Contact Information

• Primary Authors:
  Thomas Nau
  Harry Eaton
• PCB Website
• PCB Unix V1.6.3 (FTP)
  German FTP Mirror
• Mailing List
• Questions and Comments

• General Information
• Using PCB
• Printing and Saving Files
• Drill Sizing Tips
• Generating Files
• APCircuits Requirements
• Acknowledgements

PCB Unix is free software under the GNU General Public License (GPL). PCB has proven to be a solid and reliable package for simple board design, and the output formats it produces are compatible with APCircuits equipment.

PCB will run under a variety of UNIX variants using the X window system. The FreeBSD Unix variant has PCB Unix as a package/port for easy installation; this software will also work with the Linux Unix-like operating system.

Using PCB

This is the PCB main work screen.  The program supports 8 layers which can be treated as individual layers (for multi-layer boards) or grouped together for easier tracking of power and ground traces (shown here). The display supports several fixed zoom levels, such as 1:1, 2:1, 4:1, etc.  Fixed zooming ensures best accuracy between the display and the finished product, as well as speeding up display redraw.
There is a small prefab library of parts, and new part files can be created by drawing and cutting, or by editing a text macro file.  Cut and paste to multiple buffers eases layout manipulations, and multilevel undo/redo helps keep the human error factor to a minimum. Lines can be moved as individual components, or in a rubber-band mode, and can be drawn using three different automatic 45-degree placement methods. Design-rule checking is available, as is netlist comparison and rat's nest layout, features which allow you to take a schematic drawn in a circuit editing program and use the connection information stored there to greatly ease the layout of your board.

In the style of modern graphic design packages, the most used commands are available in drop-down menus, however many of the program's functions are reachable only through keystroke commands - for example, to move a trace on the board into the working layer from some other layer, point to it and press m - the segment changes layer, and vias are automatically added as necessary to keep it connected to any other traces it touches. A printable manual is supplied with the system, and it's a good idea to print one out. The layout can be printed to postscript files, encapsulated postscript, or to Gerber/RS-274X files (compatible with AP Circuits' equipment).

Printing and Saving Files

The File drop down menu allows loading and saving of a complete layout, loading of layouts or components into a paste buffer, and printing. To generate a file for PC board manufacture, select print layout from this menu. All printing is done to disk files as individual layers, which can then be sent to the printer as needed from the command line or a visual tool such as Midnight Commander.

After selecting print layout, a settings pop-up box appears. To generate postscript output for printing, select the PostScript device driver. To generate Gerber files for PC board manufacture, select the Gerber / RS-274X device driver (as shown). For easiest handling by AP Circuits, select the box labeled DOS (8.3) names. Choose OK to generate the files.

Project files are saved in a text format, and can be edited with any text editor - as a bonus, a separate save process runs in the background to handle writing layout data to disk.

Drill Sizing Tips

One point of confusion for me was that APC's free drill sizes are listed as the actual size the holes are drilled, referred to as unfinished or before plating. PCB, the program, specifies it’s hole sizes as finished holes or after plating. There are 3 ways of handling this difference:

1. Change the hole sizes to drill bit sizes as you are drawing the board
2. Change the header of the NC Drill file after the layout is plotted.
3. Create a READ.ME file when sending in your order with the phrase 'All holes are specified as FINISHED SIZE'; APC will adjust them accordingly.

Hole Size Drill Bit Size

• <= .023  .028
• .024 - .030 .035
• .031 - .037 .042
• .038 - .047 .052
• .048 - .055 .060
• .056 - .081 .086
• .082 - .120 .125
• .121 - .147 .152

Before submitting a design, run apcdrill.pl dril.gbx from a shell to change the drill sizes to free sizes.  This will also generate the tool.tbl file which AP Circuits requests be included with your order. The script is available from the PCB website, directly from APC’s site,or at  www.howman.com/files/PCB/apctools.zip If there are drill sizes you specifically need to preserve, the format of the drill.gbx file header is very simple, and is easy enough to change with any text editor.

