Pcb

Table of Contents

Pcb

This document is a manual for Pcb, the open source, interactive printed circuit board layout system.

History

Pcb is a handy tool for laying out printed circuit boards.

Pcb was first written by Thomas Nau for an Atari ST in 1990 and ported to UNIX and X11 in 1994. It was not intended as a professional layout system, but as a tool which supports people who do some home-developing of hardware.

The second release 1.2 included menus for the first time. This made Pcb easier to use and thus a more important tool.

Release 1.3 introduced undo for highly-destructive commands, more straightforward action handling and scalable fonts. Layer-groups were introduced to group signal-layers together.

Release 1.4 provided support for add-on device drivers. Two layers (the solder and the component side) were added to support SMD elements. The handling of libraries was also improved in 1.4.1. Support for additional devices like GERBER plotters started in 1.4.4. The undo feature was expanded and the redo-feature added in 1.4.5.

harry eaton took over pcb development beginning with Release 1.5, although he contributed some code beginning with Release 1.4.3

Release 1.5 provides support for rats-nest generation from simple net lists. It also allows for automatic clearances around pins that pierce a polygon. A variety of other enhancements including a Gerber RS-274X driver and NC drill file generation have also been added.

Release 1.6 provides automatic screen updates of changed regions. This should eliminate most of the need for the redraw (R key). Also some changes to what order items under the cursor are selected were made for better consistency - it is no longer possible to accidentally move a line or line point that is completely obscured by a polygon laying over top of it. Larger objects on the upper most layers can be selected ahead of smaller objects on lower layers. These changes make operations more intuitive. A new mode of line creation was added that creates two line on 45 degree angles with a single click. The actual outline of the prospective line(s) are now shown during line creation. An arc creation mode was added. Drawn arcs are quarter circles and can be useful for high frequency controlled impedance lines. (You can have eighth circle arc if the source is compiled with -DARC45, but be aware that the ends of such arcs can never intersect a grid point). Two new flags for pins and vias were created - one indicates that the pin or via is purely a drill hole and has no copper annulus. You can only toggle this flag for vias - for elements, it must be an integral part of the element definition. The other flag controls whether the pad will be round or octagonal. There is also now a feature for converting the contents of a buffer into an element.

Release 1.6.1 added the ability to make groups of action commands bound to a single X11 event to be undone by a single undo. Also a simple design rule checker was added - it checks for minimum spacing and overlap rules. Plus many fixes for bugs introduced with the many changes of 1.6

Release 1.7 added support for routing tracks through polygons without touching them. It also added support for unplated drill files, and drawing directly on the silk layer. A Netlist window for easily working with netlist was also added.

Release 2.0 adds an auto-router, a new simpler library mechanism, much improved support for graphically creating (and editing) elements, viewable solder-mask layers (and editing), snap to pins and pads, netlist entry by drawing rats, element files (and libraries) that can contain whole sub-layouts, metric grids, improved user interface, a GNU autoconf/automake based build system, and a host of other improvements.

Release 4.0.0 adds a IPC-D-356 netlister, relocate plugin, smartdisperse plugin, RenumberBlock and RenumberBuffer plugin, teardrops plugin, tooltips in the GTK UI and footprints.

Release 4.0.1 fixes a number of bugs.

Release 4.0.2 fixes a number of bugs.

Release 4.1.0 is a new features release (pcb file format change).

Release 4.1.1 fixes a number of bugs.

Release 4.1.2 fixes a number of bugs.

Release 4.1.3 fixes a number of bugs.

Release 4.2.0 is a new features release (pcb file format change).

Release 4.2.1 is a new features and bugfixes release (no pcb file format change).

Release 4.2.2 is a hot fix and bugfixes release (no pcb file format change).

Release 4.3.0 is a new features release (pcb footprint file format change).

Special thanks goes to:

Thomas Nau (who started the project and wrote the early versions).
C. Scott Ananian (who wrote the auto-router code).
Bernhard Daeubler (Bernhard.Daeubler@physik.uni-ulm.de)
Harald Daeubler (Harald.Daeubler@physik.uni-ulm.de)
DJ Delorie (djdelorie@users.sourceforge.net)
Larry Doolittle (ldoolitt@recycle.lbl.gov)
Dan McMahill (danmc@users.sourceforge.net)
Roland Merk (merk@faw.uni-ulm.de)
Erland Unruh (Erland.Unruh@malmo.trab.se)
Albert John FitzPatrick III (ajf_nylorac@acm.org)
Boerge Strand (borges@ifi.uio.no)
Andre M. Hedrick (hedrick@Astro.Dyer.Vanderbilt.Edu)
Anthony Blake (who wrote the toporouter code).

PCB Contributors:
Peter Clifton, Andrew Poelstra, Markus Hitter, Ben Jackson, Felix Ruoff,
Sergey Alyoshin, Dima Kogan, Jerome Marchand, Jean Richard, Bob Paddock,
Milan Prochac, Britton Leo Kerin, Roland Lutz, Charles Parker,
Jared Casper, Stuart Brorson, Ahmed El-Mahmoudy, Josef Wolf,
Krzysztof Kościuszkiewicz, Mike Crowe, Andrew Armenia, Jan Damborsky,
Wiley E. Hill, Sergey Stepanov, Vladimir Zhbanov, Peter Brett,
Steven Michalske, Leo Bärring, Gareth Edwards, Anton Dubniak,
Kai-Martin Knaak, Keith Packard, Patrick Bernaud, Robert Drehmel,
Erich Heinzle, Marco Ciampa, Eugene Mikhantiev, Jorge Barros de Abreu,
Richard Hughes, Eric Brombaugh, Benjamin Bergman, Braddock Gaskill,
Dan White, Alan Somers, Richard Barlow, Bdale Garbee, Stanislav Brabec,
Levente Kovacs, Ed Maste, Uwe Hermann, Ivan Stankovic, Peter S. May,
Igor2, Felix K (kuhlix), rosvall, Martin, Christian Amsüss,
Johann Klammer, Newell Jensen, Rob Spanton, Bert Timmerman.

who provided all sorts of help including porting Pcb to several operating systems and platforms, bug fixes, library enhancement, user interface suggestions and more. In addition to these people, many others donated time for bug-fixing and other important work. Some of them can be identified in the source code files. Thanks to all of them. If you feel left out of this list, I apologize; please send me an e-mail and I’ll try to correct the omission.

1 Overview

Pcb is an open source printed circuit board editor. Pcb includes many professional features such as:

• Up to 16 copper layer designs by default. By changing a compile time setting, this can be set as high as needed.
• Blind and Buried Vias
• RS-274X (Gerber) output
• NC Drill output
• Centroid (X-Y) data output
• IPC-D-356 (rev. 0) netlist data output
• Postscript and Encapsulated Postscript output
• Nelma numerical analysis package export
• GSvit numerical analysis package export
• Autorouter
• Toporouter
• Trace optimizer
• Rats nest
• Design Rule Checker (DRC)
• Connectivity verification
• Pcb is Free Software
• Can interoperate with free schematic capture tools such as gEDA and xcircuit
• Runs under Linux, NetBSD, Solaris, and other similar operating systems.
• Windows version is available

2 Introduction

Each layout consists of several, mostly independent, objects. This chapter gives an overview of the object types and their relationship to each other. For a complete description of how to use Pcb, refer to Getting Started. The layout is generated on-screen on a grid that can have its origin at any desired location. The X coordinate increases to the right, Y increases down to the bottom. All distances and sizes in Pcb are measured in mils (0.001 inch). One unit on the coordinate display is one mil in distance on the board. The grid may be set on a metric pitch, but is only correct to within the nearest +/- 0.01 mil because Pcb stores all dimensions as integer multiples of 1/100 of a mil or 0.00001 inch.

The sections in this chapter are sorted by the order of appearance of the objects within a layout file.

2.1 Header

The top object is the layout itself. It has a header with settings and layout values. Settings and layout values include the ‘release’ number, ‘FileVersion’, ‘PCB’ name, ‘PCB’ layout main dimensions, ‘Grid’ settings, ‘PolyArea’ setting, ‘Thermal’ setting, ‘DRC’ settings, ‘Flags’, ‘Groups’ layer stack, and routing ‘Styles’

2.2 Symbols

The layout uses a set of symbols that resides at the first logical level. Each symbol is uniquely identified by a seven bit ASCII code. All layout objects share the same set of symbols. These symbols are used to form text objects on the silkscreen and copper layers. Undefined symbols are drawn as filled rectangles.

Every font file is preprocessed by a user-defined command when it is loaded. For details see ‘fontCommand’, Resources.

2.3 Vias

Vias provide through-hole connectivity across all layers. While vias look a lot like element pins, don’t use vias for adding elements to the layout, even if that seems easier than creating a new element. The default solder-mask will cover over vias, so you won’t be able to solder to them. Of course, you can change this so that vias also have solder-mask cut-outs, but it is not the default. Vias are also useful for defining arbitrary drill points such as those used for mounting a board. Vias used in this way have a special flag set so that they have no annular copper ring, and also appear in the unplated drill file. Ctrl-H key over a via switches it between being a pure-mounting hole and a regular via. You can assign a name to a via, which is useful during the creation of new element definitions.

Blind and buried vias are supported. Blind and buried vias exist only on specified layer range. The first and last layer can be assigned using appropriate action, menu item or keys: Ctrl-Shift-F to set active layer as first layer, Ctrl-Shift-T to set last layer and Ctrl-Shift-P to convert via to through-hole.

Blind and buried vias have colored half-circles drawn on top to designate first and last layer..

2.4 Elements

Elements represent the components on a board. Elements are loaded from ASCII coded files in a similar manner to the layout file itself, or from the library selector window. An element is composed of lines and arcs on the silk-screen layer (used to define the package outline), pins (or pads for SMD) and three labels that define the description, the element’s layout-name (which also appears on the silk-screen layer) and its value. You can choose which of the names are displayed on the screen with the Screen menu; however, the silk screen in the printout will always show the layout-name. Element pins are contained on the first logical level and so reside on all layers, but the pads of surface-mount elements reside on only the component or solder layers. An element can have a mixture of pins, pads (on one or both sides), and mounting holes.

A mark is used to position the element with respect to the cross hair during pasting. The mark will lie on a grid point when the element is positioned. The mark is drawn as a small diamond shape, but is only visible when both the silk and pins/pads layers are visible. All parts of an element are treated as one unit, except for the name. It is not possible to delete a single pin or move only part of an element on the layout. You can resize separate pieces of an element, but doing so is usually a bad idea. You can move/rotate the element name independently of the element it belongs to. When you move an element name, a line is draw from the cursor to the element mark so it is easy to tell which element the name belongs to.

Each pin and pad has two string identifiers, one is the "name" which is a functional description of the pin (e.g. "clock in") and the other is the "number" of the pin which is used to identify it in a netlist. The "number" is usually an integer, but it can be any string. You can edit the "name" of each pin of an element, but the "number" is embedded in the element definition and is determined when the new element is first created. Pads are similar to lines on a layer but they must be oriented either vertically or horizontally. Pads can have either rounded or square ends. Pins can be round, square, or octagonal.

Elements are supported by several special layers: silk, pins/pads and far-side. The silk layer shows the package outline and also holds legend text and element names. The pins/pads layer is used to toggle whether the element’s pins and pads are displayed. The far-side layer controls visibility of objects (silkscreen and pads) that are on the far (i.e. not currently viewed) side of the board.

The “oldlib” style of footprint libraries distributed with Pcb rely upon the M4 macro processor. M4 is typically installed under the name m4 on most unix-like operating systems. It is recommended that you use the GNU version of M4 to avoid limitations found in some vendor implementations. See the m4 man page on your system for more information. Every element file is preprocessed by a user-defined command when the file is read. For details see ‘elementCommand’, Resources. m4, the default value of ‘elementCommand’, allows you to create libraries for package definitions that are shared by all elements. The old element libraries distributed with Pcb expect m4 or an equivalent to be the elementCommand. The new library scheme simply has each element stored in a self-contained file, so there is no need to learn m4 to add to the libraries.

Pcb can create a list of all connections from one (or all) elements to the others or a list of unconnected pins. It can also verify the layout connections against a netlist file. The element’s ‘layout-name’ is the name used to identify the element in a netlist file (see Netlist File).

The old libraries, or very old (pre-1.6) layout files may have incorrect pin numbering since there was no concept of pin numbers when they were created. Pcb uses the order of appearance of the pin definitions in the layout or library file if it uses the old format, but there is no guarantee that it will be correct for these old objects.

Be aware that a few of the old library parts may still be incorrectly implemented regarding pin-numbering. All of the DIL (Dual- Inline-Pins) parts are correct and most of the others are too, but you should verify the pin numbering of any non-DIL part before using an old library part. (use the ‘generate object report’ in the Info menu to see what Pcb thinks a pin’s number is) All of the old library names begin with a ~, so you can easily identify them. The old libraries also may contain other sorts of errors, including incorrect pin spacing, silkscreen overlapping solder areas, etc. Check carefully any element in the old library before using it! As the new library grows, the old library will be pared down to at least remove all of the elements with errors, but this will take time.

You can make your own element definitions graphically now. Simply draw vias for the pins, lines on the solder and/or component layers for surface-mount pads (they must be either horizontal or vertical), and lines and arcs on the silkscreen layer for the silkscreen outline. You should name (N key) each via and copper line with the pin number. Once you are happy with the geometry, select everything that is to become part of the element, then choose ‘convert selection to element’ from the Select menu. Afterwords you can make pin (or pad) one square if you like, and give the element its various names. You can also give the pins and pads their functional names. Note that the element mark corresponds to the position you click after choosing the conversion from the menu, so decide where the mark goes and make sure it falls on a grid point before you request the conversion. If the vias/lines are not named, then the pin numbering will correspond to the order in which they were placed.

When you create a new element, remember that silkscreen lines should never overlap the copper part of the pins or pads, as this can interfere with soldering. The silkscreen should identify the maximum extent of the element package so it is easy to see how close elements can be placed together.

If you want to make an element similar to an existing one, you can break an element into constituent pieces from the Buffer menu. Paste the pieces to the layout, make the necessary changes, then convert it back into an element. If the pin numbers haven’t changed, there is no need to name each via/line as they are pre-named when the element was broken apart. When you create a new element, you can save it to a file in order to have easy access to it the next time you run Pcb.

2.5 Layers

Every layout consists of several layers that can be used independently or treated as a group. Layer groups can be used to logically separate (and color-code) different traces (e.g. power and signal); however, all layers within a group reside on the same physical copper layer of a board, so using different layers within the same group won’t provide electrical separation where they touch or overlap. For details, see ‘layerGroups’, Resources. Each layer is drawn in a color defined in the resource file and identified by a name that you can change (for details see ‘layerColor’, Resources.) Layers are really just containers for line, arc, polygon, and text objects. The component and solder layers contain SMD elements as well, but the file structure doesn’t reflect that fact directly.

Each layer group represents a physical layer on the printed circuit board. If you want to make a four layer board, you’ll need to have at least four layer groups. Connections between layer groups are established only through element pins and vias. The relationship between a specific layer and the board itself is configurable from the ‘Edit layer groups’ option in the Settings menu. The layer groups corresponding to the physical layers: component-side and solder-side are always defined and you must map at least one logical layer to each, even if you plan to make a single-sided board. You are not obligated to put tracks on either of them. Surface mount elements always reside on either the component-side or the solder-side layer group. When you paste an element from the buffer, it will go onto whichever side of the board you are viewing. You can swap which side of the board you are viewing by pressing the Tab key, or by selecting ‘view solder side’ from the Screen menu. The layer groups just have a name or number associated with them - where they are sandwiched in the board is left for you to tell the manufacturer.

The silkscreen layer is special because there are actually two silkscreen layers, one for the top (component) and one for the bottom (solder) side of the board. Which silk layer you draw on is determined by the side of the board that you are viewing. If you are viewing the component side, then drawing on the silk layer draws to the component-side silk layer.

The netlist layer is another special layer. It shows rat’s-nest lines (i.e. guides that show how the netlist expects the element to interconnect). If you make this the active layer, you can use the Line tool to add entries into the netlist, or to delete connections from the netlist window. Except for these two purposes, you should not make the netlist layer the active layer. Usually there is no need to do this because a separate schematic package should be used to create the netlist. Pcb can automatically draw all of the rats from the netlist. In some cases you may want to make a small change without going to the trouble of modifying the schematic, which is why this facility is provided.

2.6 Lines

Lines are used to draw tracks on the pc board. When in the line mode, each Btn1 press establishes one end of a line. Once the second point is defined, the line is drawn and a new line started where the first one ended. You can abandon the new starting point in favor of another by pressing Ctrl-Btn1, or Btn3, but don’t use Btn2. The undo function (U key or ‘Undo’ from the Edit menu) will take you back point by point if you use it while in the line mode.

New lines can be restricted to 45 degree angles if desired. You can toggle this restriction on and off while creating lines by pressing the period key. If the 45 degree restriction is turned on, then the / (forward slash) key can be used to cycle through three different modes of 45 degree line creation. One mode just creates a single line forced to the nearest 45 degree vector. The next mode creates two lines from the start to end points such that the first line leaves the start point at a 90 degree vector, and the second line enters the end point on a 45 degree vector. The last mode creates two lines such that the first line leaves the start point on a 45 degree vector and arrives at the end point on a 90 degree vector. You can temporarily swap between the last two modes by holding the Shift key down.

It is simple to edit a line object by breaking it into pieces (insert point mode), moving an end point or the whole line (Arrow tool), or changing the layer it resides on (M key moves the line under the pointer to the active layer). In the case when two line segments meet at exactly the same point you can delete the intermediate point, otherwise the delete tool removes an entire line. Feel free to experiment since Pcb will allow you to undo and redo anything that materially affects your work. If you switch active layers in the midst of placing lines a via will automatically be placed, when necessary, in order to continue the connection. The via can be through-hole via or buried/blind via; the via type is controlled by option Auto buried vias.

If you draw a line inside a polygon, it will either plow through the polygon creating a clearance, or touch the polygon. This behavior is selectable in the Settings menu for new lines. To change the behavior of an existing line, hit the J key with the cross hair over the line. You can increase the size of the clearance by 2 mils on each edge with the K key. Shift-K will decrease the clearance by 2 mils. The increment may be changed from 2 mils through the application resource file. The clearance can be also increased, decreased and set by the ChangeClearSize action.

Lines do not need to intersect the center of a pin, pad, via, or other line for Pcb to understand that they make electrical connection. If the connection is too tenuous, running the design rule checker will report that the connection may break if the line width shrinks slightly.

2.7 Arcs

Pcb can handle arcs of any angular extent, but when you create an arc with the Arc tool, it will be a quarter circle (this means they always bend a right angle). Arcs are very similar to lines otherwise. They are created on the active layer and have the same thickness that new lines will have. The various clicks for creating lines work pretty much the same way for creating arcs. In order to make the arc curve in the desired direction, drag the mouse along the tangent line from the starting position towards the end position. If the grid is too coarse, it may not be possible to distinguish whether you’ve moved over then up, or up then over, so if you can’t seem to make the arc go in the direction you want, try pressing the Shift key while drawing the arc. Decreasing the grid spacing may also help. Alternatively you can draw the wrong arc, then rotate and move it where you want. Like the Line tool, after an arc is drawn a new starting point is established at the end point.

Whenever a starting point is established by either the Line or Arc tools it will be retained if you switch directly between the tools (e.g. F2 key for Lines, F8 key for Arcs). Arcs can either touch or clear polygons just like lines do. Of course connection searches, undo and all the other features you’d expect work with arcs too.

2.8 Polygons

Sometimes it’s useful to fill large areas with solid copper. The way to do this is with polygons. Polygons can be created in either the polygon mode or the rectangle mode. In the polygon mode, you’ll have to define each corner of the polygon with a mouse click (Btn1). When the last point is clicked exactly on top of the starting point, the polygon is finished. Since this can be hard to do, the Shift-P key will enter the final point for you, closing the polygon. If the 45 degree angle restriction is turned on and you try to close the polygon when it is not possible, you’ll get a warning instead. If you haven’t finished entering a polygon, but want to undo one (or more) of the points that you’ve already defined, use the undo command (U key).

With the rectangle tool, defining the two diagonally opposite corners is sufficient, but of course the resulting polygon is a rectangle. Like lines, a polygon can by edited by deleting, inserting and moving the points that define it. Pins and vias always clear through polygons without touching them when first positioned. You must add a thermal with the thermal tool in order to connect pins and vias to polygons. Thermals can be added and removed by clicking Btn1 with the thermal tool over the pin or via. The thermal tool always places a thermal to polygons on the active layer, so if the tool doesn’t seem to work, it’s probably because the polygon you want to touch is not on the active layer. You can change the style of thermal used or make a solid connection by holding down Shift while clicking Btn1 with the thermal tool over the pin or via.

Pcb is capable of handling complex polygons, but using a number of simpler ones improves performance of the connection tracing code. You also must be careful not to create polygons that touch or overlap themselves. The fabricated board may not look the way you expect if you violate this principle. It is always ok to have two (or more) polygons touch or overlap each other, but not for points within the same polygon to do so.

The great advantage to this new polygon behavior is that simple or complex ground and/or power planes can be easily made with polygons and seen on the screen. If you don’t want this auto-clearance behavior, or you load a layout created by an early version of Pcb, the old behavior (shorts to all piercing pins and vias) is available. A ‘ChangeSize’ operation (S key) toggles a polygon between the new and old polygon/pin behavior.

2.9 Text

Text objects should be used to label a layout or to put additional information on the board. Elements have their ‘layout-name’ labels on the silk-screen layer. If you are making a board without a silkscreen, you can use copper text to label the elements, but you have to do this manually.

Text is always horizontal when first created, but the rotate mode can align it along 0, 90, 180 and 270 degree angles. Text on the far side of the board will automatically appear mirror-imaged.

Warning: TEXT OBJECTS ON A COPPER LAYER CREATE COPPER LINES BUT THEY ARE NOT SCANNED FOR CONNECTIONS OR TESTED FOR CREATING SHORTS VS. THE NETLIST. NEITHER ARE TEXT OBJECTS TESTED AGAINST ANY DESIGN RULES.

