Eagle is the CAD of choice for many peoples on low budget due to the flexible price policy of Cadsoft, which allow peoples to use limited version of their CAD as freeware if used for personal purpose. In other hads once you get used to it you love it and don't want to replace it with anything else which usually works slower and have less flexibility. The power of Eagle is in the ULP extensions which allow users to add new functionality to Eagle i.e. making our own commands etc.

  • I'm total beginner and try to make my first PCB with Eagle, what procedure to follow to be sure that I don't do something wrong or silly?
  • Welcome to the wonderful wolrd of PCB design :) If you are beginner please follow these steps and you will make perfect boards from the very first time:

    1. Read our TECHNICAL INFO, FAQ and Design Tips web pages before you start your boards
    2. Make your schematic and then route your board, don't route just board without schematic as this is easy way to forget connection or to do something wrong. Once your schematic is correct Eagle will not allow you to route board different than the schematic (i.e. to forget to connect something or to connect it on wrong place)
    3. When you are ready with board routing run 8mils.dru and if there are errors fix them
    4. Postprocess your BRD file to Gerbers and NC drill as written below
    5. Download Gerberviewer from our Design Tools page
    6. Import your files in the Gerberviewer and re-view them carefully
    7. If evrythings looks fine send the generated Gerbers+NC drill or the BRD file to us, don't forget the README.TXT
  • I want to learn how to postprocess my Eagle .BRD files by myself?
  • It's easy. Just do the following steps:

    1. open your BRD file and run drillcfg ULP, this will create your "rack" file i.e. drill tool assignment file with extension xxx.DRL (we'll need this file for your PCB manufacturing so don't forget where you saved it)
    2. see below how to increase the Eagle default drill precision and make the necessary fixes, you need to do this only once
    3. run Excellon.cam and process your board with generated DRL rack from the ULP script, this will create xxx.DRD file which keeps XY coordinates (we'll need this file for your PCB manufacturing so don't forget where you saved it)
    4. run Gerb274x and Generate gerbers from your board files, it's very important to use Gerb274x not "Gerber" and the latest will not produce correct files, but the obsolete RS274D format (Cadsoft peoples are silly to confuse you so much putting this old stuff on their CAD aren't they?). Gerb274x will create several files from which we need xxx.CMP - your top copper gerber file, xxx.SOL - your bottom copper gerber file, xxx.PLC - your component print gerber file, xxx.STC - your top soldermask gerber file, xxx.STS - your bottom soldermask gerber file
    5. Zip these files: xxx.CMP, xxx.SOL, xxx.STC, xxx.STS, xxx.PLC, xxx.DRL, xxx.DRD, README.TXT and send to us at fastpcb@olimex.com you will receive PO form with your order confirmation
  • How do I change the Eagle NC drill file precision?
  • By default Eagle generates the NC drill files with 2.3 file format (i.e. 3 digits after the decimal point) in some cases if your board is designed in Imperial units (while default Eagle database units are metric) and the board is high density there is small error due to the rounding when the drill XY coordinates are generated. This leads to small displacement of the holes inside the pad area i.e. your holes are not in the center of your pads. You can increase the NC drill precision by following procedure:

    Go in your EAGLE BIN folder and make copy of EAGLE.DEF file, then open it and change [EXCELLON] section as follows:

    Type = DrillStation
    Long = "Excellon drill station"
    Init = "%%\n"
    Reset = "M30\n"
    ResX = 100000
    ResY = 100000
    ;Rack = ""
    Select = "%s\n" ; (Drill code)
    Drill = "X%6.0fY%6.0f\n" ; (x, y)
    Info = "Drill File Info:\n"\
    " Data Mode : Absolute\n"\
    " Units : 1/1000 Inch\n"\
    " End Of Block : CR/LF\n"\
  • How can I find what drill sizes are used in my BRD design?
  • Do run DRILLCFG.ULP which will extract all drill sizes you are using.
  • I'm sending you my Eagle BRD file. Can you postprocess my BRD file with layers different than the default Eagle CAM layers?
  • No.We postprocess Eagle BRD files with only default Eagle CAM layers. If you want other layers than defaults please postprocess your BRD file by yourself (see below how).
  • What should i know when I use copper pour (polygons)?
  • Eagle put the polygon copper on 8 mils distance by default (when ISOLATE parameter is 0). Use ISOLATE=10-12 mils to increase your copper distance from your pads and tracks.
  • What happens if I send for production both Gerbers and Eagle BRD?
  • We just will ignore the Gerbers and process the BRD file, so please decide which files you want to have your board manufactured from and send only Gerbers or BRD.
  • Is there way I can make my Eagle libraries with Olimex standard drill sizes?
  • Yes, someone already did such ULP which you can download from Eagle web site. The name of the ULP is change_libraries_to_olimex_drills.zip
  • How can I panelize my small boards inside Eagle?
  • Customer of ours wrote GREAT Tutorial how to PANELIZE your Eagle boards together in panel.