This section will explain how to translate your PCB design into a format that the ProtoMat can understand. In the following example, Eagle was used to design the PCB, but there are several other design programs that can generate the necessary files for in-house PCB fabrication.

Understanding Gerber and Excellon Files

Gerber and Excellon files are commonly used to compactly convey geometric information to milling machines like the ProtoMat. Most PCB design suites have a feature that can generate Gerber and Excellon files from specified layers of a PCB layout. To produce a double-sided circuit board, all of the files shown in Table 3.1 should be generated.

Table 3.1: Example Set of Gerber and Excellon Files.
Replace [Name] with the name of your PCB project.

There are many other acceptable file configurations available, but these files are used in the following example because of their consistent results and simple compatibility. Newer formats such as Gerber X2 might work and will require experimentation.

Producing Gerber and Excellon Files in Eagle

In Figure 3.1, an Eagle .brd file (board file) is shown. Before attempting to produce the Gerber and Excellon files, double check your board to ensure that there are no errors and that it is possible for the ProtoMat to create it. The clearance between traces and pads should be at least 0.1 mm (4 mils), and the smallest hole should have a diameter of at least 0.4 mm (16 mils).

Figure 3.1: Board File with Different Layers
Red is the top layer, blue is the bottom layer, green represents the pads and via layers, and grey represents the board outline. The drill and holes layers are not shown.

To generate the Gerber and Excellon files, select File -> CAM Processor from the Board editor window in Eagle. This opens the window shown in Figure 3.2. The Computer-aided Manufacturing (CAM) Processor can be used to assign layers of your Eagle .brd file with CAM sections. A CAM section can be processed to produce Gerber or Excellon files. A collection of sections is referred to as a CAM job.

Figure 3.2: New CAM Processor Window

To generate files for the board shown in Figure 3.1, four sections should be added to the current job. The Add button will add a section to the current job so it can be assigned layers and an output format.

The first section arbitrarily named “Top” will produce the %N.cmp Gerber file (%N automatically substitutes the name of the Eagle project). This section should be configured as shown in Figure 3.3.

Figure 3.3: Top Section Configuration
Note that only the top layer, pads layer, and vias layer are selected.

The second section shown in Figure 3.4 may be named “Bottom” and will produce the %N.sol Gerber file.

Figure 3.4: Top Section Configuration
Note that only the top layer, pads layer, and vias layer are selected.

The third section shown in Figure 3.5 may be named “Outline” and will produce the %N.gml Gerber file.

Figure 3.5: Outline Section Configuration
Any layer in the board design that makes a closed polygon can be used. In this example, the board outline layer was named “TotalOutline”.

The fourth section shown in Figure 3.6 may be named “Drills” and will produce the %N.txt and the %N.dri Excellon files.

Figure 3.6: Drills Section Configuration
The Drills and Holes layers are used. Note that the device (output format) is EXCELLON and the filename extension is .txt

When all of the sections are configured, clicking the Process Job button will process all of the sections so that the .cmp, .sol, and .gml files all reference the same aperture list file (.gpi) file. The files should appear in your project folder and are ready to be sent to the computer attached to the ProtoMat via .zip file.