2.10 Nets

Layout files also contain the netlist that describes how the elements are supposed to be interconnected. This list of connections can be loaded from a netlist file (see Netlist File), or entered by drawing rat-lines as described previously. Each net has a name and routing style associated with it. The net contains a list of all element layout-name names and pin numbers that should be connected to the net. Loading a netlist file will replace all existing nets with the ones from the file. The Netlist window provides an easy way to browse through the net list. You can display the rat’s-nest by selecting ‘optimize rats-nest’ from the Connects menu. If you move or rotate elements, the rat’s-nest will automatically follow the movements, but they won’t necessarily show the shortest paths until you optimize them again.

3 Getting Started

The goal of this chapter is to give you enough information to learn how Pcb works and how to develop your layouts to make the best use of Pcb’s features. All event translations (i.e. the buttons and keys you press) refer to the default application resource file shipped with Pcb. There is probably no need to change this unless your window manager uses some of the button events itself; however, if you want to customize the behavior of Pcb then changing the resource file is usually the best way to do it.

Get yourself a printout of this chapter and User Commands, if you haven’t already done so, and follow the examples.

Start Pcb (the actual command will use all lower-case letters) without any additional options. If you get the error message:

    can’t find default font-symbol-file ’default_font’

then the font searchpath or filename in the application resource file is wrong. Be sure that your m4 program supports search paths. If not, get GNU m4. For other messages, see Trouble Shooting. Another quick-start is provided by pcbtest.sh in the src directory. If some features don’t seem to work, try running pcbtest.sh, if that works, then Pcb hasn’t been installed properly.

3.1 The Application Window

The main window consists of five areas: the menu at the top, the layer control in the upper left, the tool buttons located below the layer controls, the Layout area to the right of these, and the status line at the bottom of the window.

3.1.1 Menus

The menus are located at the top of the Layout area. Most, but not all, of their functions are also available from the keyboard. Similarly, some functions are only achievable through the keyboard or command entry. Some menu entries such as ‘center layout’ in the Screen menu require a certain cross hair position. In this case a prompt message will popup at the bottom of the screen with wording similar to the following:

move pointer to the appropriate screen position and press a button

Any mouse button will do the job, whereas any key except the arrow (cursor) keys will cancel the operation. If it seems like the menu hasn’t done what you expected, check to see if it is waiting for the position click. For details see Actions.

Pressing Btn3 in the Layout area also pops up a menu with many of the most common operations (except when you’re in the midst of drawing a line or arc). When a choice in the Btn3 popup menu needs a cross hair position, it uses the position where the cross hair was when Btn3 was pressed. For example, to get detailed information on an object, place the cross hair over the object, press Btn3, then choose ‘object report’. If you pop up the Btn3 menu but don’t want to take any of the actions, click on one of the headers in the menu.

File

This menu offers a choice of loading, saving and printing data, saving connection information to a file or quitting the application. Most of the entries in the File menu are self explanatory. Selecting ‘Print...’ pops up a printer control dialog. Several output formats are available from the ‘Export...’ menu item. Presently PostScript, encapsulated PostScript, and GerberX are some of the supported filetypes. The GerberX driver produces all of the files necessary to have the board professionally manufactured. The connection saving features in the File menu produce outputs in an arcane format that is not too useful. They do not produce netlist files.

Edit

The Edit menu provides the usual cut, copy, paste which work on selections. To learn how to create complex selections, see Arrow Tool. The Edit menu also provides access to Undo and Redo of the last operation. These can also be accomplished with the U key and Shift-R key. Finally, the Edit menu allows you to change the names of: the layout, the active layer, or text objects on the layout.

Routes Style

The Edit menu allows you to select a group of line thickness, via diameter, via drill size, and clearance (keepaway) (collectively called a "routing style") to be copied to the "active" sizes. You can also change the names given to the routing styles and adjust their values from this menu. The "active" sizes are also adjustable from this menu. The "active" sizes are shown in the status-line and control the initial size of new vias, drilling holes, lines, clearances, text-objects and also the maximum dimensions of the board layout.

View

The View menu supports most functions related to the whole Layout area. There are various entries to change the grid to some popular values, the zoom factor, and which kind of element name is displayed. You can also re-align the grid origin and turn on and off the display of the grid. Before changing the grid alignment, I recommend that you zoom in as close as possible so that you’re sure the grid points appear exactly where you want them.

The View menu also allows you to turn on and off the visibility of the solder-mask layer. When the solder-mask layer is made visible it obscures most of the layout, so only turn this on when you really want to know what the solder-mask will look like. The solder-mask that you see belongs to the side of the board you are viewing, which can be changed with the ‘Flip up/down’ option, also found in the View menu. When the solder-mask is displayed, the pin and pad clearance adjustments (see Line Objects) alter the size of mask cut-outs.

Settings

The Settings menu controls several operating configuration parameters. The ‘all-direction lines’ entry controls the clipping of lines to 45-degree angles. You can also control whether moving individual objects causes the attached lines to "rubber band" with the move or not from the Settings menu. Another entry controls whether the starting clip angle for the two-line mode (see Line Objects) alternates every other line. You can also control whether element names must be unique from the Settings menu. When unique element names are enforced, copying a new element will automatically create a unique ‘layout-name’ name for it provided that the name originally ended with a digit (e.g. U7 or R6). The Settings menu allows you to control whether the cross hair will snap to pins and pads even when they are off-grid. Finally you can control whether new lines and arcs touch or clear intersecting polygons from this menu.

Select

This menu covers most of the operations that work with selected objects. You may either (un)select all visible objects on a layout or only the ones which have been found by the last connection scan see . You can delete all selected objects from this menu. Other entries in the Select menu change the sizes of selected objects. Note that a select action only affects those objects that are selected and have their visibility turned on in the Layer Control panel. The Select menu also provides a means for selecting objects by name using unix Regular Expressions.

Buffer

From the Buffer menu you may select one out of five buffers to use, rotate or clear its contents or save the buffer contents to a file. You can also use the ‘break buffer elements to pieces’ entry to de-compose an element into pieces for editing. Note: only objects with visibility turned on are pasted to the layout. If you have something in a buffer, then change which side of the board you are viewing, the contents of the buffer will automatically be mirrored for pasting on the side you are viewing. It is not necessary to clear a buffer before cutting or copying something into it - it will automatically be cleared first.

Connects

The entries available through the Connects menu allow you to find connections from objects and to manipulate these. You can also optimize or erase rat’s nests from this menu. Finally, the ‘auto-route all rats’ entry allows you to auto-route all connections show by the rat’s nest. The auto-router will use any visible copper layer for routing, so turn off the visibility of any layers you don’t want it to use. The auto-router will automatically understand and avoid any traces that are already on the board, but it is not restricted to the grid. Finally, the auto-router routes using the active sizes (except for nets that have a route-style defined). Pcb always knows which tracks were routed by the auto-router, and you can selectively remove them without fear of changing tracks that you have manually routed with the ‘rip-up all auto-routed tracks’ entry in the Connects menu. The ‘design rule checker’ entry runs a check for copper areas that are too close together, or connections that touch too tenuously for reliable production. The DRC stops when the first problem is encountered so after fixing a problem be sure to run it again until no problems are found.

Warning: COPPER TEXT IS IGNORED BY THE DRC CHECKER.

Info

The ‘generate object report’ entry from the Info menu provides a way to get detailed information about an object, such as its coordinates, dimensions, etc. You can also get a report summarizing all of the drills used on the board with ‘generate drill summary’. Lastly, you can get a list of all pins, pads and vias that were found during a connection search.

Window

The Window menu provides a way to bring each of Pcb's windows to the front. The Library window is used to bring elements from the library into the paste-buffer. The Message Log window holds the various messages that Pcb sends to the user. The Netlist window shows the list of connections desired.

Now that you’re familiar with the various menus, it’s time to try some things out. From the File menu choose ‘Open...’, navigate to the tutorial folder, then load the file ‘tut1.pcb’.

3.1.2 The Status-line and Input-field

The status-line is located at the bottom edge of the main window. During normal operation the status information is visible there. When a selected menu operation requires an additional button click, the status-line is replaced by a message telling you to position the cursor and click. When a text input is required, the status-line is replaced by the Input-field which has a prompt for typing the input.

The status-line shows, from left to right, the side of the board that you are viewing (Tab key changes this), the current grid values, if new lines are restricted to 45 degrees, which type of 45 degree line mode is active, whether rubberband move and rotate mode is on (R), and the zoom factor. This information is followed by the active line-width, via-size and drilling hole, keepaway spacing, and text scaling. Last is the active buffer number and the name of the layout. An asterisk appearing at the far left indicates that the layout has been modified since the last save. Note that the name of the layout is not the same thing as the filename of the layout. Change the grid factor to 1.0 mm from the Screen menu. Observe how the status line shows the new grid setting. Except for the case of the metric grid, all dimensions in the status line are in units of 0.001 inch (1 mil).

The input-field pops up (temporarily replacing the status-line) whenever user input is required. Two keys are bound to the input field: the Escape key aborts the input, Return accepts it. Let’s change the name of a component on the board to see how the input-field works. Position the cross hair over R5, and press the N key. The input field pops-up showing the name for you to edit. Go ahead and change the name, then hit return. Notice the name of the element changed. Now undo the change by pressing the U key. You can position the cross hair over the name, or the element before pressing the N key.

Now select ‘realign grid’ from the Screen menu. Notice that the status line has been replaced with an instruction to position the cursor where you want a grid point to fall. In this case, since the cross hair can only fall on a grid point, you must move the tip of the finger cursor to the place where you want a grid point to appear. Do not worry that the cross hair is not coincident with the cursor. Click Btn1 at your chosen location. See how the grid has shifted, and the status line has returned.

The present cross hair position is displayed in the upper right corner of the window. Normally this position is an absolute coordinate, but you can anchor a marker at the cross hair location by pressing Ctrl-M (try it now) and then the display will read both the absolute cross hair position as well as the difference between it and the marker. The numbers enclosed in < > are the X and Y distances between the cross hair and the mark, while the numbers enclosed in parenthesis are the distance and angle from the mark to the cross hair. The values displayed are always in units of 0.001 inch (1 mil). Pressing Ctrl-M again turns the marker off.

3.1.3 The Layer Controls

The layer control panel, located in the upper left, is used to turn on and off the display of layer groups and to select the active drawing layer. If a layer hasn’t been named, the label "(unknown)" is used as the default. If this happens, it probably means the application resources are not installed properly.

The upper buttons are used to switch layers on and off. Click <Btn1> on one or more of them. Each click toggles the setting. If you turn off the currently active layer, another one that is visible will become active. If there are no others visible, you will not be able to turn off the active layer. When the layers are grouped, clicking on these buttons will toggle the visibility of all layers in the same group. This is a good idea because layers in the same group reside on the same physical layer of the actual board. Notice that this example has 2 groups each having 3 layers, plus two other layers named ‘unused’. Use the ‘Edit layer groups’ option in the ‘Settings’ menu to change the layer groupings in the lesstif GUI or the ‘Preferences’ dialog from the ‘File’ menu in the GTK+ GUI. Note that changing the groupings can radically alter the connectivity on the board. Grouping layers is only useful for helping you to color-code signals in your layout. Note that grouping layers actually reduces the number of different physical layers available for your board, so to make an eight layer board, you cannot group any layers.

The far side button turns on and off the visibility of elements (including SMD pads) on the opposite (to the side you’re viewing) board side, as well as silk screening on that side. It does not hide the x-ray view of the other copper layers, these must be turned off separately if desired. Use the tab key to view the entire board from the other side. To see a view of what the back side of the board will actually look like, make the solder layer the active layer then press tab until the status line says "solder" on the right, then turn off the visibility of all layers except solder, pins/pads, vias, and silk. Now turn them all back on.

The lowest button, named active, is used to change the active drawing layer. Pressing <Btn1> on it pops up a menu to select which layer should be active. Each entry is labeled with the layer’s name and drawn in its color. The active layer is automatically made visible. The active layer is always drawn on top of the other layers, so the ordering of layers on the screen does not generally reflect the ordering of the manufactured board. Only the solder, component, silkscreen, and solder-mask layers are always drawn in their physical order. Bringing the active layer to the top makes it easier to select and change objects on the active layer. Try changing the active layer’s name to ABC by selecting ‘edit name of active layer’ from the ‘Edit’ menu. Changing the active layer can also be done by pressing keys 1..MAX_LAYER.

Turn off the visibility of the component layer. Now make the component layer the active layer. Notice that it automatically became visible. Try setting a few other layers as the active layer. You should also experiment with turning on and off each of the layers to see what happens.

The netlist layer is a special layer for adding connections to the netlist by drawing rat lines. This is not the recommended way to add to the netlist, but occasionally may be convenient. To learn how to use the netlist layer see Net Objects.

3.1.4 The Tool Selectors

The tool selector buttons reside below the layer controls. They are used to select which layout tool to use in the drawing area. Each tool performs its function when Btn1 is pressed. Every tool gives the cursor a unique shape that identifies it. The tool selector buttons themselves are icons that illustrate their function. Each layout tool can also be selected from the keyboard:

    F1 key       Via tool
    F2 key       Line tool
    F3 key       Arc tool
    F4 key       Text tool
    F5 key       Rectangle tool
    F6 key       Polygon tool
    F7 key       Buffer tool
    F8 key       Delete tool
    F9 key       Rotate tool
    Insert key   Insert-point tool
    F10 key      Thermal tool
    F11 key      Arrow tool
    F12 key      Lock tool

Some of the tools are very simple, such as the Via tool. Clicking Btn1 with the Via tool creates a via at the cross hair position. The via will have the diameter and drill sizes that are active, as shown in the status line. The Buffer tool is similar. With it, <Btn1> copies the contents of the active buffer to the layout, but only those parts that reside on visible layers are copied. The Rotate tool allows you to rotate elements, arcs, and text objects 90 degrees counter-clockwise with each click. Holding the Shift key down changes the Rotate tool to clockwise operation. Anything including groups of objects can be rotated inside a buffer using the rotate buffer menu option.

The Line tool is explained in detail in Line Objects. Go read that section if you haven’t already. Activate the Line tool. Set the active layer to the solder layer. Try drawing some lines. Use the U key to undo some of the lines you just created. Zoom in a bit closer with the Z key. Draw some more lines. Be sure to draw some separate lines by starting a new anchor point with Ctrl-Btn1. Change the ‘crosshair snaps to pin/pads’ behavior in the Settings menu. Now draw a line. Notice that the new line points must now always be on a grid point. It might not be able to reach some pins or pads with this setting. Increase the active line thickness by pressing the L key. Note that the status line updates to reflect the new active line thickness. Now draw another line. Before completing the next line, make the component layer active by pressing the 4 key. Now finish the line. Notice that a via was automatically placed where you switched layers. Pcb does not do any checks to make sure that the via could safely be placed there. Neither does it interfere with your desire to place lines haphazardly. It is up to you to place things properly when doing manual routing with the Line tool.

The Arc tool is explained in detail in Arc Objects. Its use is very similar to the Line tool.

The Rectangle tool, Polygon tool and Thermal tool are explained in detail in Polygon Objects. Go read that section. Remember that the Thermal tool will only create and destroy thermals to polygons on the active layer. Use the Rectangle tool to make a small copper plane on the component layer. Now place a via in the middle of the plane. Notice that it does not touch the plane, and they are not electrically connected. Use the Thermal tool to make the via connect to the plane. Thermals allow the via or pin to be heated by a soldering iron without having to heat the entire plane. If solid connections were made to the plane, it could be nearly impossible to solder. Shift-click on the via with the Thermal tool to change the style of thermal used or to make the connection solid. Click on the via again with the Thermal tool to remove the connection to the plane.

The Insert-point tool is an editing tool that allows you to add points into lines and polygons. The Insert-point tool enforces the 45 degree line rule. You can force only the shorter line segment to 45 degrees by holding the Shift key down while inserting the point. Try adding a point into one of the lines you created. Since line clipping is turned on, you may need to move the cross hair quite far from the point where you first clicked on the line. Turn off the line clipping by selecting ‘all-direction lines’ from the Settings menu (or hit the Period key). Now you can place an inserted point anywhere. Try adding a point to the rectangle you made earlier. Start by clicking somewhere along an edge of the rectangle, then move the pointer to a new location and click again.

The delete-mode deletes the object beneath the cursor with each Btn1 click. If you click at an end-point that two lines have in common, it will replace the two lines with a single line spanning the two remaining points. This can be used to delete an "inserted" point in a line, restoring the previous line. Now delete one of the original corner points of the polygon you were just playing with. To do this, place the cross hair over the corner and click on it with the Delete tool. You could also use the Backspace key if some other tool is active. Try deleting some of the lines and intermediate points that you created earlier. Use undo repeatedly to undo all the changes that you’ve made. Use redo a few times to see what happens. Now add a new line. Notice that you can no longer use redo since the layout has changed since the last undo happened. The undo/redo tree is always pruned in this way (i.e. it has a root, but no branches).

The Arrow tool is so important, it has its own section: Arrow Tool. Go read it now.

The Lock tool allows you to lock objects on the layout. When an object is locked, it can’t be selected, moved, rotated, or resized. This is useful for very large objects like ground planes, or board-outlines that are defined as an element. With such large objects, nearly anywhere you click with the Arrow tool will be on the large object, so it could be hard to draw box selections. If you lock an object, the Arrow tool will behave as if it didn’t exist. You cannot unlock an object with undo. You must click on it again with the Lock tool. If an object is locked, previous changes to it cannot be undone either. When you lock an object, a report message about it is popped up and will always tell you what object it is, and that it is locked if you just locked it. Other than noticing your inability to manipulate something, the only way to tell an object is locked is with a report from the Info menu. Use the Lock tool sparingly.

3.1.5 Layout Area

The layout area is where you see the layout. The cursor shape depends on the active tool when the pointer is moved into the layout area. A cross hair follows the mouse pointer with respect to the grid setting. Select a new grid from the Screen menu. The new value is updated in the status line. A different way to change the grid is Shift<Key>g to decrease or <Key>g to increase it, but this only works for English (integer mil) grids. The grid setting is saved along with the data when you save a pcb layout. For homemade layouts a value around 50 is a good setting. The cursor can also be moved in the layout area with the cursor (arrow) keys or, for larger distances, by pressing the Shift modifier together with a cursor key.

3.2 Log Window

This optional window is used to display all kind of messages including the ones written to stderr by external commands. The main advantage of using it is that its contents are saved in a scrolling list until the program exits. Disabling this feature by setting the resource useLogWindow to false will generate popup windows to display messages. The stderr of external commands will appear on Pcbs stderr which normally is the parent shell. I suggest you iconify the log window after startup for example by setting *log.iconic to true in the resource file. If raiseLogWindow is set true, the window will deiconify and raise itself whenever new messages are to be displayed.

3.3 Library Window

The library window makes loading elements (or even partial layouts) easy. Just click the appropriate library from the list on the left. A list of its elements then appears on the right. Select an element from the list by clicking on its description. Selecting an element from the library will also automatically copy the element into the active buffer, then invoke the Buffer tool so you can paste it to the layout. Elements in the old library should be taken with a grain of salt (i.e. check them carefully before using). The old library names all begin with ~ so you can easily distinguish between the old and new libraries. All of the elements in the new library should be thoroughly vetted, so you can use them with confidence. The new libraries are stored simply as directories full of element files, so making additions to the new library is easy since there is no need to learn m4. For details on the old libraries, check-out Library File and Library Contents File. For details on the format of an element file used for the new libraries, see Element File.

3.4 Netlist Window

The netlist window is very similar to the library window. On the left is a list of all of the nets, on the right is the list of connections belonging to the chosen net. The chosen net is highlighted in the list and also shown on the second line of the window in red. If the net name has a star to the left of it then it is "disabled". A disabled net is treated as if it were not in the net list. This is useful, for example, if you plan to use a ground plane and don’t want the ground net showing up in the rat’s nest. You can enable/disable individual nets by double-clicking the net name. If you want to enable or disable all nets at once, there are two buttons at the top of the netlist window for this purpose.

The button labeled ‘Sel Net On Layout’ can be used to select (on the layout) everything that is connected (or is supposed to be connected) to the net. If you click on a connection in the connection list, it will select/deselect the corresponding pin or pad in the layout and also center the layout window where it is located. If you "Find" (‘lookup connection’ in the Connects menu [also F key]), a pin or pad it will also choose the net and connection in the netlist window if it exists in the netlist.

If no netlist exists for the layout, then the netlist window does not appear. You can load a netlist from a file from the File menu. The format for netlist files is described in Netlist File.

3.5 Drawing and Removing Basic Objects

hace begging gutting here, and do a real-world tutorial example.

There are several ways of creating new objects: you can draw them yourself, you can copy an existing object (or selection), or you can load an element from a file or from the Library window. Each type of object has a particular tool for creating it.

The active tool can be selected from the tool selectors in the bottom left corner or by one of the function keys listed earlier in this chapter. Each <Btn1> press with the tool tells the application to create or change the appropriate object or at least take the first step to do so. Each tools causes the cursor to take on a unique shape and also causes the corresponding tool selector button to be highlighted. You can use either cue to see which tool is active.

Insert mode provides the capability of inserting new points into existing polygons or lines. The 45 degree line clipping is now enforced when selected. Press and hold the shift key while positioning the new point to only clip the line segment to the nearer of the two existing points to 45 degrees. You can also toggle the 45-degree clipping in the middle of a point insertion by pressing the <Key>. If the shift key is not depressed and the 45 degree line clipping mode is on, both new line segments must be on 45 degree angles - greatly restricting where the new point may be placed. In some cases this can cause confusion as to whether an insertion has been started since the two new lines may be forced to lie parallel on top of the original line until the pointer is moved far from the end points.

Removing objects, changing their size or moving them only applies to objects that are visible when the command is executed.

