wiki/ news/ 2003-01-28 - EAGLE PCB CAD Workshop

Tim and Andrew put on a 2 hour workshop for the EAGLE PCB CAD tool. For more information - along with a free download - see Why did we choose EAGLE? Well, in the PSAS we like to use freely available tools which work under both Linux and Windows. EAGLE fits the free, cross platform bill, with some limitations:

But these are all fine since we're usually doing small boards anyway.

Workshop Outline:

1) How to make a PCB

   A) Draw up a schematic (Schematic - .sch files)
      1. You'll probably need to generate some custom parts (Library - .lbr files)
   C) Run an ERC - electrical rule check. Ignore stupid power warnings. Fix everything else.
   D) Do the board layout (Board - .brd files)
      1. Place components (minimize crossing of airwires in the ratsnest)
      2. Route (or autoroute) traces (power, power planes, high frequency, general signals)
      3. Optimize?
   F) Do a DRC - design rule check. Fix all errors, check into warnings.
   G) Generate CAM (Computer Aided Machining) files
      1. Decide what files you need to produce (e.g. Gerber RS274x files: .top, .bot, .drl, etc.)
      2. Setup a CAM program to output those files
      3. Edit drill rack if you only have some drills available
      4. Tile boards in gerbertiler if necessary
   H) DOUBLE CHECK ALL CAM FILES WITH A 3RD PARTY VIEWER (e.g. gerbiewer, gcprevue, etc)
   I) Send off CAM files to a board house, or load them into a PCB router tool.

2) "Let's make a board!" - step by step demonstration of the schematic editor, library editor, board editor, and CAM processor.

3) Traps/Trips/Techniques/Other Demos.

EAGLE Nomenclature:

SIGNAL -- airwire
NET    -- schematic wire
ROUTE  -- board trace
BUS    -- graphical collection of nets

NAME   -- Device
VALUE  -- Device
LABEL  -- Signal (Schematic BUS or NET)

EAGLE Board Layers:

TOP            -- Top side copper
BOTTOM         -- Bottom side copper
ROUTEn         -- Inner signal layers (not Light version)
PADS           -- Through hole device pads
VIAS           -- Plated through holes w/o associated devices
UNROUTED       -- Airwires
DIMENSION      -- Board and Hole outlines, appears on silk screen
t/b DOCU       -- Package element; only shows up in Eagle
t/b PLACE      -- Silk screen
t/b ORIGINS    -- Package crosshairs
t/b NAMES      -- Package names, appears on silk screen
t/b VALUES     -- Package values
t/b STOP       -- Solder mask
t/b CREAM      -- Solder cream
t/b FINISH     -- ???
t/b GLUE       -- Glue

t/b TEST       -- Test info
t/b KEEPOUT    -- No-Go areas for packages
t/b/v RESTRICT -- No-GO areas for tracks
DRILLS         -- Plated through holes
HOLES          -- Non-plated holes
MILLING        -- Areas to be removed by milling
MEASURES       -- ???
DOCUMENT       -- Additional documentation
REFERENCE      -- Reference marks

EAGLE Files:

  .brd -- Boards
  .sch -- Schematics
  .lbr -- Part Libraries
  .scr -- Scripts
  .ulp -- User Language Programs
  .cam -- Computer Aided Manufacture script (or job)
  .dri -- Drill Info
  .gpi -- Gerber Plotter Info file
  .dru -- Design RUles
  .def -- Device Definitions
  .epf -- Eagle Project File (per project settings)
  .key -- Eagle key file (Generated from freeware key at 1st run).

Other files:

GERBER files:
  .cmp -- Component side foil
  .ly(n) -- inner signal layers (Not light version)
  .sol -- Solder side foil
  .plc -- Component side silk screen (PLace Component)
  .pls -- Solder side silk screen (PLace Solder)
  .whl -- aperture (Wheel) shapes
  .stc -- Component side solder mask
  .sts -- Solder side solder mask

Drill files:
  .drd -- NC drill file
  .drl -- Drill Rack File


EAGLE script files (.scr) are EAGLE commands that you could have typed into the command line box bundled together in a file. Not every single command can be done from a script (e.g., you can't mouse click in a script) but most can.

Useful scripts include assigning keyboard shortcuts (e.g.: assign.scr, goodkeys.scr), making pre-built board outlines (e.g.: euro.scr)... anything you want to do over and over again.

User Language Programs

The Eagle User Language Program (.ulp files) is some strange pascal like language which allow you to just about anything in EAGLE. It's a cool feature, but of course we haven't bothered to learn the language. In any case, there are some good ULPs out there, and many can be downloaded from site.



For possibly updated scripts and the latest PSAS eagle library plus other useful information