
End description |
This the page size and texts.
$SHEETDESCR |
Start description |
Sheet A4 11700 8267 |
<Page size> X_size Y_size |
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 |
Start block "SETUP" |
InternalUnit 0.000100 INCH |
|
GridSize 500 500 |
Current grid X Y size (500 x 500 units) |
ZoneGridSize 100 |
Grid used for zone filling (100 units, i.e 0.01 inch) |
Layers 2 |
|
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 |
|
$EndSETUP |
End block "SETUP" |
$EQUIPOT describes a net name.
$EQUIPOT |
Start block |
Na 2 "N-000026" |
Na <internal net number> « net name » |
St ~ |
|
$EndEQUIPOT |
End block |
General description (fixed size)
Field description (variable size)
Drawing description (variable size)
Pad description. (variable size)
3D shape informations.
$MODULE bornier6 |
$MODULE <module lib name> |
Po 62000 30500 2700 15 3EC0C28A 3EBF830C ~~ |
|
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 |
|
T0 500 -3000 1030 629 2700 120 N V 21 "P1" |
|
T1 0 3000 1201 825 2700 120 N V 21 "CONN_6" |
T1 = value |
DS -6000 -1500 -6000 1500 120 21 |
|
DS 6000 1500 6000 -1500 120 21 |
An other Draw Segment |
DC ox oy fx fy w |
|
DA x0 y0 x1 y1 angle width layer |
|
$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 |
Normal (Has usualy 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.
$PAD |
Start description |
Sh "2" C 1500 1500 0 0 2700 |
Shape: <pad name> shape Xsize Ysize Xdelta Ydelta Orientation |
Dr 600 0 0 |
Drill <Pad drill> Xoffset Yoffset |
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 |
C (circle)
R (Rectangular).
O (Oblong)
T (Trapèze)
segments (strait line)
circles
arcs
$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 |
shape = 0
Angle is used only for arc segments (unused for line, left for compatibility).
$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 |
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)
$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 |
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.
Example:
$TEXTPCB |
Start description |
Te "TDI" |
Text "string" |
Po 57250 35750 600 600 150 0 |
Position Xstart Ystart Xsize Ysize rotation |
De 15 1 0 0 |
|
$EndTEXTPCB |
End description |
|
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 |
Start description |
Ge 0 24 0 |
|
Te "4,5500''" |
|
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 |
Start description |
Po 0 36750 37000 36550 37000 250 |
|
De 15 0 1 0 400 |
|
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 section is like track section. (There is no via in Zone section).
$ZONE |
Start description |
Po 0 67100 33700 67100 38600 100 |
Same as track description |
De 0 0 2 3EDDB09D 0 |
|
$EndZONE |
End description |
Page -