3.5.1 Common Drawing and Removing Methods

There are several keystrokes and button events referring to an object without identifying its type. Here’s a list of them:

<Btn1> creates (or deletes) an object depending on the current mode.

<Key>BackSpace or <Key>Delete removes the visible object at the cursor location. When more than one object exists at the location, the order of removal is: via, line, text, polygon and element. The drawn layer order also affects the search - whatever is top - most (except elements) is affected before lower items. Basically all this means that what is removed is probably just what you expect. If for some reason it isn’t, undo and try again. Only one object is removed for each keystroke. If two or more of the same type match, the newest one is removed.

Use <Key>s and Shift<Key>s to change the size (width) of lines, arcs, text objects, pins, pads and vias, or to toggle the style of polygons (whether pins and vias automatically have clearances).

<Key>n changes the name of pins, pads, vias, the string of a text object, or the currently displayed label of an element.

<Key>m moves the line, arc, or polygon under the cross hair to the active layer if it wasn’t on that layer already.

<Key>u (undo) recovers from an unlimited number of operations such as creating, removing, moving, copying, selecting etc. It works like you’d expect even if you’re in the midst of creating something.

Shift<Key>r restores the last undone operation provided no other changes have been made since the undo was performed.

<Key>tab changes the board side you are viewing.

For a complete list of keystrokes and button events see Translations.

3.5.2 Lines

To draw new lines you have to be in line-mode. Get there either by selecting it from the Tool palette or by pressing <Key>F2. Each successive notify event creates a new line. The adjustment to 45 degree lines is done automatically if it is selected from the Display menu. You can toggle the 45 degree mode setting by pressing the <Key>. (That is the period key). When 45 degree enforcement is turned on there are three distinct modes of line creation: a single line on the closest 45 degree vector towards the cross hair (but not necessarily actually ending at the cross hair), two lines created such that the first leaves the start point on a 90 degree vector and the second arrives at the cross hair on a 45 degree vector, and finally two lines created such that the first leaves the start point on a 45 degree vector and the second arrives at the cross hair on a 90 degree vector. These last two modes always connect all the way from the start and end points, and all lines have angles in 45 degree multiples. The <Key>/ cycles through the three modes. The status line shows a text icon to indicate which of the modes is active and the lines following the cross hair motion show the outline of the line(s) that will actually be created. Press <Key>Escape to leave line-mode.

<Key>l, Shift<Key>l and the entries in the Sizes menu change the initial width of new lines. This width is also displayed in the status line.

3.5.3 Arcs

An Arc is drawn with the arc-tool. Get there either by selecting it from the Tool palette or by pressing <Key>F8. Press Btn1 to define the starting point for the arc. Drag the mouse towards the desired end point along the path you want the arc to follow. The outline of the arc that will be created is shown on the screen as you move the mouse. Arcs are always forced to be 90 degrees and have symmetrical length and width ( i.e. they are a quarter circle). The next Btn1 click creates the arc. It will have the same width as new lines (displayed in the status line) and appear on the active layer. The arc leaves the starting point towards the cross hair along the axis whose distance from the cross hair is largest. Normally this means that if you drag along the path you want the arc to follow, you’ll get what you want. If the grid is set to the arc radius, then the two distances will be equal and you won’t be able to get all of the possible directions. If this is thwarting your desires, reduce the grid spacing (!Shift<Key>G) and try again.

3.5.4 Polygons and Rectangles

A polygon is drawn by defining all of its segments as a series of consecutive line segments. If the first point matches a new one and if the number of points is greater than two, then the polygon is closed. Since matching up with the first point may be difficult, you may use Shift<Key>p to close the polygon. The Shift<Key>p won’t work if clipping to 45 degree lines is selected and the final segment cannot match this condition. I suggest you create simple convex polygons in order to avoid a strong negative impact on the performance of the connection scanning routines. The rectangle-mode is just an easy way to generate rectangular polygons. Polygon-mode also is selected by <Key>F6 whereas rectangle-mode uses <Key>F4. Pressing a <Btn1> at two locations creates a rectangle by defining two of its corners. <Key>Insert brings you to insert-point-mode which lets you add additional points to an already existing polygon. Single points may be removed by moving the cross hair to them and selecting one of the delete actions (remove-mode, BackSpace, or Delete. This only works if the remaining polygon will still have three or more corners. Pressing <Key>u or <Key>p while entering a new polygon brings you back to the previous corner. Removing a point does not force clipping to 45 degree angles (because it’s not generally possible). Newly created polygons will not connect to pins or vias that pierce it unless you create a thermal (using the thermal mode) to make the connection. If the edge of a polygon gets too close to a pin or via that lies outside of it, a warning will be issued and the pin will be given a special color. Increasing the distance between them will remove the warning color.

3.5.5 Text

Pressing <Key>F5 or clicking one of the text selector buttons changes to text-mode. Each successive notify event (<Btn1>) pops up the input line at the bottom and queries for a string. Enter it and press <Key>Return to confirm or <Key>Escape to abort. The text object is created with its upper left corner at the current pointer location. The initial scaling is changed by <Key>t and Shift<Key>t or from the Sizes menu.

Now switch to rotate-mode and press <Btn1> at the text-objects location. Text objects on the solder side of the layout are automatically mirrored and flipped so that they are seen correctly when viewing the solder-side.

Use <Key>n to edit the string.

TEXT OBJECTS ON COPPER LAYERS CREATE COPPER LINES BUT THEY ARE NOT SCANNED FOR CONNECTIONS. If they are moved to the silkscreen layer, they no longer create copper.

3.5.6 Vias

The initial size of new vias may be changed by <Key>v and Shift<Key>v or by selecting the appropriate entry from the Sizes menu. Mod1<Key>v and Mod1 Shift<Key>v do the same for the drilling hole of the via. The statusline is updated with the new values. Creating a via is similar to the other objects. Switch to via-mode by using either the selector button or <Key>F1 then press <Key>] or <Btn1> to create one. <Key>n changes the name of a via. If you want to create a mounting hole for your board, then you can place a via where you want the hole to be then convert the via into a hole. The conversion is done by pressing !Ctrl<Key>h with the cross hair over the via. Conceptually it is still a via, but it has no copper annulus. If you create such a hole in the middle of two polygons on different layers, it will short the layers. Theoretically you could arrange for such a hole not to be plated, but a metal screw inserted in the hole would still risk shorting the layers. A good rule is to realize that holes in the board really are vias between the layers and so place them where they won’t interfere with connectivity. You can convert a hole back into a normal via with the same keystroke used to convert it in the first place.

The via can be converted to blind or buried via using appropriate action, menu item or keys: Ctrl-Shift-F to set active layer as first layer, Ctrl-Shift-T to set last layer and Ctrl-Shift-P to convert via back to through-hole via.

3.5.7 Elements

Some of the functions related to elements only work if both the package layer and the pin layer are switched on.

Now that you’re familiar with many of the basic commands, it is time to put the first element on the layout. First of all, you have to load data into the paste buffer. There are four ways to do this:

   1) load the data from a library
   2) load the data from a file
   3) copy data from an already existing element
   4) convert objects in the buffer into an element

We don’t have any elements on the screen yet nor anything in the buffer, so we use number one.

Select lsi from the menu in the library window press <Btn1> twice at the appropriate text-line to get the MC68030 CPU. The data is loaded and the mode is switched to pastebuffer-mode. Each notify event now creates one of these beasts. Leave the mode by selecting a different one or by <Key>Escape which resets all modes.. The cross hair is located at the mark position as defined by the data file. Rotating the buffer contents is done by selecting the rotate entry of the Buffer menu or by pressing Shift<Key>F3. The contents of the buffer are valid until new data is loaded into it either by a cut-to-buffer operation, copy-to-buffer operation or by loading a new data file. There are 5 buffers available (possibly more or less if changed at compile time with the MAX_BUFFER variable in globalconfig.h). Switching between them is done by selecting a menu entry or by Shift<Key>1..MAX_BUFFER. Each of the two board sides has its own buffers.

The release includes all data files for the circuits that are used by the demo layout. The elements in the LED example are not found in the library, but you can lift them from the example itself if you want. If you have problems with the color of the cross hair, change the resource cross hairColor setting to a different one.

Now load a second circuit, the MC68882 FPU for example. Create the circuit as explained above. You now have two different unnamed elements. Unnamed means that the layout-name of the element hasn’t been set yet. Selecting description from the Display menu displays the description string of the two circuits which are CPU and FPU. The values of the circuits are set to MC68030 and MC68882. Each of the names of an element may be changed by <Key>n at the elements location and editing the old name in the bottom input line. Naming pins and vias is similar to elements. You can hide the element name so that it won’t appear on the board silkscreen by pressing <key>h with the cursor over the element. Doing so again un-hides the element name.

Entering :le and selecting an element data file is the second way to load circuits.

The third way to create a new element is to copy an existing one. Please refer to Moving and Copying.

The fourth way to create a new element is to convert a buffer’s contents into an element. Here’s how it’s done: Select the Via-tool from the Tool pallet. Set the grid spacing to something appropriate for the element pin spacing. Now create a series of vias where the pins go. Create them in pin number order. It is often handy to place a reference point (!Ctrl<Key>m) in the center of the first pin in order to measure the location of the other pins. Next make a solder-side layer the active layer from the active-layer popup menu. Now draw the outline of the element using lines and arcs. When you’re done, select everything that makes up the element with a box selection (<Btn3Down> drag, <Btn3Up>). Now select "cut to buffer" from the Buffer menu. Position the cursor over the center of pin 1 and press the left button to load the data into the buffer. Finally select "convert buffer to element" from the Buffer menu. You’ll only want to create elements this way if they aren’t already in the library. It’s also probably a good idea to do this before starting any of the other aspects of a layout, but it isn’t necessary.

To display the pinout of a circuit move to it and press Shift<Key>d or select show pinout from the Objects menu. A new window pops up and displays the complete pinout of the element. This display can be difficult to read if the component has been rotated 90 degrees :-( therefore, the new window will show an un-rotated view so the pin names are readable. <Key>d displays the name of one or all pins/pads inside the Layout area, this is only for display on-screen, it has no effect on any printing of the layout.

You also may want to change a pin’s or pad’s current size by pressing <Key>s to increase or Shift<Key>s to decrease it. While this is possible, it is not recommended since care was probably taken to define the element structure in the first place. You can also change the thickness of the element’s silkscreen outline with the same keys. You can change whether a pin or SMD pad is rounded or square with the <Key>q. SMD pads should usually have squared ends. Finally, you can change whether the non-square pins are round or octagonal with the !Ctrl<Key>o.

SMD elements and silkscreen objects are drawn in the "invisible object" color if they are located on the opposite side of the board.

For information on element connections refer to Connection Lists.

3.5.8 Pastebuffer

The line-stack and element-buffer of former releases have been replaced by 5 (possibly more or less if changed at compile time with the MAX_BUFFER variable in globalconfig.h) multi-purpose buffers that are selected by Shift<Key>1..MAX_BUFFER. The status line shows which buffer is the active one. You may load data from a file or layout into them. Cut-and-paste works too. If you followed the instructions earlier in this chapter you should now have several objects on the screen. Move the cross hair to one of them and press <Btn3Down> to toggle its selection flag. (If you drag the mouse while the button is down, a box selection will be attempted instead of toggling the selection.) The object is redrawn in a different color. You also may want to try moving the pointer while holding the third button down and release it on a different location. This selects all objects inside the rectangle and unselects everything else. If you want to add a box selection to an existing selection, drag with Mod1<Btn3Down> instead. Dragging Shift Mod1<Btn3Down> unselects objects in a box. Now change to pastebuffer-mode and select some operations from the Buffer menu. Copying objects to the buffer is available as Mod1<Key>c while cutting them uses Mod1<Key>x as shortcut. Both clear the buffer before new data is added. If you use the menu entries, you have to supply a cross hair position by pressing a mouse button. The objects are attached to the pastebuffer relative to that cross hair location. Element data or PCB data may be merged into an existing layout by loading the datafiles into the pastebuffer. Both operations are available from the File menu or as user commands.

3.6 Moving and Copying

All objects can be moved including element-names, by <Btn2Down>, dragging the pointer while holding the button down and releasing it at the new location of the object. If you use Mod1<Btn2Down> instead, the object is copied. Copying does not work for element-names of course. You can move all selected objects with Shift <Btn1>. This uses the Pastebuffer, so it will remove whatever was previously in the Pastebuffer. Please refer to Pastebuffer. If you want to give a small nudge to an object, but you don’t think that the mouse will give you the fine level of control that you want, you can position the cursor over the object, press <Key>[, move it with the arrow keys, then press <Key>] when it’s at the desired position. Remember that all movements are forced onto grid coordinates, so you may want to change the grid spacing first.

To move a trace or group of traces to a different layer, first select the tracks to be moved. It’s easiest to do this if you shut off everything but that layer first (i.e. silk, pins, other layers, etc). Now set the current layer to be the new layer. Press Shift-M to move all the selected tracks to the current layer. See the MoveToCurrentLayer action for more details.

3.7 Loading and Saving

After your first experience with Pcb you will probably want to save your work. :s name passes the data to an external program which is responsible for saving it. For details see saveCommand in Resources. Saving also is available from the File menu, either with or without supplying a filename. Pcb reuses the last filename if you do not pass a new one to the save routine.

To load an existing layout either select Open... from the File menu or use :l filename. A file select box pops up if you don’t specify a filename. Merging existing layouts into the new one is supported either by the File menu or by :m filename.

Pcb saves a backup of the current layout at a user specified interval. The backup filename is created by appending a dash, "-", to the .pcb filename. For example, if you are editing the layout in projects/board.pcb then the backup file name will be projects/board.pcb-. If the layout is new and has not been saved yet, then the backup file name is PCB.####.backup where the "####" will be replaced by the process ID of the currenting running copy of Pcb. This default backup file name may be changed at compilation time via the BACKUP_NAME variable in globalconfig.h. During critical sections of the program or when data would be lost it is saved as PCB.%i.save. This file name may be changed at compile time with the SAVE_NAME variable in globalconfig.h.

3.8 Printing

Pcb now has support for device drivers, PostScript, encapsulated PostScript, and Gerber RS-274X drivers are available so far. The Gerber RS-274X driver additionally generates a numerical control (NC) drill file for automated drilling, a bill of materials file to assist in materials procurement and inventory control, and a centroid (X-Y) file which includes the centroid data needed by automatic assembly (pick and place) machines. I recommend the use of GhostScript if you don’t have a PostScript printer for handling the PostScript output. Printing always generates a complete set of files for a specified driver. See the page about the Print() action for additional information about the filenames. The control panel offers a number of options. Most of them are not available for Gerber output because it wouldn’t make sense, for example, to scale the gerber output (you’d get an incorrectly made board!). The options are:

‘device’

The top menu button selects from the available device drivers.

‘rotate’

Rotate layout 90 degrees counter-clockwise before printing (default).

‘mirror’

Mirror layout before printing. Use this option depending on your production line.

‘color’

Created colored output. All colors will be converted to black if this option is inactive.

‘outline’

Add a board outline to the output file. The size is determined by the maximum board size changeable from the sizes menu. The outline appears on the top and bottom sides of the board, but not on the internal layers. An outline can be useful for determining where to shear the board from the panel, but be aware that it creates a copper line. Thus it has the potential to cause short circuits if you don’t leave enough room from your wiring to the board edge. Use a viewer to see what the output outline looks like if you want to know what it looks like.

‘alignment’

Additional alignment targets are added to the output. The distances between the board outline is set by the resource alignmentDistance. Alignment targets should only be used if you know for certain that YOU WILL BE USING THEM YOURSELF. It is extremely unlikely that you will want to have alignment targets if you send gerber files to a commercial pcb manufacture to be made.

‘scaling’

It’s quite useful to enlarge your printout for checking the layout. Use the scrollbar to adjust the scaling factor to your needs.

‘media’

Select the size of the output media from this menu. The user defined size may be set by the resource media either from one of the well known paper sizes or by a X11 geometry specification. This entry is only available if you use X11R5 or later. For earlier releases the user defined size or, if not available, A4 is used. Well known size are:

	A3
	A4
	A5
	letter
	tabloid
	ledger
	legal
	executive

‘offset’

Adjust the offsets of the printout by using the panner at the right side of the dialog box. This entry is only available if you use X11R5 or later. A zero offset is used for earlier releases.

‘8.3 filenames’

Select this button to generate DOS compatible filenames for the output files. The command input area will disappear if selected.

‘commandline’

Use this line to enter a command (starts with |) or a filename. A %f is replaced by the current filename. The default is set by the resource printCommand.

The created file includes some labels which are guaranteed to stay unchanged

‘PCBMIN’

identifies the lowest x and y coordinates in mil.

‘PCBMAX’

identifies the highest x and y coordinates in mil.

‘PCBOFFSET’

is set to the x and y offset in mil.

‘PCBSCALE’

is a floating point value which identifies the scaling factor.

‘PCBSTARTDATA’

‘PCBENDDATA’

all layout data is included between these two marks. You may use them with an awk script to produce several printouts on one piece of paper by duplicating the code and putting some translate commands in front. Note, the normal PostScript units are 1/72 inch.

3.9 Exporting a layout

To export a layout choose Export layout from the File menu, then select the desired exporter.

3.9.1 Bill of materials (bom)

Produces a bill of materials (BOM) file and a centroid (XY) file.

3.9.2 Bill Of Materials in MarkDown format (bom_md)

Produces a bill of materials (BOM) file in MarkDown format.

3.9.3 G-code (gcode)

The gcode exporter can generate RS274/NGC G-CODE files to be used with a CNC mill to produce pcb’s by mechanically removing copper from the perimeter of all elements.

The elements are enlarged in order to compensate for the cutting tool size so that the remaining copper corresponds to the original size; however all polygons are left unchanged and will end up being a little smaller; this is not a problem because the electrical connection is done with traces, which are correctly enlarged.

A .cnc file is generated for every copper layer, with the bottom layer mirrored so that the milling is done right; of course it’s not possible to produce directly multi-layer (more than 2) pcb’s with this method, but the cnc files for intermediate layers are generated anyways.

A drill file is also generated, and it contains all drills regardless of the hole size; the drilling sequence is optimized in order to require the least amount of movement.

The export function generates an intermediate raster image before extracting the contour of copper elements, and this image is saved as well (in .png format) for inspection.

When the spacing between two elements is less than the tool diameter they will merge and no isolation will be cut between them; the control image should be checked for this behaviour.

Possible workarounds are: increasing spacing, decreasing the tool size, increasing the intermediate image resolution.

To maximize the chance of producing correct pcb’s it would be better to increase the DRC clearance to at least the tool diameter and use traces as thick as possible; the rule is: use the largest element that will not prevent the isolation cut.

The exporter parameters are:

basename

base name for generated files

dpi

intermediate image resolution; affects precision when extracting contours

mill depth

should be the copper depth

safe z

Z value when moving between polygons

tool radius

copper elements are enlarged by this amount

drill depth

depth of drills

measurement unit

for all parameters above, can be mm,um,inch,mil; g-code is always mm or inch

All .cnc files specify Z values as parameters, so that it’s easy to change them without the need to run the exporter again.

Operation was verified with the EMC2 g-code interpreter.

Following is a sample layout that is converted with default settings:

The control image shows that the spacing is sufficient:

The final tool path follows the perimeter of all elements:

3.9.4 Gerber (gerber)

Produces RS274-X (a.k.a. gerber) photo plot files and Excellon drill files.

3.9.5 Postscript (ps)

Export as postscript. Can be later converted to pdf.

3.9.6 Encapsulated Postscript (eps)

Export as eps (encapsulated postscript) for inclusion in other documents. Can be later converted to pdf.

3.9.7 Image (png)

Produces GIF/JPEG/PNG image files.

3.9.8 Nelma (nelma)

Numerical analysis package export.

Nelma is a (command line) tool for numerically calculating various electrical properties of printed circuit boards or similar objects composed of conductors and dielectrics (however code is optimized for circuit board-like geometry).

It is currently capable of calculating capacitances between objects - nets on a PCB.

It returns a spice-compatible description of an equivalent circuit of stray capacitances that can be for example used for more accurate circuit simulation.

Alternatively it can also produce field data that can be plotted for example with Gnuplot.

Support for calculating resistances existed for a while but was later removed because it didn’t receive much testing.

The Nelma exporter produces a PNG image file for every copper layer and an input file (.em).

The home page of Nelma can be found at https://www.tablix.org/~avian/nelma/.

3.9.9 GSvit (gsvit)

Numerical analysis package export.

GSvit covers set of numerical tools for Finite Difference in Time Domain calculations supporting use of Nvidia CUDA environment compatible graphics cards.

Main scientific purposes include research in nanotechnology and nanoscale optics, like scanning near-field optical microscopy, tip enhanced Raman scattering, rough surface scattering, etc.

However, as FDTD is an universal method, it can be used for any other purposes.

The GSvit exporter produces a PNG image file for every copper layer and a xml input file (.xem).

The home page of GSvit can be found at http://gsvit.net.

3.9.10 IPC-D-356 (ipcd356)

Produces an IPC-D-356 compliant netlist file for bare board testing.

3.10 Connection Lists

After completing parts of your layout you may want to check if all drawn connections match the ones you have in mind. This is probably best done in conjunction with a net-list file: see Rats Nest. The following examples give more rudimentary ways to examine the connections.

    1) create at least two elements and name them
    2) create some connections between their pins
    3) optionally add some vias and connections to them

Now select lookup connection from the Connections menu, move the cursor to a pin or via and press any mouse button. Pcb will look for all other pins and/or vias connected to the one you have selected and display the objects in a different color. Now try some of the reset options available from the same menu.

There also is a way to scan all connections of one element. Select a single element from the menu and press any button at the element’s location. All connections of this element will be saved to the specified file. Either the layout name of the element or its canonical name is used to identify pins depending on the one which is displayed on the screen (may be changed by Display menu).

An automatic scan of all elements is initiated by choosing all elements. It behaves in a similar fashion to scanning a single element except the resource resetAfterElement is used to determine if connections should be reset before a new element is scanned. Doing so will produce very long lists because the power lines are rescanned for every element. By default the resource is set to false for this reason.