The libraries provided with PCB do not necessarily use APCircuits' free drill sizes, nor are these sizes particularly easy to select from the PCB drop down menus.  The easiest way to handle this is to use the global change command (available by keyboard entry only) to change all .025 holes to .028, all .040 holes to .042, etc. You can also modify the components in the library (trivial using any text editor) so that when you use them next time, they already use free drill sizes. When placing vias, free drill sizes can be selected in advance with keyboard commands rather than using the default sizes from the drop-down menus, which are in multiples of 5 mils. Before submitting a design, select Report from the menu, and generate a drill report.  Make sure that all drills are free sizes whenever possible, to minimize the cost of your completed boards.

Generating Files

To generate Gerber/NC Drill files for submitting to AP Circuits, use the print layout command - all printing is done to disk files rather than going directly to a printer, so you print the layout in the Gerber format and then send the resulting files to AP Circuits.

After selecting print layout, a settings pop-up box appears. To generate postscript output for printing, select the PostScript device driver. To generate Gerber files for PC board manufacture, select the Gerber / RS-274X device driver (as shown). For easiest handling by AP Circuits, select the box labeled DOS (8.3) names.  Choose OK to generate the files. The results will be a series of files, all with a .gbx extension.

The layer plot files will be numbered starting at 1.gbx, going up to 8.gbx if no layers are grouped together.  In this example, the first three layers (solder, GND-sldr, Vcc-sldr) were grouped together, and they would appear in 1.gbx.  The next three layers (component, GND-comp, Vcc-comp) were also grouped together, and they appeared in 2.gbx.  The two layers named unused appeared in 3.gbx and 4.gbx.

The solder mask files are called smsk.gbx and cmsk.gbx, for solder and component side respectively.  Similarly, the silk screen files are named sslk.gbx and cslk.gbx for solder and component side silk screens.

The CNC drill file (it is the proper type of file, even though it has the confusing .gbx extension instead of a .CNC) is dril.gbx.

For clarity, rename 1.gbx to solder.gbx and 2.gbx to compont.gbx, and delete unused layer files. Remember, the printouts go by layer GROUP, not by layer.  If you are unsure, print out a set of postscript files first, and either print them to paper or view them with ghostview (gv 1.ps from a shell) or another postscript viewer. If using PROTO 1 service (no solder mask or silk screen) you can also delete the  ?msk.gbx and ?slk.gbx files.

APCircuits Requirements

APCircuits order forms request two extra files - a tool table and an aperture table. As mentioned above, running apcdrill.pl automatically creates the tool.tbl file. Also included in the apctools.zip file is a script called apcaperture.pl - running it on one of the layer files (1.gbx or solder.gbx) will produce aperture.tbl in the preferred APCircuits format.

The GBX Gerber format that PCB creates is known as RS274-X and does not require the traditional companion aperture file. On the offhand chance that a definition in the 274-X data is not part of the traditional shape list, the aperture file, if provided, is a quick reference for shape identification. Similarly, the drill.gbx file has the drill sizes embedded in the file header, this eliminates the need for the companion NC Tool List.

APCircuits requires that files be sent in a .ZIP type archive. The GPL tool zip will generate MS-DOS compatible archives - this program is included in all common Linux distributions, and is available for other Unix systems.

You will also need to download a copy of the order form to include in the .ZIP file. Use any text editor to fill in the required information on the form.

Use the command zip -jkz project.zip *.gbx order.frm READ.ME to produce an MS-DOS compatible archive file containing the .gbx files, your completed order form, and the READ.ME file. This archive file can then be sent to APC via FTP or email.

Acknowledgements

APCircuits thanks Phil Salkie for his suggestions and guidance in the construction of this section. Since the creation, a number of excellent suggestions and recommendations have been added. In the interests of continuity we would like to suggest that fellow contributors pass the information over to Phil for editing.