Creating Printed Circuit Boards using EAGLE and the Roland EGX-300 Engraver


There are four stages to the PCB design and manufacturing process:

  1. Design stage. Here the board is designed using EAGLE's schematic draw and board layout programs. There are special considerations based on the fact that the board will be produced on the Roland Engraver.

  2. File Prep stage. Here CAD files are produced from EAGLE and other external conversion tools. The ultimate goal is HPGL (Hewlett-Packard Graphics Language) .plt files which can be sent directly to the engraver.

  3. File Preview stage. At this stage, we load the HPGL CAD files into GraphicCode's free “GCPREVUE,”. This venerable PCB CAD file viewer program lets us verify that the files were outputted properly.

  4. Manufacturing Stage. In this stage, the board is actually manufactured. Steps include: anchoring the blank PCB to the workspace; XY calibration of the machine to your board files and the location of the blank PCB; installation of engraving tools and drills, and Z axis calibration before each tool is used.

Let's begin!

Design Stage

We will be designing single sided PCBs with copper layer on the solder side (bottom).

Here are some considerations for board layout in EAGLE.

When your board design is done, we move on to the File Preparation Stage!


File Preparation Stage

  1. Create Solder Side Artwork. From the EAGLE PCB program, choose File:Cam Processor. From the CAM Processor window, choose File:Open:Job. Select the gerb274x job. Click the tab to the Solder side and then click the "Process Section" button at the bottom. You don't have to process the whole job. This creates a file with a .sol (solder side) suffix.

  2. Create Drill Configuration File. From the EAGLE PCB program, select File:Run... and then select drillcfg.ulp. Choose inches as the units. When done, it will create a file with a .DRL suffix, which contains tooling information (your drill diameters), e.g.:
    T01 0.024in
    T02 0.032in
    T03 0.040in
    T04 0.047in
    T05 0.066in

    You won't need this file directly, but it's used in the very next stage.

  3. Create NC Drill File. From the EAGLE PCB program, choose File:Cam Processor. From the CAM Processor window, choose File:Open:Job. Select the excellon job. Make sure to select the Mirror checkbox. You'll be drilling from the bottom just as you're engraving from the bottom, so you need to mirror. Click on either Process Job or Process Section (there is only one section, so “process job” will do the right thing). This creates a file with a .ncd (NC Drill) suffix.

  4. Create Engraver File from .sol File Use MIT web tool to create engraver path from solder side file, Give it your .sol file. It will return a file with a .plt suffix.

  5. Create Drill Hit Files from the NCD File. Use Fred's Java program to create drill hit file(s) from NC Drill file, Download this file to your working directory and then compile it with javac Then run it with java NCDrill . This will create files with a _t01.plt, _t02.plt etc. suffix (one for each tool from your drill configuration file).


File Preview Stage

GC-PREVUE is your friend! This tool will let you visualize your .plt files and make sure you'll be manufacturing what you want.

  1. Load Engraver PLT File. Use GC-PREVUE's File:Import (not File Open). Choose HPGL as the file type in the pop-up window; the software will otherwise mis-recognize the file type.

  2. Load the Drill Hit PLT File(s) with the same method. These files should be recognized properly by GC-PREVUE.

  3. Make sure the drill files and the engraving file are superimposed properly.

  4. See directions below for determining offset of your design from the XY = 0,0 origin.


Manufacturing Stage