To scan for unconnected pins select unused pins from the same menu.

3.11 Arrow Tool

Some commands mentioned earlier in this chapter also are able to operate on all selected and visible objects. The Arrow tool is used to select/deselect objects and also to move objects or selections. If you click and release on an object with the Arrow tool, it will unselect everything else and select the object. Selected objects change color to reflect that they are selected. If you Shift click, it will add the object to (or remove) the object from the existing selection. If you drag with the mouse button down with the Arrow tool, one of several things could happen: if you first pressed the button on a selected object, you will be moving the selection to where you release the button. If you first pressed the button on an unselected object, you will be moving that object. If you first pressed the button over empty space, you will be drawing a box to select everything inside the box. The Shift key works the same way with box selections as it does with single objects.

Moving a single un-selected object is different from moving a selection. First of all, you can move the end of line, or a point in a polygon this way which is impossible by moving selections. Secondly, if rubber banding is turned on, moving a single object will rubber-band the attached lines. Finally, it is faster to move a single object this way since there is no need to select it first.

You can select any visible object unless it is locked. If you select an object, then turn off its visibility with the Layer controls, it won’t be moved if you move the remaining visible selection.

If you have not configured to use strokes in the Pcb user interface, then the middle mouse button is automatically bound to the arrow tool, regardless of the active tool (which is bound to the first mouse button). So using the middle button any time is just like using the first mouse button with the Arrow tool active.

The entries of the Selection menu are hopefully self-explanatory. Many of the Action Commands can take various key words that make them function on all or some of the selected items.

3.12 Rats Nest

If you have a netlist that corresponds to the layout you are working on, you can use the rats-nest feature to add rat-lines to the layout. First you will need to load a netlist file (see :rn, User Commands). <Key>w adds rat-lines on the active layer using the current line thickness shown in the status line (usually you’ll want them to be thin lines). Only those rat-lines that fill in missing connectivity (since you have probably routed some connections already) are added. If the layout is already completely wired, nothing will be added, and you will get a message that the wiring is complete.

Rat-lines are lines having the special property that they only connect to pins and pads at their end points. Rat-lines may be drawn differently to other lines to make them easier to identify since they have special behavior and cannot remain in a completed layout. Rat-lines are added in the minimum length straight-line tree pattern (always ending on pins or pads) that satisfies the missing connectivity in the circuit. Used in connection with moves and rotates of the elements, they are extremely useful for deciding where to place elements on the board. The rat-lines will always automatically rubberband to the elements whether or not the rubberband mode is on. The only way for you to move them is by moving the parts they connect to. This is because it is never desirable to have the rat-lines disconnected from their element pins. Rat-lines will normally criss-cross all over which gives rise to the name "rats nest" describing a layout connected with them. If a SMD pad is unreachable on the active layer, a warning will be issued about it and the rat-line to that pad will not be generated.

A common way to use rats nests is to place some elements on the board, add the rat-lines, and then use a series of moves/rotates of the elements until the rats nest appears to have minimum tangling. You may want to iterate this step several times. Don’t worry if the layout looks messy - as long as you can get a sense for whether the criss-crossing is better or worse as you move things, you’re fine. After moving some elements around, you may want to optimize the rats nest <Key>o so that the lines are drawn between the closest points (this can change once you’ve moved components). Adding rat-lines only to selected pads/pins (Shift<Key>w) is often useful to layout a circuit a little bit at a time. Sometimes you’ll want to delete all the rat-lines (<Key>e) or selected rat-lines (Shift<Key>e) in order to reduce confusion. With a little practice you’ll be able to achieve a near optimal component placement with the use of a rats nest.

Rat-lines are not only used for assisting your element placement, they can also help you to route traces on the board. Use the <Key>m to convert a rat-line under the cursor into a normal line on the active layer. Inserting a point into a rat-line will also cause the two new lines to be normal lines on the board. Another way that you can use rat-lines is to use the <Key>f with the cursor over a pad or pin. All of the pins and pads and rat-lines belonging to that net will be highlighted. This is a helpful way to distinguish one net from the rest of the rats nest. You can then route those tracks, turn off the highlighting (Shift<Key>f) and repeat the process. This will work even if the layer that the rat-lines reside on is made invisible - so only the pins and pads are highlighted. Be sure to erase the rat-lines (<Key>e erases them all) once you’ve duplicated their connectivity by adding your own lines. When in doubt, the <Key>o will delete only those rat-lines that are no longer needed.

If connections exist on the board that are not listed in the netlist when <Key>w is pressed, warning messages are issued and the affected pins and pads are drawn in a special warnColor until the next Notify() event. If the entire layout agrees completely with the netlist, a message informs you that the layout is complete and no rat-lines will be added (since none are needed). If the layout is complete, but still has rat-lines then you will be warned that rat-lines remain. If you get no message at all it’s probably because some elements listed in the net list can’t be found and where reported in an earlier message. There shouldn’t be any rat-lines left in a completed layout, only normal lines.

The Shift<Key>w is used to add rat-lines to only those missing connections among the selected pins and pads. This can be used to add rat-lines in an incremental manner, or to force a rat-line to route between two points that are not the closest points within the net. Often it is best to add the rats nest in an incremental fashion, laying out a sub-section of the board before going further. This is easy to accomplish since new rat-lines are never added where routed connectivity already makes the necessary connections.

3.13 Design Rule Checking

After you’ve finished laying out a board, you may want to check to be certain that none of your interconnections are too closely spaced or too tenuously touching to be reliably fabricated. The design rule checking (DRC) function does this for you. Use the command ":DRC()" (without the quotes of course) to invoke the checker. If there are no problem areas, you’ll get a message to that effect. If any problem is encountered, you will get a message about it and the affected traces will be highlighted. One part of the tracks of concern will be selected, while the other parts of concern will have the "FindConnection" highlighting. The screen will automatically be centered in the middle of the object having the "FindConnection" (Green) highlighting. The middle of the object is also the coordinates reported to be "near" the problem. The actual trouble region will be somewhere on the boundary of this object. If the two parts are from different nets then there is some place where they approach each other closer than the minimum rule. If the parts are from the same net, then there is place where they are only barely connected. Find that place and connect them better.

After a DRC error is found and corrected you must run the DRC again because the search for errors is halted as soon as the first problem is found. Unless you’ve been extremely careless there should be no more than a few design rule errors in your layout. The DRC checker does not check for minimum spacing rules to copper text, so always be very careful when adding copper text to a layout. The rules for the DRC are specified in the application resource file. The minimum spacing value (in mils) is given by the Settings.Bloat value. The default is 7 mils. The minimum touching overlap (in mils) is given by the Settings.Shrink value. This value defaults to 5 mils. Check with your fabrication process people to determine the values that are right for you.

If you want to turn off the highlighting produced by the DRC, perform an undo (assuming no other changes have been made). To restore the highlighting, use redo. The redo will restore the highlighting quickly without re-running the DRC checker.

3.14 Trace Optimizer

PCB includes a flexible trace optimizer. The trace optimizer can be run after auto routing or hand routing to clean up the traces.

Auto-Optimize

Performs debumpify, unjaggy, orthopull, vianudge, and viatrim, in that order, repeating until no further optimizations are performed.

Debumpify

Looks for U shaped traces that can be shortened or eliminated.

Unjaggy

Looks for corners which could be flipped to eliminate one or more corners (i.e. jaggy lines become simpler).

Vianudge

Looks for vias where all traces leave in the same direction. Tries to move via in that direction to eliminate one of the traces (and thus a corner).

Viatrim

Looks for traces that go from via to via, where moving that trace to a different layer eliminates one or both vias.

Orthopull

Looks for chains of traces all going in one direction, with more traces orthogonal on one side than on the other. Moves the chain in that direction, causing a net reduction in trace length, possibly eliminating traces and/or corners.

SimpleOpts

Removing unneeded vias, replacing two or more trace segments in a row with a single segment. This is usually performed automatically after other optimizations.

Miter

Replaces 90 degree corners with a pair of 45 degree corners, to reduce RF losses and trace length.

3.15 Searching for elements

To locate text or a specific element or grouping of similar elements choose ‘Select by name’ from the Select menu, then choose the appropriate subsection. At the bottom of the screen the prompt pattern: appears. Enter the text or Regular Expressions of the text to be found. Found text will be highlighted.

3.16 Measuring distances

To measure distances, for example the pin-to-pin pitch of a part to validate a footprint, place the cursor at the starting measurement point, then press !Ctrl<Key>m. This marks the current location with a X. The X mark is now the zero point origin for the relative cursor position display. The cursor display shows both absolute position and position relative to the mark as the mouse is moved away from the mark. If a mark is already present, the mark is removed and the cursor display stops displaying relative cursor coordinates.

3.17 Vendor Drill Mapping

Pcb includes support for mapping drill holes to a specified set of sizes used by a particular vendor. Many PCB manufacturers have a prefered set of drill sizes and charge extra when others are used. The mapping can be performed on an existing design and can also be enabled to automatically map drill holes as vias and elements are instantiated.

The first step in using the vendor drill mapping feature is to create a resource file describing the capabilities of your vendor. The file format is the resource file format described in Resource Syntax. A complete example is given below.

# Optional name of the vendor
vendor = "Vendor Name"

# units for dimensions in this file.
# Allowed values:  mil/inch/mm
units = mil

# drill table
drillmap = {
   # When mapping drill sizes, select the nearest size
   # or always round up.  Allowed values:  up/nearest
   round = up

   # The list of vendor drill sizes.  Units are as specified
   # above.
   20
   28
   35
   38
   42
   52
   59.5
   86
  125   
  152

   # optional section for skipping mapping of certain elements
   # based on reference designator, value, or description
   # this is useful for critical parts where you may not
   # want to change the drill size.  Note that the strings
   # are regular expressions.  
   skips = {
      {refdes "^J3$"}  # Skip J3.
      {refdes "J3"}  # Skip anything with J3 as part of the refdes.
      {refdes "^U[1-3]$" "^X.*"} # Skip U1, U2, U3, and anything starting with X.
      {value "^JOHNSTECH_.*"} # Skip all Johnstech footprints based on the value of a part.
      {descr "^AMP_MICTOR_767054_1$"} # Skip based on the description.
   }
}

# If specified, this section will change the current DRC
# settings for the design.  Units are as specified above.
drc = {
   copper_space = 7
   copper_width = 7
   silk_width = 10
   copper_overlap = 4
}

The vendor resource is loaded using the LoadVendor action. This is invoked by entering:

:LoadVendor(vendorfile)

from within Pcb. Substitute the file name of your vendor resource file for ‘vendorfile’. This action will load the vendor resource and modify all the drill holes in the design as well as the default via hole size for the various routing styles.

Once a vendor drill map has been loaded, new vias and elements will automatically have their drill hole sizes mapped to the vendor drill table. Automatic drill mapping may be disabled under the “Settings” menu. To re-apply an already loaded vendor drill table to a design, choose “Apply vendor drill mapping” from the “Connects” menu.

See Actions for a complete description of the actions associated with vendor drill mapping.

Note that the expressions used in the skips section are regular expressions. See Regular Expressions for an introduction to regular expressions.

4 Autorouter

Pcb includes an autorouter which can greatly speed up the layout of a circuit board. The autorouter is a rectangle-expansion type of autorouter based on “A Method for Gridless Routing of Printed Circuit Boards” by A. C. Finch, K. J. Mackenzie, G. J. Balsdon, and G. Symonds in the 1985 Proceedings of the 22nd ACM/IEEE Design Automation Conference. This reference is available from the ACM Digital Library at http://www.acm.org/dl for those with institutional or personal access to it. It’s also available from your local engineering library. The reference paper is not needed for using the autorouter.

Before using the autorouter, all elements need to be loaded into the layout and placed and the connectivity netlist must be loaded. Once the elements have been placed and the netlist loaded, the following steps will autoroute your design.

1. Turn off visibility of any layers that you don’t want the router to use.
2. Turn off via visibility if you don’t want the router to use any new vias.
3. Use only plain rectangles for power/ground planes that you want the router to use [use the rectangle tool!]
4. Make at least one connection from any plane you want the router to use to the net you want it to connect to.
5. Draw continuous lines (on all routing layers) to outline keep-out zones if desired.
6. Use routing styles in the netlist to have per-net routing styles. Note that the routing style will be used for an entire net. This means if you have a wide metal setting for a power net you will need to manually route breakouts from any fine pitch parts on their power pins because the router will not be able to change to a narrow trace to connect to the part.
7. Set the current routing style to whatever you’d like the router to use for any nets not having a defined route style in the netlist.
8. Disable any nets that you don’t want the autorouter to route (double-click them in the netlist window to add/remove the *).

   NOTE: If you will be manually routing these later not using planes, it is usually better to let the autorouter route them then rip them up yourself afterwards. If you plan to use a ground/power plane manually, consider making it from one or more pure rectangles and letting the autorouter have a go at it.

9. Create a fresh rat’s nest. (E then W)
10. Select “show autorouter trials” in the settings menu if you want to watch what’s happening.
11. Choose “autoroute all rats” in the connection menu.
12. If you really want to muck with the router because you have a special design, e.g. all through-hole components you can mess with layer directional costs by editing the autoroute.c source file and changing the directional costs in lines 929-940. and try again. Even more mucking about with costs is possible in lines 4540-4569, but it’s probably not such a good idea unless you really just want to experiment.

After the design has been autorouted, you may want to run the trace optimizer. See section Trace Optimizer for more information on the trace optimizer.

5 Toporouter

Pcb includes a Topological autorouter (Toporouter) which can greatly speed up the layout of a circuit board.

The Topological autorouter was implemented by Anthony Blake and is a topological type of autorouter based on:

“Layer Assignment for a Rubber Band Router” by Dayan, T. and Dai, W.W.M., Tech Report UCSC-CRL-92-50, Univ. of California, Santa Cruz, 1992.

“Topological Routing in SURF: Generating a Rubber-Band Sketch” by Dai, W.W.M and Dayan, T. and Staepelaere, D., Proc. 28th ACM/IEEE Design Automation Conference, 1991, pp. 39-44.

“SURF: Rubber-Band Routing System for Multichip Modules,” by David Staepelaere, Jeffrey Jue, Tal Dayan, Wayne Wei-Ming Dai, IEEE Design and Test of Computers ,vol. 10, no. 4, pp. 18-26, October/December, 1993.

“Rubber-band based topological router” by Dayan, T., PhD Thesis, Univ. of California, Santa Cruz, 1997.

“Geometric transformations for a rubber-band sketch” by David Staepelaere, Master’s thesis, Univ. of California, Santa Cruz, September 1992.

These reference papers are not needed for using the Topological autorouter.

In difference to the autorouter, the Topological autorouter makes global optimization of routes, and uses lines and arcs that meet the current DRC. The current implementation is not capable to connect pads to rectangles and polygons.

Choose “Toporouter” in the “Connection” menu to use Topological autorouter.

Before using the Topological autorouter, all elements need to be loaded into the layout and placed, and the connectivity netlist must be loaded.

Once the elements have been placed and the netlist loaded, the following steps will route your design:

1. Turn off visibility of any layers that you don’t want the router to use.
2. Set the current routing style to whatever you’d like the router to use for any nets not having a defined route style in the netlist.

Toporouter is an experimental code, so remember to save your design before calling Toporouter.

6 User Commands

The entering of user-commands is initiated by selecting Command entry in the menu or typing a (":"). This runs the action routine Command(), which replaces the bottom statusline with an input area or opens a separate command window. Error and diagnostic messages go to the Message Log, so it’s a good idea to have this window open as well. Command entry is finished by either <Key>Return or <Key>Escape to confirm or to abort.

Commands can be entered in one of two styles, command entry syntax:

Command arg1 arg2

or action script syntax:

Action1(arg1, arg2); Action2(arg1, arg2);

To find out about how a command works, use the argument usage:

SaveTo usage

There is a command for usage of the complete set of commands.

Quoting arguments works similar to bash quoting:

• A backslash (\) is the escape character. It preserves the literal value of the next character that follows. To get a literal ’\’ use "\\".
• Enclosing characters in single quotes preserves the literal value of each character within the quotes. A single quote may not occur between single quotes, even when preceded by a blackslash.
• Enclosing characters in double quotes preserves the literal value of all characters within the quotes, with the exception of ’\’ which maintains its special meaning as an escape character.

Action commands allow you to initiate actions which are not bound to any menu item. They can be used to initiate any action with whatever arguments you enter. For example, to change the drilling hole diameter of all vias in the layout to 32 mils, you could select everything using the selection menu, then type:

:ChangeDrillSize(SelectedVias, 32mil)

Another example might be to set the grid to 2.5 mil by typing:

:SetValue(Grid, 2.5mil)

Note that some actions use the current cursor location, so be sure to place the cursor where you want before entering the command. For more actions, see the Actions section.

7 Command-Line Options

The synopsis of the pcb command is:

pcb [OPTION ...] [LAYOUT-FILE.pcb] to start the application in GUI mode,

or

pcb [-h | -V | --copyright] for a list of options, version, and copyright,

or

pcb -p [OPTION ...] [LAYOUT-FILE.pcb] to print a layout,

or

pcb -x HID [OPTION ...] [LAYOUT-FILE.pcb] to export.

Possible values for the parameter ‘HID’ are:

‘bom’

Export a bill of materials

‘gcode’

Export to G-Code

‘gerber’

Export RS-274X (Gerber)

‘nelma’

Numerical analysis package export

‘png’

export GIF/JPEG/PNG

‘ps’

export postscript

‘eps’

export encapsulated postscript

There are several resources which may be set or reset in addition to the standard toolkit command-line options. For a complete list refer to Resources.

7.1 General Options

--help

Show help on command line options.

--version

Show version.

--verbose

Be verbose on stdout.

--copyright

Show copyright.

--show-defaults

Show option defaults.

--show-actions

Show available actions and exit.

--dump-actions

Dump actions (for documentation).

--grid-units-mm <string>

Set default grid units. Can be mm or mil. Defaults to mil.

--clear-increment-mm <string>

Set default clear increment (amount to change when user presses k or K) when user is using a metric grid unit.

--grid-increment-mm <string>

Set default grid increment (amount to change when user presses g or G) when user is using a metric grid unit.

--line-increment-mm <string>

Set default line increment (amount to change when user presses l or L) when user is using a metric grid unit.

--size-increment-mm <string>

Set default size increment (amount to change when user presses s or S) when user is using a metric grid unit.

--clear-increment-mil <string>

Set default clear increment (amount to change when user presses k or K) when user is using an imperial grid unit.

--grid-increment-mil <string>

Set default grid increment (amount to change when user presses g or G) when user is using a imperial grid unit.

--line-increment-mil <string>

Set default line increment (amount to change when user presses l or L) when user is using a imperial grid unit.

--size-increment-mil <string>

Set default size increment (amount to change when user presses s or S) when user is using a imperial grid unit.

--backup-interval

Time between automatic backups in seconds. Set to 0 to disable. The default value is 60.

--groups <string>

Layer group string. Defaults to "1,c:2:3:4:5:6,s:7:8".

--route-styles <string>

A string that defines the route styles. Parameters are (in order): line width, via hole size, via ring size, clearance, solder mask clearance. The units are cmils. Defaults to
"Signal,1000,3600,2000,1000,0:Power,2500,6000,3500,1000,0 :Fat,4000,6000,3500,1000,0:Skinny,600,2402,1181,600,0"

--element-path <string>

A colon separated list of directories or commands (starts with ’|’). The path is passed to the program specified in --element-command.

--action-script <string>

If set, this file is executed at startup.

--action-string <string>

If set, this string of actions is executed at startup.

--fab-author <string>

Name of author to be put in the Gerber files.

--layer-stack <string>

Initial layer stackup, for setting up an export. A comma separated list of layer names, layer numbers and layer groups.

--save-last-command

If set, the last user command is saved.

--save-in-tmp

If set, all data which would otherwise be lost are saved in a temporary file /tmp/PCB.%i.save . Sequence ‘%i’ is replaced by the process ID.

--save-metric-only

If set, save pcb files using only mm unit suffix rather than ’smart’ mil/mm.

--reset-after-element

If set, all found connections are reset before a new component is scanned.

--auto-buried-vias

Enables automatically created vias (during line moves and layer switch) to be buriad/blind vias

--ring-bell-finished

Execute the bell command when all rats are routed.

7.2 General GUI Options

--pinout-offset-x <num>

Horizontal offset of the pin number display. Defaults to 100mil.

--pinout-offset-y <num>

Vertical offset of the pin number display. Defaults to 100mil.

--pinout-text-offset-x <num>

Horizontal offset of the pin name display. Defaults to 800mil.

--pinout-text-offset-y <num>

Vertical offset of the pin name display. Defaults to -100mil.

--draw-grid

If set, draw the grid at start-up.

--clear-line

If set, new lines clear polygons.

--full-poly

If set, new polygons are full ones.

--unique-names

If set, you will not be permitted to change the name of an component to match that of another component.

--snap-pin

If set, pin centers and pad end points are treated as additional grid points that the cursor can snap to.

--all-direction-lines

Allow all directions, when drawing new lines.

--show-number

Pinout shows number.

7.3 GTK+ GUI Options

--listen

Listen for actions on stdin.

--bg-image <string>

File name of an image to put into the background of the GUI canvas. The image must be a color PPM image, in binary (not ASCII) format. It can be any size, and will be automatically scaled to fit the canvas.

--pcb-menu <string>

Location of the gpcb-menu.res file which defines the menu for the GTK+ GUI.

7.4 lesstif GUI Options

--listen

Listen for actions on stdin.

--bg-image <string>

File name of an image to put into the background of the GUI canvas. The image must be a color PPM image, in binary (not ASCII) format. It can be any size, and will be automatically scaled to fit the canvas.

--pcb-menu <string>

Location of the pcb-menu.res file which defines the menu for the lesstif GUI.

7.5 Colors

--black-color <string>

Color value for black. Default: ‘#000000’

--black-color <string>

Color value for white. Default: ‘#ffffff’

--background-color <string>

Background color of the canvas. Default: ‘#e5e5e5’

--crosshair-color <string>

Color of the crosshair. Default: ‘#ff0000’

--cross-color <string>

Color of the cross. Default: ‘#cdcd00’

--via-color <string>

Color of vias. Default: ‘#7f7f7f’

--via-selected-color <string>

Color of selected vias. Default: ‘#00ffff’

--pin-color <string>

Color of pins. Default: ‘#4d4d4d’

--pin-selected-color <string>

Color of selected pins. Default: ‘#00ffff’

--pin-name-color <string>

Color of pin names and pin numbers. Default: ‘#ff0000’

--element-color <string>

Color of components. Default: ‘#000000’

--rat-color <string>

Color of ratlines. Default: ‘#b8860b’

--invisible-objects-color <string>

Color of invisible objects. Default: ‘#cccccc’

--invisible-mark-color <string>

Color of invisible marks. Default: ‘#cccccc’

--element-selected-color <string>

Color of selected components. Default: ‘#00ffff’

--rat-selected-color <string>

Color of selected rats. Default: ‘#00ffff’

--connected-color <string>

Color to indicate physical connections. Default: ‘#00ff00’

--found-color <string>

Color to indicate logical connections. Default: ‘#ff00ff’

--off-limit-color <string>

Color of off-canvas area. Default: ‘#cccccc’

--grid-color <string>

Color of the grid. Default: ‘#ff0000’

--layer-color-<n> <string>

Color of layer <n>, where <n> is an integer from 1 to 16.

--layer-selected-color-<n> <string>

Color of layer <n>, when selected. <n> is an integer from 1 to 16.

--warn-color <string>

Color of offending objects during DRC. Default value is "#ff8000"

--mask-color <string>

Color of the mask layer. Default value is "#ff0000"

7.6 Layer Names

--layer-name-1 <string>

Name of the 1st Layer. Default is "top".

--layer-name-2 <string>

Name of the 2nd Layer. Default is "ground".

--layer-name-3 <string>

Name of the 3nd Layer. Default is "signal2".

--layer-name-4 <string>

Name of the 4rd Layer. Default is "signal3".

--layer-name-5 <string>

Name of the 5rd Layer. Default is "power".

--layer-name-6 <string>

Name of the 6rd Layer. Default is "bottom".

--layer-name-7 <string>

Name of the 7rd Layer. Default is "outline".

--layer-name-8 <string>

Name of the 8rd Layer. Default is "spare".

7.7 Paths

--lib-newlib <string>

Top level directory for the newlib style library.

--lib-name <string>

The default filename for the library.

--default-font <string>

The name of the default font.

--file-path <string>

A colon separated list of directories or commands (starts with ’|’). The path is passed to the program specified in --file-command together with the selected filename.

--font-path <string>

A colon separated list of directories to search the default font. Defaults to the default library path.

--lib-path <string>

A colon separated list of directories that will be passed to the commands specified by --element-command and --element-contents-command.

7.8 Sizes

All parameters should be given with an unit. If no unit is given, 1/100 mil (cmil) will be used. Write units without space to the number like 3mm, not 3 mm. Valid Units are:

‘km’

Kilometer

‘m’

Meter

‘cm’

Centimeter

‘mm’

Millimeter

‘um’

Micrometer

‘nm’

Nanometer

‘in’

Inch (1in = 0.0254m)

‘mil’

Mil (1000mil = 1in)

‘cmil’

Centimil (1/100 mil)

--via-thickness <num>

Default diameter of vias. Default value is 60mil.

--via-drilling-hole <num>

Default diameter of holes. Default value is 28mil.

--via-solder-mask-clerance <num>

Default soldermask clearance around vias. Default value is 0mil.

--line-thickness <num>

Default thickness of new lines. Default value is 10mil.

--rat-thickness <num><unit>

Thickness of rats. If no unit is given, PCB units are assumed (i.e. 100 means "1 nm"). This option allows for a special unit px which sets the rat thickness to a fixed value in terms of screen pixels. Maximum fixed thickness is 100px. Minimum saling rat thickness is 101nm. Default value is 10mil.

--keepaway <num>

Default minimum distance between a track and adjacent copper. Default value is 10mil.

--default-PCB-width <num>

Default width of the canvas. Default value is 6000mil.

--default-PCB-height <num>

Default height of the canvas. Default value is 5000mil.

--text-scale <num>

Default text scale. This value is in percent. Default value is 100.

--alignment-distance <num>

Specifies the distance between the board outline and alignment targets. Default value is 2mil.

--grid <num>

Initial grid size. Default value is 10mil.

--minimum polygon area <num>

Minimum polygon area.

--paste-adjust <num>

Adjust pad thickness in paste layer. Default value is 0. Shrinking the pads is done with a negative amount.

Example:

pcb -x gerber --paste-adjust -0.07mm filename.pcb

7.9 Commands

pcb uses external commands for input output operations. These commands can be configured at start-up to meet local requirements. The command string may include special sequences %f, %p or %a. These are replaced when the command is called. The sequence %f is replaced by the file name, %p gets the path and %a indicates a package name.

--font-command <string>

Command to load a font.

--file-command <string>

Command to read a file.

--element-command <string>

Command to read a footprint.
Defaults to "M4PATH='%p';export M4PATH;echo 'include(%f)' | m4"

--print-file <string>

Command to print to a file.

--lib-command-dir <string>

Path to the command that queries the library.

--lib-command <string>

Command to query the library.
Defaults to "QueryLibrary.sh '%p' '%f' %a"

--lib-contents-command <string>

Command to query the contents of the library.
Defaults to "ListLibraryContents.sh %p %f" or, on Windows builds, an empty string (to disable this feature).

--save-command <string>

Command to save to a file.

--rat-command <string>

Command for reading a netlist. Sequence %f is replaced by the netlist filename.

7.10 DRC Options

All parameters should be given with an unit. If no unit is given, 1/100 mil (cmil) will be used for backward compability. Valid units are given in section Sizes.

--bloat <num>

Minimum spacing. Default value is 10mil.

--shrink <num>

Minimum touching overlap. Default value is 10mil.

--min-width <num>

Minimum width of copper. Default value is 10mil.

--min-silk <num>

Minimum width of lines in silk. Default value is 10mil.

--min-drill <num>

Minimum diameter of holes. Default value is 15mil.

--min-ring <num>

Minimum width of annular ring. Default value is 10mil.

7.11 BOM Creation

--bomfile <string>

Name of the BOM output file. Parameter <string> can include a path.

--xyfile <string>

Name of the XY output file. Parameter <string> can include a path.

--attrs <string>

Name of the attributes input file. Parameter <string> can include a path. The input file can be any path, the format matches what gschem uses. One attribute per line, and whitespace is ignored. Example:

device
manufacturer
manufacturer_part_number
vendor
vendor_part_number

--xy-unit <unit>

Unit of XY dimensions. Defaults to mil. Parameter <unit> can be ‘km’, ‘m’, ‘cm’, ‘mm’, ‘um’, ‘nm’, ‘px’, ‘in’, ‘mil’, ‘dmil’, ‘cmil’, or ‘inch’.

7.12 BOM MarkDown Creation

--bom_md_file <string>

Name of the BOM MarkDown output file. Parameter <string> can include a path.

--attrs <string>

Name of the attributes input file. Parameter <string> can include a path. The input file can be any path, the format matches what gschem uses. One attribute per line, and whitespace is ignored. Example:

device
manufacturer
manufacturer_part_number
vendor
vendor_part_number

7.13 G-code Options

--basename <string>

File name prefix and suffix, layer names will be inserted before the suffix. Parameter <string> can include a path.

--measurement-unit <unit>

Measurement unit used in the G-code output. Defaults to mil. Parameter <unit> can be ‘km’, ‘m’, ‘cm’, ‘mm’, ‘um’, ‘nm’, ‘px’, ‘in’, ‘mil’, ‘dmil’, ‘cmil’, or ‘inch’.

--dpi <int>

Accuracy of the mill path generation in pixels/inch.

--safe-Z <real>

Safe Z for traverse movements of all operations.

--iso-mill-depth <real>

Isolation milling depth.

--iso-tool-diameter <real>

Isolation milling tool diameter.

--iso-tool-plunge <real>

Isolation milling feedrate when plunging into the material.

--iso-tool-feedrate <real>

Isolation milling feedrate.

--predrill

Whether to pre-drill all drill spots with the isolation milling tool. Drill depth is iso-mill-depth here. This feature eases and enhances accuracy of manual drilling.

--drill-depth <real>

Drilling depth.

--drill-feedrate <real>

Drilling feedrate.

--drill-mill

Whether to produce drill holes equal or bigger than the milling tool diameter with the milling tool. With the milling tool bigger holes can be accurately sized without changing the tool.

--outline-mill-depth <real>

Milling depth when milling the outline. Currently, only the rectangular extents of the board are milled, no polygonal outlines or holes.

--outline-tool-diameter <real>

Diameter of the tool used for outline milling.

--outline-mill-plunge <real>

Outline milling feedrate when plunging into the material.

--outline-mill-feedrate <real>

Outline milling feedrate.

--advanced-gcode

Whether to produce G-code for advanced interpreters, like using variables or drill cycles. Not all machine controllers understand this, but it allows better hand-editing of the resulting files.

7.14 Gerber Export

--gerberfile <string>

Gerber output file prefix. Parameter <string> can include a path.

--all-layers

Output contains all layers, even empty ones.

--verbose

Print file names and aperture counts on stdout.

--metric

Generate metric Gerber and drill files

--copy-outline <string>

Copy the outline onto other layers. Parameter <string> can be ‘none’, ‘mask’, ‘silk’ or ‘all’.

--name-style <string>

Naming style for individual gerber files. Parameter <string> can be ‘fixed’, ‘single’, ‘first’, ‘eagle’, ‘hackvana’ or ‘oshpark’.

7.15 Postscript Export

--psfile <string>

Name of the postscript output file. Can contain a path.

--drill-helper

Print a centering target in large drill holes.

--align-marks

Print alignment marks on each sheet. This is meant to ease alignment during exposure.

--outline

Print the contents of the outline layer on each sheet.

--mirror

Print mirror image.

--fill-page

Scale output to make the board fit the page.

--auto-mirror

Print mirror image of appropriate layers.

--ps-color

Postscript output in color.

--ps-bloat <num>

Amount to add to trace/pad/pin edges.

--ps-invert

Draw objects as white-on-black.

--media <media-name>

Size of the media, the postscript is fitted to. The parameter <media-name> can be any of the standard names for paper size: ‘A0’ to ‘A10’, ‘B0’ to ‘B10’, ‘Letter’, ‘11x17’, ‘Ledger’, ‘Legal’, ‘Executive’, ‘A-Size’, ‘B-size’, ‘C-Size’, ‘D-size’, ‘E-size’, ‘US-Business_Card’, ‘Intl-Business_Card’.

--psfade <num>

Fade amount for assembly drawings (0.0=missing, 1.0=solid).

--scale <num>

Scale value to compensate for printer sizing errors (1.0 = full scale).

--multi-file

Produce multiple files, one per page, instead of a single multi page file.

--xcalib <num>

Paper width. Used for x-Axis calibration.

--ycalib <num>

Paper height. Used for y-Axis calibration.

--drill-copper

Draw drill holes in pins / vias, instead of leaving solid copper.

--show-legend

Print file name and scale on printout.

7.16 Encapsulated Postscript Export

--eps-file <string>

Name of the encapsulated postscript output file. Can contain a path.

--eps-scale <num>

Scale EPS output by the parameter ‘num’.

--screen-layer-order

Export layers as shown on screen.

--monochrome

Convert output to monochrome.

--only-visible

Limit the bounds of the EPS file to the visible items.

7.17 PNG Options

--outfile <string>

Name of the file to be exported to. Parameter <string> can include a path.

--dpi

Scale factor in pixels/inch. Set to 0 to scale to size specified in the layout.

--x-max

Width of the png image in pixels. No constraint, when set to 0.

--y-max

Height of the png output in pixels. No constraint, when set to 0.

--xy-max

Maximum width and height of the PNG output in pixels. No constraint, when set to 0.

--screen-layer-order

Export layers in the order shown on screen.

--monochrome

Convert output to monochrome.

--only-visible

Limit the bounds of the exported PNG image to the visible items.

--use-alpha

Make the background and any holes transparent.

--fill-holes

Drill holes in pins/pads are filled, not hollow.

--format <string>

File format to be exported. Parameter <string> can be ‘PNG’, ‘GIF’, or ‘JPEG’.

--png-bloat <num><dim>

Amount of extra thickness to add to traces, pads, or pin edges. The parameter ‘<num><dim>’ is a number, appended by a dimension ‘mm’, ‘mil’, or ‘pix’. If no dimension is given, the default dimension is 1/100 mil.

--photo-mode

Export a photo realistic image of the layout.

--photo-flip-x

In photo-realistic mode, export the reverse side of the layout. Left-right flip.

--photo-flip-y

In photo-realistic mode, export the reverse side of the layout. Up-down flip.

--photo-mask-colour <colour>

In photo-realistic mode, export the solder mask as this colour. Parameter <colour> can be ‘green’, ‘red’, ‘blue’, ‘purple’, ‘black’, or ‘white’.

--photo-plating <colour>

In photo-realistic mode, export the exposed copper as though it has this type of plating. Parameter <colour> can be ‘tinned’, ‘gold’, ‘silver’, or ‘copper’.

--photo-silk-colour <colour>

In photo-realistic mode, export the silk screen as this colour. Parameter <colour> can be ‘white’, ‘black’, or ‘yellow’.

7.18 Nelma Options

--basename <string>

File name prefix.

--dpi <num>

Horizontal scale factor (grid points/inch).

--copper-height <num>

Copper layer height (um).

--substrate-height <num>

Substrate layer height (um).

--substrate-epsilon <num>

Substrate relative epsilon.

7.19 IPC-D-356 Netlist Export

--netlist-file <string>

Name of the IPC-D-356 Netlist output file. Parameter <string> can include a path.

7.20 gsvit Options

-- basename <string>

File name prefix.

--dpi <num>

Horizontal scale factor (grid points/inch).

7.21 lpr Printing Options

--lprcommand <string>

Command to use for printing. Defaults to lpr. This can be used to produce PDF output with a virtual PDF printer. Example:
--lprcommand "lp -d CUPS-PDF-Printer".

In addition, all Postscript Export options are valid.

8 X11 Interface

This chapter gives an overview about the additional X11 resources which are defined by Pcb as well as the defined action routines.

8.1 Non-Standard X11 Application Resources

In addition to the toolkit resources, Pcb defines the following resources:

‘absoluteGrid (boolean)’

Selects if either the grid is relative to the position where it has changed last or absolute, the default, to the origin (0,0).

‘alignmentDistance (dimension)’

Specifies the distance between the boards outline to the alignment targets.

‘allDirectionLines (boolean)’

Enables (default) or disables clipping of new lines to 45 degree angles.

‘backgroundImage (string)’

If specified, this image will be drawn as the background for the board. The purpose of this option is to allow you to use a scan of an existing layout as a prototype for your new layout. To do this, there are some limitations as to what this image must be. The image must be a PPM binary image (magic number ‘P6’). It must have a maximum pixel value of 255 or less (i.e. no 16-bit images). It must represent the entire board, as it will be scaled to fit the board dimensions exactly. Note that it may be scaled unevenly if the image doesn’t have the same aspect ratio of your board. You must ensure that the image does not use more colors than are available on your system (mostly this is for pseudo-color displays, like old 8-bit displays). For best results, I suggest the following procedure using The Gimp: Load your image (any type). Image->Scale if needed. Image->Colors->Curves and for each of Red, Green, and Blue channel move the lower left point up to about the 3/4 line (value 192). This will make your image pale so it doesn’t interfere with the traces you’ll be adding. Image->Mode->Indexed and select, say, 32 colors with Normal F-S dithering. File->Save As, file type by extension, use .ppm as the extension. Select Raw formatting.

‘backupInterval (int)’

Pcb has an automatic backup feature which saves the current data every n seconds. The default is 300 seconds. A value of zero disables the feature. The backup file is named /tmp/PCB.%i.backup by default (this may have been changed at compilation time via the BACKUP_NAME variable in globalconfig.h). %i is replaced by the process ID. See also, the command-line option –backup-interval.

‘Bloat (dimension)’

Specifies the minimum spacing design rule in mils.

‘connectedColor (color)’

All pins, vias, lines and rectangles which are selected during a connection search are drawn with this color. The default value is determined by XtDefaultForeground.

‘cross hairColor (color)’

This color is used to draw the cross hair cursor. The color is a result of a XOR operation with the contents of the Layout area. The result also depends on the default colormap of the X11 server because only the colormap index is used in the boolean operation and Pcb doesn’t create its own colormap. The default setting is XtDefaultForeground.

‘elementColor (color)’

‘elementSelectedColor (color)’

The elements package part is drawn in these colors, for normal and selected mode, respectively, which both default to XtDefaultForeground.

‘elementCommand (string)’

Pcb uses a user defined command to read element files. This resource is used to set the command which is executed by the users default shell. Two escape sequences are defined to pass the selected filename (%f) and the current search path (%p). The command must write the element data to its standard output. The default value is

    M4PATH="%p";export M4PATH;echo 'include(%f)' | m4

Using the GNU version of m4 is highly recommended. See also, the command-line option –element-command.

‘elementPath (string)’

A colon separated list of directories or commands (starts with ’|’). The path is passed to the program specified in elementCommand together with the selected element name. A specified command will be executed in order to create entries for the fileselect box. It must write its results to stdout one entry per line. See also, the user-command le[!].

‘fileCommand (string)’

The command is executed by the user’s default shell whenever existing layout files are loaded. Data is read from the command’s standard output. Two escape sequences may be specified to pass the selected filename (%f) and the current search path (%p). The default value is:

    cat %f

See also, the command-line option –file-command.

‘filePath (string)’

A colon separated list of directories or commands (starts with ’|’). The path is passed to the program specified in fileCommand together with the selected filename. A specified command will be executed in order to create entries for the fileselect box. It must write its results to stdout one entry per line. See also, the user-command l[!].

‘fontCommand (string)’

Loading new symbol sets also is handled by an external command. You again may pass the selected filename and the current search path by passing %f and %p in the command string. Data is read from the commands standard output. This command defaults to

    cat %f

See also, the command-line option –font-command.

‘fontFile (string)’

The default font for new layouts is read from this file which is searched in the directories as defined by the resource fontPath. Searching is only performed if the filename does not contain a directory component. The default filename is default_font.

‘fontPath (string)’

This resource, a colon separated list of directories, defines the searchpath for font files. See also, the resource fontFile.

‘grid (int)’

This resource defines the initial value of one cursor step. It defaults to 100 mil and any changes are saved together with the layout data.

‘gridColor (color)’

This color is used to draw the grid. The color is a result of a INVERT operation with the contents of the Layout area. The result also depends on the default colormap of the X11 server because only the colormap index is used in the boolean operation and Pcb doesn’t create its own colormap. The default setting is XtDefaultForeground.

‘invisibleObjectsColor (color)’

Elements located on the opposite side of the board are drawn in this color. The default is XtDefaultForeground.

‘layerColor1..MAX_LAYER (color)’

‘layerSelectedColor1..MAX_LAYER (color)’

These resources define the drawing colors of the different layers in normal and selected state. All values are preset to XtDefaultForeground.

‘layerGroups (string)’

The argument to this resource is a colon separated list of comma separated layer numbers (1..MAX_LAYER). All layers within one group are switched on/off together. The default setting is 1:2:3:...:MAX_LAYER which means all layers are handled separately. Grouping layers one to three looks like 1,2,3:4:...:MAX_LAYER

‘layerName1..MAX_LAYER (string)’

The default name of the layers in a new layout are determined by these resources. The defaults are empty strings.

‘libraryCommand (string)’

Pcb uses a command to read element data from libraries. The resource is used to set the command which is executed by the users default shell. Three escape sequences are defined to pass the selected filename (%f), the current search path (%p) as well (%a) as the three parameters template, value and package to the command. It must write the element data to its standard output. The default value is

    NONE/share/pcb/oldlib/QueryLibrary.sh %p %f %a

‘libraryContentsCommand (string)’

Similar to libraryCommand, Pcb uses the command specified by this resource to list the contents of a library.

	NONE/share/pcb/oldlib/ListLibraryContents.sh %p %f

is the default.

‘libraryFilename (string)’

The resource specifies the name of the library. The default value is pcblib unless changed at compile time with the LIBRARYFILENAME variable in globalconfig.h.

‘libraryPath (string)’

A colon separated list of directories that will be passed to the commands specified by elementCommand and elementContentsCommand.

‘lineThickness (dimension)’

The value, in the range [1..250] (the range may be changed at compile time with the MIN_LINESIZE and MAX_LINESIZE variables in globalconfig.h), defines the initial thickness of new lines. The value is preset to ten mil.

‘media (<predefined> | <width>x<height>+-<left_margin>+-<top_margin>)’

The default (user defined) media of the PostScript device. Predefined values are a3, a4, a5, letter, tabloit, ledger, legal, and executive. The second way is to specify the medias width, height and margins in mil. The resource defaults to a4 size unless changed at compile time with the DEFAULT_MEDIASIZE variable in globalconfig.h.

‘offLimitColor (color)’

The area outside the current maximum settings for width and height is drawn with this color. The default value is determined by XtDefaultBackground.

‘pinColor (color)’

‘pinSelectedColor(color)’

This resource defines the drawing color of pins and pads in both states. The values are preset to XtDefaultForeground.

‘pinoutFont (string)’

This fonts are used to display pin names. There is one font for each zoom value. The values are preset to XtdefaultFont.

‘pinoutNameLength (int)’

This resource limits the number of characters which are displayed for pin names in the pinout window. By default the string length is limited to eight characters per name.

‘pinoutOffsetX (int)’

‘pinoutOffsetY (int)’

These resources determine the offset in mil of the circuit from the upper left corner of the window when displaying pinout information. Both default to 100 mil.

‘pinoutTextOffsetX (int)’

‘pinoutTextOffsetY (int)’

The resources determine the distance in mil between the drilling hole of a pin to the location where its name is displayed in the pinout window. They default to X:50 and Y:0.

‘pinoutZoom (int)’

Sets the zoom factor for the pinout window according to the formula: scale = 1:(2 power value). Its default value is two which results in a 1:4 scale.

‘printCommand (string)’

Default file for printouts. If the name starts with a ’|’ the output is piped through the command. A %f is replaced by the current filename. There is no default file or command.

‘raiseLogWindow (boolean)’

The log window will be raised when new messages arrive if this resource is set true, the default.

‘ratCommand (string)’

Default command for reading a netlist. A %f is replaced by the netlist filename. Its default value is "cat %f".

‘ratPath (string)’

Default path to look for netlist files. It’s default value is "."

‘resetAfterElement (boolean)’

If set to true, all found connections will be reset before a new element is scanned. This will produce long lists when scanning the whole layout for connections. The resource is set to false by default. The feature is only used while looking up connections of all elements.

‘ringBellWhenFinished (boolean)’

Whether to ring the bell (the default) when a possibly lengthy operation has finished or not. See also, the command-line option –ring-bell-finished.

‘routeStyle (string)’

Default values for the menu of routing styles (seen in the sizes menu). The string is a comma separated list of name, line thickness, via diameter, and via drill size. e.g. "Fat,50,100,40:Skinny,8,35,20:75Ohm,110,110,20" See also, the command-line option –route-styles and Sizes Menu

‘rubberBandMode (boolean)’

Whether rubberband move and rotate (attached lines stretch like rubberbands) is enabled (the default).

‘saveCommand (string)’

This command is used to save data to a layout file. The filename may be indicated by placing %f in the string. It must read the data from its standard input. The default command is:

    cat - > %f

See also, the command-line option –save-command.

‘saveInTMP (boolean)’

Enabling this resource will save all data which would otherwise be lost in a temporary file /tmp/PCB.%i.save. The file name may be changed at compile time with the EMERGENCY_NAME variable in globalconfig.h. . %i is replaced by the process ID. As an example, loading a new layout when the old one hasn’t been saved would use this resource. See also, the command-line option –save-in-tmp.

‘saveLastCommand (boolean)’

Enables the saving of the last entered user command. The option is disabled by default. See also, the command-line option –save-last-command.

‘Shrink (dimension)’

Specifies the minimum overlap (touching) design rule in mils.

‘size (<width>x<height>)’

Defines the width and height of a new layout. The default is 7000x5000 unless changed at compile time with the DEFAULT_SIZE variable in globalconfig.h.

‘stipllePolygons (boolean)’

Determines whether to display polygons on the screen with a stippled pattern. Stippling can create some amount of transparency so that you can still (to some extent) see layers beneath polygons. It defaults to False.

‘textScale (dimension)’

The font scaling in percent is defined by this resource. The default is 100 percent.

‘useLogWindow (boolean)’

Several subroutines send messages to the user if an error occurs. This resource determines if they appear inside the log window or as a separate dialog box. See also, the resource raiseLogWindow and the command line option -loggeometry. The default value is true.

‘viaColor (color)’

‘viaSelectedColor (color)’

This resource defines the drawing color of vias in both states. The values are preset to XtDefaultForeground.

‘viaThickness (dimension)’

‘viaDrillingHole (dimension)’

The initial thickness and drilling hole of new vias. The values must be in the range [30..400] (the range may be changed at compile time with the MIN_PINORVIASIZE and MAX_PINEORVIASIZE variables in globalconfig.h), with at least 20 mil of copper. The default thickness is 40 mil and the default drilling hole is 20 mil.

‘volume (int)’

The value is passed to XBell() which sets the volume of the X speaker. The value lies in the range -100..100 and it defaults to the maximum volume of 100.

‘warnColor (color)’

This resource defines the color to be used for drawing pins and pads when a warning has been issued about them.

‘zoom (int)’

The initial value for output scaling is set according to the following formula: scale = 1:(2 power value). It defaults to three which results in an output scale of 1:8.

Refer also to Command-Line Options.

8.2 Actions

All user accessible commands may be bound to almost any X event. Almost no default binding for commands is done in the binaries, so it is vital for the application that at least a system-wide application resource file exists. This file normally resides in the share/pcb directory and is called Pcb. The bindings to which the manual refers to are the ones as defined by the shipped resource file. Besides binding an action to an X11 event, you can also execute any action command using a ":" command (see User Commands).

Take special care about translations related to the functions keys and the pointer buttons because most of the window managers use them too. Change the file according to your hardware/software environment. You may have to replace all occurrences of baseTranslations to translations if you use a X11R4 server.

Passing Object as an argument to an action routine causes the object at the cursor location to be changed, removed or whatever. If more than one object is located at the cross hair position the smallest type is used. If there are two of the same type the newer one is taken. SelectedObjects will handle all selected and visible objects.

‘AddRats(AllRats|SelectedRats)’

Adds rat-lines to the layout using the loaded netlist file (see the :rn, User Commands.). Rat lines are added on the active layer using the current line thickness shown in the status line. Only missing connectivity is added by the AddRats command so if, for example, the layout is complete nothing will be added. Rat lines may be drawn different to other lines on the screen to make them easier to identify since they cannot appear in a completed layout. The rat-lines are added in the minimum length straight-line tree pattern (always ending on pins or pads) that satisfies the missing connectivity in the circuit. If a SMD pad is unreachable on the active layer, a warning will be issued about it and the rat-line to that pad will not be generated. If connections exist on the board which are not listed in the netlist while AllRats are being added, warning messages will be issued and the affected pins and pads will be drawn in a special warnColor until the next Notify() event. If the entire layout agrees completely with the net-list a message informs you that the layout is complete and no rat-lines are added (since none are needed). If SelectedRats is passed as the argument, only those missing connections that might connect among the selected pins and pads are drawn. Default:

None<Key>w:	AddRats(AllRats)
!Shift<Key>w:	AddRats(SelectedRats)
None<Key>o:	DeleteRats(AllRats) AddRats(AllRats)
!Shift<Key>o:	DeleteRats(SelectedRats) AddRats(SelectedRats)

‘ApplyVendor()’

Applies an already loaded vendor drill map to the design.

ApplyVendor()

‘Atomic(Save|Restore|Block|Close)’

Controls the undo grouping of sequences of actions. Before the first action in a group, Atomic(Save) should be issued. After each action that might be undoable, Atomic(Restore) should be issued. Atomic(Block) concludes and save the undo grouping if there was anything in the group to undo. Atomic(Close) concludes and save the undo grouping even if nothing was actually done. Thus it might produce an "empty" undo. This can be useful when you want to use undo in a group of actions.

‘Bell([-100..100])’

Rings the bell of your display. If no value is passed the setting of the resource volume will be used.

‘ChangeClearSize(Object, value[, unit])’

‘ChangeClearSize(SelectedPins|SelectedVias, value[, unit])’

The effect of this action depends on if the soldermask display is presently turned on or off. If soldermask is displayed, then the soldermask relief size will be changed. If soldermask display is turned off, then the clearance to polygons will be changed. unit is "mil" or "mm". If not specified the units will default to the internal unit of 0.01 mil.

!Mod1<Key>k:      ChangeClearSize(Object, +2, mil)
!Mod1 Shift<Key>k: ChangeClearSize(Object, -2, mil)

‘ChangeDrillSize(Object, value[, unit])’

‘ChangeDrillSize(SelectedPins|SelectedVias, value[, unit])’

This action routine changes the drilling hole of pins and vias. If value starts with + or -, then it adds (or subtracts) value from the current hole diameter, otherwise it sets the diameter to the value. unit is "mil" or "mm". If not specified the units will default to the internal unit of 0.01 mil. Default:

!Mod1<Key>s:       Change2ndSize(Object, +5, mil)
!Mod1 Shift<Key>s: Change2ndSize(Object, -5, mil)

‘ChangeFlag(Object|SelectElements|SelectedPins|SelectedVias|Selected,thermal|octagon|square,0|1)’

Sets/clears the indicated flag. This adds/removes thermals, adds/removes the flag which indicates a pin/pad should be square, or adds/removes the flag which indicates a pin/pad should be octagonal.

:ChangeFlag(SelectedVias,thermal,1)
:ChangeFlag(SelectedPads,square,0)

‘ChangeHole(Object|SelectedVias)’

This action routine converts a via to and from a hole. A hole is a via that has no copper annulus. The drill size for the via determines the hole diameter.

!Ctrl<Key>h:	ChangeHole(Object)

‘ChangeName(Object)’

‘ChangeName(Layer|Layout)’

Changes the name of the visible object at the cursor location. A text object doesn’t have a name therefore the text string itself is changed. The element name currently used for display is always the one changed with this command. See Display(Description|NameOnPCB|Value) for details. Passing Layer changes the current layers name. Default:

None<Key>n: ChangeName(Object)

‘ChangeOctagon(Object|SelectElements|SelectedPins|SelectedVias|Selected)’

Toggles what shape the affected pin(s) or via(s) will be drawn when they are not square. The shape will either be round or octagonal. Default:

!Ctrl<Key>o: ChangeOctagon(Object)

‘ChangePinName(ElementName, PinNumber, PinName)’

Changes the name for a specified pin or pad number on a specified element. This action is typically used to forward annotate pin/pad names from a schematic to the layout.

ChangePinName(U1, 14, VDD)

‘ChangeSize(Object, value[, unit])’

‘ChangeSize(SelectedLines|SelectedPins|SelectedVias, value[, unit])’

‘ChangeSize(SelectedPads|SelectedTexts|SelectedNames, value[, unit])’

‘ChangeSize(SelectedElements, value[, unit])’

To change the size of an object you have to bind these action to some X event (or use :ChangeSize(...)). If value begins with a + or - then the value will be added (or subtracted) from the current size, otherwise the size is set equal to value. Range checking is done to insure that none of the maximum/minimums of any size are violated. If Object is passed then a single object at the cursor location is changed. If any of the Selected arguments are passed then all selected and visible objects of that type are changed. If the type being modified is an element, then the thickness of the silkscreen lines defining the element is changed. unit is "mil" or "mm". If not specified the units will default to the internal unit of 0.01 mil. Default:

None<Key>s:   ChangeSize(Object, +5)
!Shift<Key>s: ChangeSize(Object, -5)

‘ChangeSquare(Object|SelectedElements|SelectedPins)’

Toggles the setting of the square flag. The flag is used to identify a certain pin, normally the first one, of circuits. It is also used to make SMD pads have square ends.

None<Key>q:   ChangeSquare(Object)

‘ClrFlag(Object|SelectElements|SelectedPins|SelectedVias|Selected,thermal|octagon|square)’

Clears the indicated flag. This removes thermals, removes the flag which indicates a pin/pad should be square, or removes the flag which indicates a pin/pad should be octagonal.

:ClrFlag(SelectedVias,thermal)

‘Command()’

Calling Command() pops up an input line at the bottom of the window which allows you to enter commands. Including all action commands! The dialog ends when None<Key>Return to confirm or None<Key>Escape to abort is entered. Default:

<Key>colon: Command()

‘Connection(Find)’

‘Connection(ResetFoundLinesAndRectangles|ResetPinsViasAndPads|Reset)’

The Connection() action is used to mark all connections from one pin, line or via to others. The ResetFoundLinesAndRectangles, ResetFoundPinsAndVias and Reset arguments may be used to reset all marked lines and rectangles, vias and pins or all of them. The search starts with the pin or via at the cursor position. All found objects are drawn with the color defined by the resource connectedColor. See also, Display(Description|NameOnPCB|Value). Default:

!Shift<Key>c: Connection(Reset)
None<Key>f:   Connection(Find)
!Shift<Key>f: Connection(Reset)

‘DeleteRats(AllRats|SelectedRats)’

This routine deletes either all rat-lines in the layout, or only the selected and visible ones. Non-rat-lines and other layout objects are unaffected. Default:

None<Key>e:   DeleteRats(AllRats)
!Shift<Key>e: DeleteRats(SelectedRats)

‘DisableVendor()’

Disables automatic drill size mapping to the loaded vendor drill table.

DisableVendor()

‘DisperseElements(All|Selected)’

Disperses either all elements or only the selected elements in the layout. This action should be used at the start of a design to spread out all footprints before any placement or routing is done.

DisperseElements(All)

‘Display(Description|NameOnPCB|Value)’

‘Display(Toggle45Degree|CycleClip)’

‘Display(Grid|ToggleGrid)’

‘Display(ToggleRubberBandMode)’

‘Display(Center|ClearAndRedraw|Redraw)’

‘Display(Pinout|PinOrPadName)’

This action routines handles some output related settings. It is used to center the display around the cursor location and to redraw the output area optionally after clearing the window. Centering is done with respect to the grid setting. Displaying the grid itself may be switched on and off by Grid but only if the distance between two pixels exceeds 4 pixels. Pcb is able to handle several labels of an element. One of them is a description of the functionality (eg resistor), the second should be a unique identifier (R1) whereas the last one is a value (100k). The Display() action selects which of the names is displayed. It also controls which name will be affected by the ChangeName command. If ToggleGrid is passed, Pcb changes between relative (’rel’ in the statusline) and absolute grid (an ’abs’ in the statusline). Relative grid means the pointer position when the command is issued is used as the grid origin; while (0,0) is used in the absolute grid case. Passing Pinout displays the pinout of the element at the current cursor location whereas PinOrPadName toggles displaying of the pins or pads name under the cursor. If none of them matches but the cursor is inside of an element, the flags is toggled for all of its pins and pads. For details about rubberbands see also the details about Mode. Default:

None<Key>c:  Display(Center)
None<Key>d:  Display(PinOrPadName)
!Shift<Key>d: Display(Pinout)
None<Key>r:  Display(ClearAndRedraw)
None<Key>.:  Display(Toggle45Degree)
None<Key>/:  Display(CycleClip)

‘DRC()’

Initiates design rule checking of the entire layout. Must be repeated until no errors are found.

‘ExecuteFile(filename)’

Executes the PCB actions contained in the specified file. This can be used to automate a complex sequence of operations.

:ExecuteFile(custom.cmd)

The command file contains a list of PCB actions. Blank lines are ignored and lines starting with a # are treated as comment lines. For example

# This is a comment line
Display(Grid)
SetValue(Zoom,2)
DRC()

‘EditLayerGroups()’

Pops up a dialog box to edit the layergroup setting. The function is also available from the Objects menu. There are no defaults.

‘EnableVendor()’

Enables automatic drill size mapping to the loaded vendor drill table.

EnableVendor()

‘Load(ElementToBuffer|Layout|LayoutToBuffer|Nelist)’

This routine pops up a fileselect box to load layout, element data, or netlist. The passed filename for layout data is saved and may be reused. ElementToBuffer and LayoutToBuffer load the data into the current buffer. There are no defaults.

‘LoadVendor(vendorfile)’

Loads the specified vendor resource file.

LoadVendor(myvendor.res)

‘MarkCrosshair()’

This routine marks the current cursor location with an X, and then the cursor display shows both absolute position and position relative to the mark. If a mark is already present, this routine removes it and stops displaying relative cursor coordinates. Defaults:

!Ctrl<key>m:	MarkCrosshair()

‘Mode(Copy|InsertPoint|Line|Move|None|PasteBuffer|Polygon|Thermal)’

‘Mode(Remove|Rectangle|RubberbandMove|Text|Via)’

‘Mode(Cycle)’

‘Mode(Notify)’

‘Mode(Save|Restore)’

Switches to a new mode of operation. The active mode is displayed by a thick line around the matching mode selector button. Most of the functionality of Pcb is implemented by selecting a mode and calling Mode(Notify). The arguments Line, Polygon, Rectangle, Text and Via are used to create the appropriate object whenever Mode(Notify) is called. Some of them, such as Polygon, need more than one call for one object to be created. InsertPoint adds points to existing polygons or lines. Save and Restore are used to temporarily save the mode, switch to another one, call Mode(Notify) and restore the saved one. Have a look at the application resource file for examples. Copy and Move modes are used to change an object’s location and, optionally, to create a new one. The first call of Mode(Notify) attaches the object at the pointer location to the cross hair whereas the second one drops it to the layout. The rubberband version of move performs the move while overriding the current rubberband mode. Passing PasteBuffer attaches the contents of the currently selected buffer to the cross hair. Each call to Mode(Notify) pastes this contents to the layout. Mode(Cycle) cycles through the modes available in the mode-button pallet. Mode(None) switches all modes off. Default:

<Key>Escape:             Mode(None)
<Key>space:              Mode(Cycle)
None<Key>BackSpace:      Mode(Save) Mode(Remove) Mode(Notify) Mode(Restore)
None<Key>Delete:         Mode(Save) Mode(Remove) Mode(Notify) Mode(Restore)
None<Key>F1:             Mode(Via)
None<Key>F2:             Mode(Line)
None<Key>F3:             Mode(PasteBuffer)
None<Key>F4:             Mode(Rectangle)
None<Key>F5:             Mode(Text)
None<Key>F6:             Mode(Polygon)
None<Key>F7:             Mode(Thermal)
None<Key>F8:		 Mode(Arc)
None<Key>Insert:         Mode(InsertPoint)
None<Key>[:              Mode(Save) Mode(Move) Mode(Notify)
None<Key>]:              Mode(Notify) Mode(Restore)
None<Btn1>:          Mode(Notify)
!Shift Ctrl<Btn1>:   Mode(Save) Mode(Remove) Mode(Notify) Mode(Restore)
None<Btn2Down>:          Mode(Save) Mode(Move) Mode(Notify)
None<Btn2Up>:            Mode(Notify) Mode(Restore)
!Mod1<Btn2Down>:       Mode(Save) Mode(Copy) Mode(Notify)
!Mod1<Btn2Up>:         Mode(Notify) Mode(Restore)
Shift BTNMOD<Btn2Down>: Mode(Save) Mode(RubberbandMove) Mode(Notify)

‘MovePointer(delta_x, delta_y)’

With this function it is possible to move the cross hair cursor by using the cursor keys. The X server’s pointer follows because the necessary events are generated by Pcb. All movements are performed with respect to the currently set grid value. Default:

None<Key>Up:      MovePointer(0, -1)
!Shift<Key>Up:    MovePointer(0, -10)
None<Key>Down:    MovePointer(0, 1)
!Shift<Key>Down:  MovePointer(0, 10)
None<Key>Right:   MovePointer(1, 0)
!Shift<Key>Right: MovePointer(10, 0)
None<Key>Left:    MovePointer(-1, 0)
!Shift<Key>Left:  MovePointer(-10, 0)

‘MoveToCurrentLayer(Object|SelectedObjects)’

The function moves a single object at the cross hair location or all selected objects to the current layer. Elements are not movable by this function. They have to be deleted and replaced on the other side. If a line segment is moved and the movement would result in a loss of connectivity to another segment then via(s) are automatically added to maintain the connectivity.

None<Key>m:       MoveToCurrentLayer(Object)
!Shift<Key>m:     MoveToCurrentLayer(SelectedObjects)

‘New()’

Clear the current layout and starts a new one after entering its name. Refer to the resource backup for more information. No defaults.

‘PasteBuffer(AddSelected|Clear|1..5)’

‘PasteBuffer(Rotate, 1..3)’

‘PasteBuffer(Convert)’

This action routine controls and selects the pastebuffer as well as all cut-and-paste operations. Passing a buffer number selects one in of the range 1..5. The statusline is updated with the new number. Rotate performs a number of 90 degree counter clockwise rotations of the buffer contents. AddSelected as first argument copies all selected and visible objects into the buffer. Passing Clear removes all objects from the currently selected buffer. Convert causes the contents of the buffer (lines, arc, vias) to be converted into an element definition. Refer to Pastebuffer for examples. Default:

!Ctrl<Key>x:       PasteBuffer(Clear) PasteBuffer(AddSelected)
		   Mode(PasteBuffer)
!Shift Ctrl<Key>x: PasteBuffer(Clear) PasteBuffer(AddSelected)
		   RemoveSelected() Mode(PasteBuffer)
!Mod1<Key>c:       PasteBuffer(Clear) PasteBuffer(AddSelected)
!Mod1<key>x:       PasteBuffer(Clear) PasteBuffer(AddSelected)
		   RemoveSelected()
!Shift<Key>1:      PasteBuffer(1)
!Shift<Key>2:      PasteBuffer(2)
!Shift<Key>3:      PasteBuffer(3)
!Shift<Key>4:      PasteBuffer(4)
!Shift<Key>5:      PasteBuffer(5)
None<Key>F3:       Mode(PasteBuffer)

‘Polygon(Close|PreviousPoint)’

Polygons need a special action routine to make life easier. Calling Polygon(PreviousPoint) resets the newly entered corner to the previous one. The Undo action will call Polygon(PreviousPoint) when appropriate to do so. Close creates the final segment of the polygon. This may fail if clipping to 45 degree lines is switched on, in which case a warning is issued. Default:

None<Key>p:             Polygon(Close)
!Shift<Key>p:           Polygon(Close)

‘Print()’

Pops up a print control box that lets you select the output device, scaling and many more options. Each run creates all files that are supported by the selected device. These are mask files as well as drilling files, silk screens and so on. The table shows the filenames for all possible files:

	POSIX (extension)             8.3 filename
		---------------------------------------------
		*_componentmask.*             cmsk.*
		*_componentsilk.*             cslk.*
		*_soldermask.*                smsk.*
		*_soldersilk.*                sslk.*
		*_drill.*                     dril.*
		*_groundplane.*               gpl.*
		*_group[1..8].*     [..8].*

The output may be sent to a post-processor by starting the filename with the pipe ("|") character. Any "%f" in a command is replaced with the current filename. The function is available from the file menu. There are no defaults.

‘Quit()’

Quits the application after confirming the operation. Default:

<Message>WM_PROTOCOLS: Quit()

‘Redo()’

This routine allows you to recover from the last undo command. You might want to do this if you thought that undo was going to revert something other than what it actually did (in case you are confused about which operations are un-doable), or if you have been backing up through a long undo list and over-shoot your stopping point. Any change that is made since the undo in question will trim the redo list. For example if you add ten lines, then undo three of them you could use redo to put them back, but if you move a line on the board before performing the redo, you will lose the ability to "redo" the three "undone" lines. Default:

!Shift<Key>r:	Redo()

‘RemoveSelected()’

This routine removes all visible and selected objects. There are no defaults.

‘Report(Object|DrillReport)’

This routine pops up a dialog box describing the various characteristics of an object (or piece of an object such as a pad or pin) in the layout at the cursor position, or a report about all of the drill holes in the layout. There are no defaults.

‘RouteStyle(1|2|3|4)’

This routine copies the sizes corresponding to the numbered route style into the active line thickens, via diameter, and via drill size. Defaults:

!Ctrl<Key>1: RouteStyle(1)
...
!Ctrl<Key>NUM_STYLES: RouteStyle(NUM_STYLES)

The variable NUM_STYLES is set at compile time in globalconfig.h.

‘Save(Layout|LayoutAs)’

‘Save(AllConnections|AllUnusedPins|ElementConnections)’

Passing Layout saves the layout using the file from which it was loaded or, if it is a new layout, calls Save(LayoutAs) which queries the user for a filename. The values: AllConnections, AllUnusedPins and ElementConnections start a connection scan and save all connections, all unused pins or the connections of a single element to a file. There are no defaults.

‘Select(All|Block|Connection|ToggleObject)’

‘Select(ElementByName|ObjectByName|PadByName|PinByName)’

‘Select(TextByName|ViaByName)’

Toggles either the selection flag of the object at the cross hair position (ToggleObject) or selects all visible objects, all inside a rectangle or all objects which have been found during the last connection scan. The ByName functions use a Regular Expressions search, always case insensitive, to select the objects. Default:

None<Btn3Down>:  Select(ToggleObject)
None<Btn3Down>,None<Btn3Motion>: See resource file - this is complex

‘SetFlag(Object|SelectElements|SelectedPins|SelectedVias|Selected,thermal|octagon|square)’

Sets the indicated flag. This adds thermals, sets the flag which indicates a pin/pad should be square, or sets the flag which indicates a pin/pad should be octagonal.

:SetFlag(Selected,thermal)

‘SetValue(Grid|LineSize|TextScale|ViaDrillingHole|ViaSize|Zoom, value)’

Some internal values may be changed online by this function. The first parameter specifies which data has to be changed. The other one determines if the resource is set to the passed value, if value is specified without sign, or increments/decrements if it is specified with a plus or minus sign. The function doesn’t change any existing object only the initial values of new objects. Use the ChangeSize() and ChangeDrillSize() to change existing objects. Default:

None<Key>g:        SetValue(Grid, +5)
!Shift<Key>g:      SetValue(Grid, -5)
None<Key>l:        SetValue(LineSize, +5)
!Shift<Key>l:      SetValue(LineSize, -5)
None<Key>t:        SetValue(TextScale, +10)
!Shift<Key>t:      SetValue(TextScale, -10)
None<Key>v:        SetValue(ViaSize, +5)
!Shift<Key>v:      SetValue(ViaSize, -5)
!Mod1<Key>v:       SetValue(ViaDrillingHole, +5)
!Mod1 Shift<Key>v: SetValue(ViaDrillingHole, -5)
None<Key>z:        SetValue(Zoom, -1)
!Shift<Key>z:      SetValue(Zoom, +1)

‘SwapSides()’

This routine changes the board side you are viewing. Default:

None<Key>Tab:      SwapSides()

‘SwitchDrawingLayer(value)’

Makes layer number 1..MAX_LAYER the current one. Default:

None<Key>1:        SwitchDrawingLayer(1)
...
None<Key>MAX_LAYER:        SwitchDrawingLayer(MAX_LAYER)

‘ToggleHideName(Object|SelectedElements)’

Toggles whether the element’s name is displayed or hidden. If it is hidden you won’t see it on the screen and it will not appear on the silk layer when you print the layout.

None<Key>h:	ToggleHideName(Object)
!Shift<Key>h:	ToggleHideName(SelectedElements)

‘ToggleVendor()’

Toggles automatic drill size mapping to the loaded vendor drill table.

ToggleVendor()

‘ToggleVisibility(Layer)’

Toggles the visibility of the layer.

Mod1<Key>1:	ToggleVisibility(1)
Mod1<Key>2:	ToggleVisibility(2)
Mod1<Key>3:	ToggleVisibility(3)
Mod1<Key>4:	ToggleVisibility(4)

‘Undo()’

‘Undo(ClearList)’

The unlimited undo feature of Pcb allows you to recover from most operations that materially affect you work. Calling Undo() without any parameter recovers from the last (non-undo) operation. ClearList is used to release the allocated memory. ClearList is called whenever a new layout is started or loaded. See also Redo. Default:

None<Key>u:        Undo()
!Shift Ctrl<Key>u: Undo(ClearList)

‘UnloadVendor()’

Unloads the loaded vendor drill table.

UnloadVendor()

‘Unselect(All|Block|Connection)’

Unselects all visible objects, all inside a rectangle or all objects which have been found during the last connection scan. Default:

!Shift <Btn3Down>: Mode(Save) Mode(None) Unselect(Block)
!Shift <Btn3Up>:   Unselect(Block) Mode(Restore)

8.3 Default Translations

This section covers some default translations of key and button events as defined in the shipped default application resource file. Most of them have already been listed in Actions. Pcb makes use of a nice X11 feature; calling several action routines for one event.

‘None<Key>BackSpace:’

‘None<key>Delete:’

‘!Shift<Key>BackSpace:’

‘!Shift Ctrl<Btn1>:’

The object at the cursor location is removed by None<Key>BackSpace or Shift Ctrl<Btn1> whereas Shift<Key>BackSpace also removes all other objects that are fully-connected to the one at the cursor location.

‘!Mod1 Ctrl<Key>Left:’

‘!Mod1 Ctrl<Key>Right:’

‘!Mod1 Ctrl<Key>Up:’

‘!Mod1 Ctrl<Key>Down:’

Scroll one page in one of the four directions.

‘None<Key>Left:, !Shift<Key>Left:’

‘None<Key>Right:, !Shift<Key>Right:’

‘None<Key>Up:, !Shift<Key>Up:’

‘None<Key>Down:, !Shift<Key>Down:’

Move cross hair either one or ten points in grid.

‘None<Key>Return:’

Finished user input, selects the ’default’ button of dialogs.

‘None<Key>Escape:’

Mode(Reset), aborts user input, selects the ’abort’ button of dialogs or resets all modes.

‘None<Btn2Down>, Btn2<Motion>, None<Btn2Up>:’

‘!Mod1<Btn2Down>, Btn2<Motion>, !Mod1<Btn2Up>:’

The first sequence moves the object or element name at the cursor location. The second one copies the objects. Copying isn’t available for element names.

9 File Formats

All files used by Pcb are read from the standard output of a command or written to the standard input of one as plain seven bit ASCII. This makes it possible to use any editor to change the contents of a layout file. It is the only way for element or font description files to be created. To do so you’ll need to study the example files example/* and default_font which are shipped with Pcb. For an overview refer to Intro.

The following sections provide the necessary information about the syntax of the files. Netlist files are not created by Pcb, but it does use them. For information on the format of a netlist file see the :rn, User Commands. The commands described allow you to add almost any additional functionality you may need. Examples are compressed read and write access as well as archives. The commands themselves are defined by the resources elementCommand, fileCommand, fontCommand, libraryCommand, libraryContentsCommand and saveCommand. Note that the commands are not saved along with the data. It is considered an advantage to have the layout file contain all necessary information, independent of any other files.

One thing common to all files is they may include comments, newlines, and carriage returns at any place except within quoted strings.

9.1 Pad and Line Representation

Pads and lines (copper traces, silk screen lines, etc) are represented by the line end points and the aperture used to draw the line. It is important to understand this when creating the pads for a new footprint. The following figure illustrates a pad or line which is drawn using a square aperture. The end points (X0,Y0), (X1,Y1) specify the center of the aperture. The size parameter specifies the size of the aperture.

Pads and lines are represented in this way because this is how lines are specified in RS-274X (Gerber) files which are used for creating the masks used in board manufacturing. In fact, older mask making equipment created lines in precisely this fashion. A physical aperture was used to pass light through onto a photosensitive film.

There is an alternate representation of the pad - a pad can be specified as coordinates of its centerpoint and pad size. The pad is internally stored in traditional format. This format significantly simplifies the manual design of elements.

9.2 Layout File Format

The layout file describes a complete layout including symbols, vias, elements and layers with lines, rectangles and text. This is the most complex file of all. As Pcb has evolved, the file format has changed several times to accommodate new features. Pcb has always been able to read all older versions of the .pcb file. This allows the migration of older designs to newer versions of the program. Obviously older versions of Pcb will not be able to properly read layout files stored in newer versions of the file format.

In practice it is very common for footprint libraries to contain elements which have been defined in various versions of the Pcb file format. When faced with trying to understand an element file or layout file which includes syntax not defined here, the best approach is to examine the file src/parse_y.y which is the definitive definition of the file format.

The PCB layout file contains the following contents, in this order (individual items are defined in File Syntax):

PCB

This names the board and sets its size

Grid

Optional.

Cursor

Optional.

Flags

Optional.

Groups

Optional.

Styles

Optional.

Symbols

Optional.

Vias, Rats, Layers, and Elements

These may occur in any order, at this point in the file.

Netlists

Optional.

9.3 Element File Format

Element files are used to describe one component which then may be used several times within one or more layouts. You will normally split the file into two parts, one for the pinout and one for the package description. Using m4 allows you to define pin names as macros in one file and include a package description file which evaluates the macros. See the resource elementCommand for more information. The pins (and pads) must appear in sequential order in the element file (new in 1.5) so that pin 1 must be the first PIN(...) in the file.

Doing things this way makes it possible to use one package file for several different circuits. See the sample files dil*.

The lowest x and y coordinates of all sub-objects of an element are used as an attachment point for the cross hair cursor of the main window, unless the element has a mark, in which case that’s the attachment point.

9.4 Font File Format

A number of user defined Symbols are called a font. There is only one per layout. All symbols are made of lines. See the file default_font as an example.

A font file is simply a text file that contains the defined symbols making up the font. The font file text can be inserted into a layout file after the Styles definition.

If a layout file does not contain a font, component labels will be invisible, although component outlines, pins and pads will be visible.

The lowest x and y coordinates of all lines of a font are transformed to (0,0).

Font symbols are typically 4000mil high, and are rendered with SymbolLine primitives. Arcs and polygons are not supported in font symbols.

A typical symbol:

Symbol['"' 1200]
(
    SymbolLine[0 1000 0 2334 800]
    SymbolLine[1523 1000 1523 2334 800]
)

In the example above, 1200 indicates the intercharacter spacing required after the symbol, in this case the symbol is the double quote ’"’. The SymbolLine definitions define the lines making up the symbol as [x1 y1 x2 y2 linewidth]. Standard height symbols, such as the letter H or N, span 1000 to 5000 in the y axis, where 0,0 is at the upper left. Taller symbols, such as a bracket, may span 0 to 6000 in the y axis. Symbols for use as Pcb fonts can be generated from fonts intended for use in pen plotters or engravers, known as centerline fonts, or one stroke fonts. Outline fonts, such as TTF fonts, if converted to Pcb format, are usually converted into polygons which are incompatible with font symbol rendering.

A practical means by which a new font symbol can be created is to export the character as an Encapsulated Postscript (EPS) image, and run a utility such as pstoedit to convert to Pcb compatible line descriptions.

pstoedit artwork.eps -psarg "-r1000x1000" -f pcb artwork.pcb

The -r1000x1000 command makes the paths adhere to a 1000x1000 grid. The resulting artwork.pcb file can be used to create a font symbol. An efficient way to convert multiple symbols is to export an entire glyph table as EPS, run the pstoedit utility to create a PCB file with all of the font symbols of interest, and after loading the PCB file, select one font symbol at a time and save the PCB file using CTRL-S. In a console terminal:

cat artwork.pcb | grep "elected" > SelectedSymbol.txt

will extract the line descriptors for the selected symbol, which can then be used to create a font symbol, after extraction of the x1,y1,x2,y2 coordinates, followed by suitable scaling and translation of the coordinates.

A set of font symbols can be combined to create a font file.

9.5 Netlist File Format

Netlists read by Pcb must have this simple text form:

netname [style] NAME-PINNUM NAME2-PINNUM2 NAME3-PINNUM3 ... [\]

for each net on the layout. where "netname" is the name of the net which must be unique for each net, [style] is an optional route-style name, NAME is the layout-name name given to an element, and PINNUM is the (usually numeric) pin number of the element that connects to the net (for details on pin numbering see Element Objects). Spaces or tabs separate the fields. If the line ends with a "\" the net continues on the next line and the "\" is treated exactly as if it were a space. If a NAME ends with a lower-case letter, all lower-case letters are stripped from the end of the NAME to determine the matching layout-name name. For example:

     Data U1-3 U2abc-4 FLOP1a-7 Uabc3-A9

specifies that the net called "Data" should have pin 3 of U1 connected to pin 4 of U2, to pin 7 of FLOP1 and to pin A9 of Uabc3. Note that element name and pin number strings are case-sensitive. It is up to you to name the elements so that their layout-name names agrees with the netlist.

9.6 Library Contents File Format

There is nothing like a special library format. The ones that have been introduced in 1.4.1 just use some nice (and time consuming) features of GNU m4. The only predefined format is the one of the contents file which is read during startup. It is made up of two basic line types:

menu entry      = "TYPE="name
contents line   = template":"package":"value":"description
name            = String
template        = String
package         = String
value           = String
description     = String
String          = <anything except ":", "\n" and "\r">

No leading white spaces or comments are allowed in this file. If you need either one, define a command that removes them before loading. Have a look to the libraryContentsCommand resource.

The menu entry will appear in the selection menu at the top and of the library window.

9.7 Library File Format

This section provides an overview about the existing m4 definitions of the elements. There are basically two different types of files. One to define element specific data like the pinout, package and so on, the other to define the values. For example the static RAM circuits 43256 and 62256 are very similar. They therefore share a common definition in the macro file but are defined with two different value labels.

The macro file entry:

define(`Description_43256_dil', `SRAM 32Kx8')
define(`Param1_43256_dil', 28)
define(`Param2_43256_dil', 600)
define(`PinList_43256_dil', ``pin1', `pin2', ...')

And the list file:

43256_dil:N:43256:62256

The macro must define a description, the pin list and up to two additional parameters that are passed to the package definitions. The first one is the number of pins whereas the second one defines for example the width of a package.

It is very important to select a unique identifier for each macro. In the example this would be 43256_dil which is also the templates name. It is required by some low-level macros that Description_, Param1_, Param2_ and PinList_ are perpended.

The list file uses a syntax:

template:package:value[:more values]

This means that the shown example will create two element entries with the same package and pinout but with different names.

A number of packages are defined in common.m4. Included are:

DIL packages with suffix D, DW, J, JD, JG, N, NT, P
PLCC
TO3
generic connectors
DIN 41.612 connectors
zick-zack (SD suffix)
15 pin multiwatt

If you are going to start your own library please take care about m4 functions. Be aware of quoting and so on and, most important check your additional entry by calling the macro:

CreateObject(`template', `value', `package suffix')

If quoting is incorrect an endless loop may occur (broken by a out-of-memory message).

The scripts in the lib directory handle the creation of libraries as well as of their contents files. Querying is also supported.

I know quite well that this description of the library implementation is not what some out there expect. But in my opinion it’s much more useful to look at the comments and follow the macros step by step.

9.8 File Syntax

A special note about units: Older versions of pcb used mils (1/1000 inch) as the base unit; a value of 500 in the file meant half an inch. Newer versions uses a "high resolution" syntax, where the base unit is 1/100 of a mil (0.000010 inch); a value of 500 in the file means 5 mils. As a general rule, the variants of each entry listed below which use square brackets are the high resolution formats and use the 1/100 mil units, and the ones with parentheses are the older variants and use 1 mil units. Note that when multiple variants are listed, the most recent (and most preferred) format is the first listed.

The square bracket syntax specifies only the enclosed values as high resolution. Whenever child elements need high resolution, they have to use square brackets on their own, as in this example:

   Symbol['!' 12]                       # 12 is a high resolution value
   (  # <--- this pair is only for grouping and can never be a square
           SymbolLine[0 4500 0 5000 8]  # high resolution
           SymbolLine(0   10 0   35 8)  # standard resolution

Symbolic and numeric flags (SFlags and NFlags) are described in Object Flags.

9.8.1 Arc

Current syntax:

Arc [X Y RadiusX RadiusY Thickness Clearance StartAngle DeltaAngle SFlags]

Legacy syntax:

Arc (X Y RadiusX RadiusY Thickness Clearance StartAngle DeltaAngle NFlags)
Arc (X Y RadiusX RadiusY Thickness StartAngle DeltaAngle NFlags)

X Y

Coordinates of the center of the arc.

RadiusX RadiusY

The RadiusX and RadiusY, from the center to the edge (centerline of the trace). The bounds of the circle of which this arc is a segment, is thus 2*RadiusX by 2*RadiusY.

Thickness

The width of the copper trace which forms the arc.

Clearance

The amount of space cleared around the arc when the line passes through a polygon. The clearance is added to the thickness to get the thickness of the clear; thus the space between the arc and the polygon is Clearance/2 wide.

StartAngle

The angle of one end of the arc, in degrees. In PCB, an angle of zero points left (negative X direction), and 90 degrees points down (positive Y direction).

DeltaAngle

The sweep of the arc. This may be negative. Positive angles sweep counterclockwise.

SFlags

Symbolic or numeric flags.

NFlags

Numeric flags.

9.8.2 Attribute

Attribute ("Name" "Value")

Attributes allow boards and elements to have arbitrary data attached to them, which may or may not be used by PCB itself, but may be of use by other programs or users.

Name

The name of the attribute

Value

The value of the attribute. Values are always stored as strings, even if the value is interpreted as, for example, a number.

Below are some examples of global (board wide) attributes:

Attribute("PCB::grid::unit" "mil")

Attribute("PCB::grid::size" "39.37mil")

Attribute("PCB::grid::unit" "mm")

and some examples for attributes in an element (local):

Element["lock" "BGA676N100P26X26-2700X2700X260" "U?" "FG676" 20.0000mm 20.0000mm 0.0000 -631.49mil 0 100 ""]
(
	Attribute("author" "PCB Contributors")
	Attribute("dist-license" "GPL2")
	Attribute("use-license" "unlimited2")
	Attribute("status" "Experimental")
	Attribute("attributes in footprint" "1")
	Attribute("package body length" "27.000000")
	Attribute("package body width" "27.000000")
	Attribute("package height" "2.600000")

9.8.3 Connect

Connect ("PinPad")

PinPad

The name of a pin or pad which is included in this net. Pin and Pad names are named by the refdes and pin name, like "U14-7" for pin 7 of U14, or "T4-E" for pin E of T4.

9.8.4 Cursor

Legacy syntax:

Cursor [X Y Zoom]
Cursor (X Y Zoom)

X Y

Location of the cursor when the board was saved. As of November 2012 the cursor position is not written to file anymore. Older versions of pcb ignore the absence of this line in the pcb file.

Zoom

The current zoom factor. Note that a zoom factor of "0" means 1 mil per screen pixel, N means 2^N mils per screen pixel, etc. The first variant accepts floating point numbers. The special value "1000" means "zoom to fit"

This field is ignored by PCB.

9.8.5 DRC

DRC [Bloat Shrink Line Silk Drill Ring]
DRC [Bloat Shrink Line Silk]
DRC [Bloat Shrink Line]

Bloat

Minimum spacing between copper.

Shrink

Minimum copper overlap to guarantee connectivity.

Line

Minimum line thickness.

Silk

Minimum silk thickness.

Drill

Minimum drill size.

Ring

Minimum width of the annular ring around pins and vias.

9.8.6 Element

Current syntax:

Element [SFlags "Desc" "Name" "Value" MX MY TX TY TDir TScale TSFlags] (
   … contents …
)

Legacy syntax:

Element (NFlags "Desc" "Name" "Value" MX MY TX TY TDir TScale TNFlags) (
Element (NFlags "Desc" "Name" "Value" TX TY TDir TScale TNFlags) (
Element (NFlags "Desc" "Name" TX TY TDir TScale TNFlags) (
Element ("Desc" "Name" TX TY TDir TScale TNFlags) (
   … contents …
)

SFlags

Symbolic or numeric flags, for the element as a whole.

NFlags

Numeric flags, for the element as a whole.

Desc

The description of the element. This is one of the three strings which can be displayed on the screen.

Name

The name of the element, usually the reference designator.

Value

The value of the element.

MX MY

The location of the element’s mark. This is the reference point for placing the element and its pins and pads.

TX TY

The upper left corner of the text (one of the three strings).

TDir

The relative direction of the text. 0 means left to right for an unrotated element, 1 means up, 2 left, 3 down.

TScale

Size of the text, as a percentage of the “default” size of of the font (the default font is about 40 mils high). Default is 100 (40 mils).

TSFlags

Symbolic or numeric flags, for the text.

TNFlags

Numeric flags, for the text.

Elements may contain pins, pads, element lines, element arcs, attributes, and (for older elements) an optional mark. Note that element definitions that have the mark coordinates in the element line, only support pins and pads which use relative coordinates. The pin and pad coordinates are relative to the mark. Element definitions which do not include the mark coordinates in the element line, may have a Mark definition in their contents, and only use pin and pad definitions which use absolute coordinates.

9.8.7 ElementArc

Current syntax:

ElementArc [X Y Width Height StartAngle DeltaAngle Thickness]

Legacy syntax:

ElementArc (X Y Width Height StartAngle DeltaAngle Thickness)

X Y

Coordinates of the center of the arc. These are relative to the Element’s mark point for new element formats, or absolute for older formats.

Width Height

The width and height, from the center to the edge. The bounds of the circle of which this arc is a segment, is thus 2*Width by 2*Height.

StartAngle

The angle of one end of the arc, in degrees. In PCB, an angle of zero points left (negative X direction), and 90 degrees points down (positive Y direction).

DeltaAngle

The sweep of the arc. This may be negative. Positive angles sweep counterclockwise.

Thickness

The width of the silk line which forms the arc.

9.8.8 ElementLine

Current syntax:

ElementLine [X1 Y1 X2 Y2 Thickness]

Legacy syntax:

ElementLine (X1 Y1 X2 Y2 Thickness)

X1 Y1 X2 Y2

Coordinates of the endpoints of the line. These are relative to the Element’s mark point for new element formats, or absolute for older formats.

Thickness

The width of the silk for this line.

9.8.9 FileVersion

FileVersion[Version]

Version

File format version. This version number represents the date when the pcb file format was last changed.

Any version of pcb build from sources equal to or newer than this number should be able to read the file. If this line is not present in the input file then file format compatibility is not checked.

9.8.10 Flags

Flags(Number)

Number

A number, whose value is normally given in hex, individual bits of which represent pcb-wide flags as defined in PCBFlags.

9.8.11 Grid

Current syntax:

Grid [Step OffsetX OffsetY Visible]

Legacy syntax:

Grid (Step OffsetX OffsetY Visible)
Grid (Step OffsetX OffsetY)

Step

Distance from one grid point to adjacent points. This value may be a floating point number for the first two variants.

OffsetX OffsetY

The "origin" of the grid. Normally zero.

Visible

If non-zero, the grid will be visible on the screen.

9.8.12 Groups

Groups("String")

String

Encodes the layer grouping information. Each group is separated by a colon, each member of each group is separated by a comma. Group members are either numbers from 1..N for each layer, and the letters c or s representing the component side and solder side of the board. Including c or s marks that group as being the top or bottom side of the board.

Groups("1,2,c:3:4:5,6,s:7,8")

9.8.13 Layer

Layer (LayerNum "Name" "Flags") (
   … contents …
)

LayerNum

The layer number. Layers are numbered sequentially, starting with 1. The last two layers (9 and 10 by default) are solder-side silk and component-side silk, in that order. The two silk layers also mark top and bottom side; the layer group where the solder-side silk layer is member in is the solder side group. Analogous for the other side.

Name

The layer name.

For layout files predating layer flags the name also defines the layer type in some situations. For example, a layer named outline was considered to be the layer defining the extents of the board.

Flags

Layer flags. Currently this is the layer type, like copper, silk or outline. For a complete list see layertype_name[] in layerflags.c.

With layer flags missing, the type of layer is guessed at load time, mostly by the layer name. This mechanism ensures compatibility with older layouts.

contents

The contents of the layer, which may include attributes, lines, arcs, rectangles, text, and polygons.

9.8.14 Line

Current syntax:

Line [X1 Y1 X2 Y2 Thickness Clearance SFlags]

Legacy syntax:

Line (X1 Y1 X2 Y2 Thickness Clearance NFlags)
Line (X1 Y1 X2 Y2 Thickness NFlags)

X1 Y1 X2 Y2

The end points of the line

Thickness

The width of the line

Clearance

The amount of space cleared around the line when the line passes through a polygon. The clearance is added to the thickness to get the thickness of the clear; thus the space between the line and the polygon is Clearance/2 wide.

SFlags

Symbolic or numeric flags

NFlags

Numeric flags.

9.8.15 Mark

Legacy syntax:

Mark [X Y]
Mark (X Y)

X Y

Coordinates of the Mark, for older element formats that don’t have the mark as part of the Element line.

9.8.16 Net

Net ("Name" "Style") (
   … connects …
)

Name

The name of this net.

Style

The routing style that should be used when autorouting this net.

9.8.17 Netlist

Netlist ( ) (
   … nets …
)

9.8.18 Pad

Current syntax:

Pad [rX1 rY1 rX2 rY2 Thickness Clearance Mask "Name" "Number" SFlags]
Pad [cX cY sX sY Clearance Mask "Name" "Number" SFlags]

Legacy syntax:

Pad (rX1 rY1 rX2 rY2 Thickness Clearance Mask "Name" "Number" NFlags)
Pad (cX cY sX sY Clearance Mask "Name" "Number" NFlags)
Pad (aX1 aY1 aX2 aY2 Thickness "Name" "Number" NFlags)
Pad (aX1 aY1 aX2 aY2 Thickness "Name" NFlags)

rX1 rY1 rX2 rY2

Coordinates of the endpoints of the pad, relative to the element’s mark. Note that the copper extends beyond these coordinates by half the thickness. To make a square or round pad, specify the same coordinate twice.

aX1 aY1 aX2 aY2

Same, but absolute coordinates of the endpoints of the pad.

cX cY sX sY

Coordinates of the pad centerpoint (cX, cY) and pad size (sX, sY).

Thickness

width of the pad.

Clearance

add to thickness to get clearance width.

Mask

width of solder mask opening.

Name

name of pin

Number

number of pin

SFlags

symbolic or numerical flags

NFlags

numerical flags only

9.8.19 PCB

Current syntax:

PCB ["Name" Width Height]

Legacy syntax:

PCB ("Name" Width Height)
PCB ("Name")

Name

Name of the PCB project

Width Height

Size of the board

If you don’t specify the size of the board, a very large default is chosen.

9.8.20 Pin

Current syntax:

Pin [rX rY Thickness Clearance Mask Drill "Name" "Number" SFlags]

Legacy syntax:

Pin (rX rY Thickness Clearance Mask Drill "Name" "Number" NFlags)
Pin (aX aY Thickness Drill "Name" "Number" NFlags)
Pin (aX aY Thickness Drill "Name" NFlags)
Pin (aX aY Thickness "Name" NFlags)

rX rY

coordinates of center, relative to the element’s mark

aX aY

absolute coordinates of center.

Thickness

outer diameter of copper annulus

Clearance

add to thickness to get clearance diameter

Mask

diameter of solder mask opening

Drill

diameter of drill

Name

name of pin

Number

number of pin

SFlags

symbolic or numerical flags

NFlags

numerical flags only

9.8.21 PolyArea

PolyArea [Area]

Area

Minimum area of polygon island to retain. If a polygon has clearances that cause an isolated island to be created, then will only be retained if the area exceeds this minimum area.

9.8.22 Polygon

Current syntax:

Polygon (SFlags) (
   … [X Y] …
   Hole (
      … [X Y] …
   )
   …
)

Legacy syntax:

Polygon (SFlags) (
   … (X Y) …
   Hole (
      … (X Y) …
   )
   …
)

SFlags

Symbolic or numeric flags.

X Y

Coordinates of each vertex. You must list at least three coordinates.

Hole (...)

Defines a hole within the polygon’s outer contour. There may be zero or more such sections.

9.8.23 Rat

Current syntax:

Rat [X1 Y1 Group1 X2 Y2 Group2 SFlags]

Legacy Syntax:

Rat (X1 Y1 Group1 X2 Y2 Group2 NFlags)

X1 Y1 X2 Y2

The endpoints of the rat line.

Group1 Group2

The layer group each end is connected on.

SFlags

Symbolic or numeric flags.

NFlags

Numeric flags.

9.8.24 Styles

Styles("String")

String

Encodes the four routing styles pcb knows about. The four styles are separated by colons. Each style consists of five parameters as follows:

Name

The name of the style.

Thickness

Width of lines and arcs.

Diameter

Copper diameter of pins and vias.

Drill

Drill diameter of pins and vias.

Keepaway

Minimum spacing to other nets. If omitted, 10 mils is the default.

Via Mask Aperture (optional)

The diameter of the solder mask opening around vias. A value of 0 produces a tented via. This parameter is omitted if 0 for backwards compatibility.

Current syntax example:

Styles["Logic,1000,3600,2000,1000,0:Power,2500,6000,3500,1000,70mil:
   Line,4000,6000,3500,1000:Breakout,600,2402,1181,600"]

Legacy syntax example:

Styles("Signal,10,40,20:Power,25,60,35:Fat,40,60,35:Skinny,8,36,20")

Note that strings in actual files cannot span lines; the above example is split across lines only to make it readable.

9.8.25 Symbol

Current syntax:

Symbol [Char Delta] (
   … symbol lines …
)

Legacy syntax:

Symbol (Char Delta) (
   … symbol lines …
)

Char

The character or numerical character value this symbol represents. Characters must be in single quotes.

Delta

Additional space to allow after this character.

9.8.26 SymbolLine

Current syntax:

SymbolLine [X1 Y1 X2 Y2 Thickness]

Legacy syntax:

SymbolLine (X1 Y1 X2 Y2 Thickness)

X1 Y1 X2 Y2

The endpoints of this line.

Thickness

The width of this line.

9.8.27 Text

Current syntax:

Text [X Y Direction Scale "String" SFlags]

Legacy syntax:

Text (X Y Direction Scale "String" NFlags)
Text (X Y Direction "String" NFlags)

X Y

The location of the upper left corner of the text.

Direction

0 means text is drawn left to right, 1 means up, 2 means right to left (i.e. upside down), and 3 means down.

Scale

Size of the text, as a percentage of the “default” size of of the font (the default font is about 40 mils high). Default is 100 (40 mils).

String

The string to draw.

SFlags

Symbolic or numeric flags.

NFlags

Numeric flags.

9.8.28 Thermal

Thermal [Scale]

Scale

Relative size of thermal fingers. A value of 1.0 makes the finger width twice the clearance gap width (measured across the gap, not diameter). The normal value is 0.5, which results in a finger width the same as the clearance gap width.

9.8.29 Via

Current syntax:

Via [X Y Thickness Clearance Mask Drill BuriedFrom BuriedTo "Name" SFlags]
Via [X Y Thickness Clearance Mask Drill "Name" SFlags]

Legacy syntax:

Via (X Y Thickness Clearance Mask Drill "Name" NFlags)
Via (X Y Thickness Clearance Drill "Name" NFlags)
Via (X Y Thickness Drill "Name" NFlags)
Via (X Y Thickness "Name" NFlags)

X Y

coordinates of center

Thickness

outer diameter of copper annulus

Clearance

add to thickness to get clearance diameter

Mask

diameter of solder mask opening

Drill

diameter of drill

BuriedFrom

upper layer from which the buried via starts

BuriedTo

lower layer to which the buried via ends

Name

string, name of via (vias have names?)

SFlags

symbolic or numerical flags

NFlags

numerical flags only

Example:

Via[15.0000mm 11.0000mm 24.00mil 12.00mil 0.0000 11.81mil 0 5 "" ""]

The above example gives a via at coordinates x=15.0000 mm, y=11.0000mm, with a 24.00mil thickness, a 6.00mil clearance, a 0.0000 gap, a -12.00mil mask (tented), a 11.81mil drill width, starting at the top layer ("0"), ending at the 3rd copper layer ("2"), and has no names and no flags.

9.9 Object Flags

Note that object flags can be given numerically (like 0x0147) or symbolically (like "found,showname,square". Some numeric values are reused for different object types. The table below lists the numeric value followed by the symbolic name.

0x0001 pin

If set, this object is a pin. This flag is for internal use only.

0x0002 via

Likewise, for vias.

0x0004 found

If set, this object has been found by FindConnection().

0x0008 hole

For pins and vias, this flag means that the pin or via is a hole without a copper annulus.

0x0008 nopaste

For pads, set to prevent a solderpaste stencil opening for the pad. Primarily used for pads used as fiducials.

0x0010 rat

If set for a line, indicates that this line is a rat line instead of a copper trace.

0x0010 pininpoly

For pins and pads, this flag is used internally to indicate that the pin or pad overlaps a polygon on some layer.

0x0010 clearpoly

For polygons, this flag means that pins and vias will normally clear these polygons (thus, thermals are required for electrical connection). When clear, polygons will solidly connect to pins and vias.

0x0010 hidename

For elements, when set the name of the element is hidden.

0x0020 showname

For elements, when set the names of pins are shown.

0x0020 clearline

For lines and arcs, the line/arc will clear polygons instead of connecting to them.

0x0020 fullpoly

For polygons, the full polygon is drawn (i.e. all parts instead of only the biggest one).

0x0040 selected

Set when the object is selected.

0x0080 onsolder

For elements and pads, indicates that they are on the solder side.

0x0080 auto

For lines and vias, indicates that these were created by the autorouter.

0x0100 square

For pins and pads, indicates a square (vs round) pin/pad.

0x0200 rubberend

For lines, used internally for rubber band moves.

0x0200 warn

For pins, vias, and pads, set to indicate a warning.

0x0400 usetherm

Obsolete, indicates that pins/vias should be drawn with thermal fingers.

0x0400

Obsolete, old files used this to indicate lines drawn on silk.

0x0800 octagon

Draw pins and vias as octagons.

0x1000 drc

Set for objects that fail DRC.

0x2000 lock

Set for locked objects.

0x4000 edge2

For pads, indicates that the second point is closer to the edge. For pins, indicates that the pin is closer to a horizontal edge and thus pinout text should be vertical.

0x8000 marker

Marker used internally to avoid revisiting an object.

0x10000 connected

If set, this object has been as physically connected by FindConnection().

9.10 PCBFlags

0x00001

Pinout displays pin numbers instead of pin names.

0x00002

Use local reference for moves, by setting the mark at the beginning of each move.

0x00004

When set, only polygons and their clearances are drawn, to see if polygons have isolated regions.

0x00008

Display DRC region on crosshair.

0x00010

Do all move, mirror, rotate with rubberband connections.

0x00020

Display descriptions of elements, instead of refdes.

0x00040

Display names of elements, instead of refdes.

0x00080

Auto-DRC flag. When set, PCB doesn’t let you place copper that violates DRC.

0x00100

Enable ’all-direction’ lines.

0x00200

Switch starting angle after each click.

0x00400

Force unique names on board.

0x00800

New lines/arc clear polygons.

0x01000

Crosshair snaps to pins and pads.

0x02000

Show the solder mask layer.

0x04000

Draw with thin lines.

0x08000

Move items orthogonally.

0x10000

Draw autoroute paths real-time.

0x20000

New polygons are full ones.

0x40000

Names are locked, the mouse cannot select them.

0x80000

Everything but names are locked, the mouse cannot select anything else.

0x100000

New polygons are full polygons.

0x200000

When set, element names are not drawn.

10 Library Creation

This chapter provides a detailed look at how footprint libraries are created and used. The chapter is split into two section, the first section covers the "old" style libraries which use the m4 macro processor and the second section covers the "new" style libraries.

Despite the names "old" and "new", both styles of libraries are useful and the "old" style should not be discounted because of its name. The advantage of the old style libraries is that one can define a family of footprints, say a DIP package, and then quickly produce all the members of that family. Because the individual packages make use of a base definition, corrections made to the base definition propagate to all the members of a family. The primary drawback to using this library approach is that the effort to create a single footprint is more than a graphical interface and may take even longer if the user has not used the m4 macro language previously.

The new style of footprint libraries stores each footprint in its own file. The footprints are created graphically by placing pads and then converting a group of pads to a component. This library method has the advantage of being quick to learn and it is easily to build single footprints quickly. If you are building a family of parts, however, the additional effort in creating each one individually makes this approach undesirable. In addition, creating a part with a large pin count can be quite tedious when done by hand.

10.1 Old Style (m4) Libraries

The old style libraries for pcb use the m4 macro processor to allow the definition of a family of parts. There are several files associated with the old style library. The file common.m4 is the top level file associated with the library. common.m4 defines a few utility macros which are used by other portions of the library, and then includes a predefined set of library files (the lines like include(geda.inc)).

10.1.1 Overview of Oldlib Operation

The big picture view of the old style library system is that the library is simply a collection of macro definitions. The macros are written in the m4 macro language. An example of a macro and what it expands to is the following. One of the predefined footprints in the library which comes with PCB is the PKG_SO8 macro. Note that all the footprint macros begin with PKG_. For this particular example, PKG_SO8 is a macro for an 8-pin small outline surface mount package. All of the footprint macros take 3 arguments. The first is the canonical name of the footprint on the board. In this case "SO8" is an appropriate name. The second argument is the reference designator on the board such as "U1" or "U23". The third and final argument is the value. For an integrated circuit this is usually the part number such as "MAX4107" or "78L05" and for a component such as a resistor or capacitor it is the resistance or capacitance. The complete call to the macro in our example is ‘PKG_SO8(SO8, U1, MAX4107)’. When processed by m4 using the macros defined in the PCB library, this macro expands to

Element(0x00 "SO8" "U1" "MAX4107" 146 50 3 100 0x00)
(
	Pad(10 25 38 25 20 "1" 0x00)
	Pad(10 75 38 75 20 "2" 0x100)
	Pad(10 125 38 125 20 "3" 0x100)
	Pad(10 175 38 175 20 "4" 0x100)
	Pad(214 175 242 175 20 "5" 0x100)
	Pad(214 125 242 125 20 "6" 0x100)
	Pad(214 75 242 75 20 "7" 0x100)
	Pad(214 25 242 25 20 "8" 0x100)
	ElementLine(0 0 151 0 10)
	ElementArc(126 0 25 25 0 180 10)
	ElementLine(101 0 252 0 10)
	ElementLine(252 0 252 200 10)
	ElementLine(252 200 0 200 10)
	ElementLine(0 200 0 0 10)
	Mark(29 25)
)

which is the actual definition of the footprint that the PCB program works with. As a user of PCB the only time you will need or want to run m4 directly is when you are debugging a new library addition. In normal operation, the calls to m4 are made by helper scripts that come with PCB.

Tools such as gsch2pcb (used to interface the gEDA schematic capture program to PCB layout) will call m4 to produce an initial PCB layout that includes all the components on a schematic. In addition, when manually instantiating parts from within PCB, m4 will be called by PCB’s helper scripts to produce the footprints.

10.1.2 The Library Scripts

There are several scripts that are used for processing the m4 libraries. This section briefly describes these scripts and details how they are used by PCB.

10.1.2.1 Scripts Used During Compilation

The scripts described in this section are used during compilation of PCB. They are run automatically by the build system, but are described here to help document the complete library processing that occurs. During the build of PCB, the following actions are taken. The CreateLibrary.sh script is run to produce an M4 "frozen file". This frozen file is simply a partially processed M4 input file which can be loaded by M4 more quickly than the original input file.

A typical call to CreateLibrary.sh used during the compilation of PCB is:

./CreateLibrary.sh -I . pcblib ./common.m4 TTL_74xx_DIL.m4
connector.m4 crystal.m4 generic.m4 genericsmt.m4 gtag.m4
jerry.m4 linear.m4 logic.m4 lsi.m4 memory.m4 optical.m4 pci.m4
resistor_0.25W.m4 resistor_adjust.m4 resistor_array.m4
texas_inst_amplifier.m4 texas_inst_voltage_reg.m4
transistor.m4 geda.m4

The ‘-I .’ says to search in the current directory for the .m4 files. The output frozen file is pcblib. The main common.m4 file is listed as well as all of the *.m4 files which define the components in the library.

In addition, a library contents file is created during the build with the CreateLibraryContents.sh script. A typical call to CreateLibrary.sh used during the compilation of PCB is:

./CreateLibraryContents.sh -I . ./common.m4 TTL_74xx_DIL.list
connector.list crystal.list generic.list genericsmt.list gtag.list
jerry.list linear.list logic.list lsi.list memory.list optical.list
pci.list resistor_0.25W.list resistor_adjust.list resistor_array.list
texas_inst_amplifier.list texas_inst_voltage_reg.list transistor.list
geda.list > pcblib.contents

The pcblib.contents file is used by the PCB program to define the libraries and components which will be displayed when you bring up the library window from within PCB. An example of part of the pcblib.contents file is:

TYPE=~TTL 74xx DIL
7400_dil:N:7400:4 dual-NAND
7401_dil:N:7401:4 dual-NAND OC
7402_dil:N:7402:4 dual-NOR
TYPE=~geda
geda_DIP6:DIP6:DIP6:Dual in-line package, narrow (300 mil)
geda_DIP8:DIP8:DIP8:Dual in-line package, narrow (300 mil)
geda_DIP14:DIP14:DIP14:Dual in-line package, narrow (300 mil)
geda_ACY300:ACY300:ACY300:Axial non-polar component,

The TYPE= lines define the library name that will show up in the library window in PCB. The other lines define the actual components in the library.

10.1.2.2 Scripts Used by PCB at Runtime

When PCB is first executed, it makes a call to the ListLibraryContents.sh script. This script provides the PCB program with the contents of the library contents file created when PCB was compiled. A typical call to ListLibraryContents.sh is

../lib/ListLibraryContents.sh .:/tmp/pcb-20030903/src/../lib pcblib

This command says to search the path ‘.:/tmp/pcb-20030903/src/../lib’ for a file called pcblib.contents (the .contents part is added automatically) and display the contents of the file. PCB parses this output and generates the library window entries.

When you pick a library component from the library window, PCB calls the QueryLibrary.sh script to actually pull the footprint into the layout. For example, when the ACY300 component is selected from the ~geda library, the generated call may be:

/tmp/pcb-20030903/src/../lib/QueryLibrary.sh
.:/tmp/pcb-20030903/src/../lib pcblib geda_ACY300 ACY300
ACY300

If you were to run this command by hand you would see the PCB code for the element:

Element(0x00 "Axial non-polar component," "" "ACY300" 245 70 0 100 0x00)
(
	Pin(0 25 50 20 "1" 0x101)
	Pin(300 25 50 20 "2" 0x01)

	ElementLine(0 25 75 25 10)
	ElementLine(225 25 300 25 10)

	ElementLine(75 0 225 0 10)
	ElementLine(225 0 225 50 10)
	ElementLine(225 50 75 50 10)
	ElementLine(75 50 75 0 10)

#       ElementArc(X1 Y 50 50 270 180 10)
#       ElementArc(X2 Y 50 50 90 180 10)

	Mark(75 25)
)