When you set up your project by following the File → New → Project menu path, you had five options from which to choose: a project, a design, a library, a VHDL file, or a Text file. The options we are most interested in are projects and libraries, and we look at those in great detail throughout the book. VHDL files are used in field programmable gate array projects and are not discussed here. A Text file is simply a text file (for making project notes, for example).

After you selected the New Project option to begin setting up your project, four more options were available to you in the New Project dialog box: Analog or Mixed-Signal A/D, PC Board Wizard, Programmable Logic Wizard, or Schematic. A flow diagram of these options and suboptions is shown in Figure 3-1 (see also Figure 2-2). Analog or Mixed-Signal A/D is used to simulate analog and/or digital circuits using PSpice. PSpice is used to develop and test models (Chapter 7), perform circuit simulations (Chapter 7 and the PCB Design Examples), and simulate transmission lines (PCB Design Examples). For now, we work mostly with the second option, the PC Board Wizard, while we focus on designing PCBs. The next option, Programmable Logic Wizard, is for working with programmable devices and is not discussed in this text. A Schematic is basically just a design file with only a schematic and a parts cache. The thick green line in Figure 3-1 shows the path you followed in Chapter 2, that is, File → New → Project → PC Board Wizard → No Simulation.

There are four types of OrCAD libraries. As shown in Figure 3-2, these four libraries have three file extensions. There are two types of OLB libraries: an LIB library and a symbols library, which contains .dra files as well as some other files that are explained in detail in Chapter 8. Inside the capture folder is a library folder, which contains one of the types of OLB files, and a folder called pspice, which contains the other types of OLB files. The OLB files located directly in the Capture library folder contain simple schematic part symbols and are the ones we used in Chapter 2. The libraries located in the pspice folder contain parts with schematic symbols, too, but the parts also contain PSpice templates, which are links to specific PSpice models. The PSpice models to which templates point are located in the main OrCAD pspice folder (shown at the bottom of Figure 3-2). Individual models are grouped into various PSpice library files, which contain the .LIB extension. The share folder contains the footprint models (called symbols), which are files with the .dra extension. Most parts in Capture are capable of having a PSpice template or a footprint assigned to them, but only some parts have them preassigned. It may seem backward, but only parts from the PSpice part library (located in the Capture/library folder) have preassigned templates and footprints, and the footprints are OrCAD Layout footprints not PCB Editor footprints. So, in Chapter 2, when you worked with the PCB Project Wizard, you selected libraries from the Capture/library folder, which had parts with schematic symbols but had no PSpice simulation capabilities or footprints assigned to them.

Once you clicked Finish in the PCB Project Wizard box, Capture opened up the Project Manager window shown in Figure 3-3. Behind the scenes, Capture generated two files: an OrCAD project file (name.OPJ) and a design file (name.DSN). These files will be in the directory you chose when you set up the project.

As you look at the Project Manager window, you can see that a project contains three folders labeled Design Resources, Outputs, and Referenced Projects. Initially, the Outputs and Referenced Projects folders are empty. When a netlist is created, netlist files are placed in the Outputs folder. The Design Resources folder contains one design (represented by the icon) and a Library folder. A project can have only one design, but a design can have several subfolders, which in turn may contain several different items. The Library folder contains links to the libraries used by your design. We discuss library management in Chapter 7. The design contains at least one Schematic folder (the root folder) and a Design Cache folder. A design can contain multiple Schematic folders, and each Schematic folder can contain multiple schematic pages. The Design Cache folder contains a record of each part you used in your design. If you modify one of the parts on a Schematic page, Capture makes a copy of it (leaving the original part in the library unchanged) and adds a record of the modified part to the design cache. A design with one Schematic folder and one or more Schematic pages connected together by off page connectors is called a flat design. A design with more than one Schematic folder and one or more Schematic pages per folder or that contains hierarchical blocks is called a hierarchical design. Hierarchical designs are not discussed here, since they are not used with PCB design projects. For more information on project details, see Chapter 2 of the Capture User’s Guide, under “Starting a New Project” (cap_ug.pdf in the OrCAD_16.0/DOC folder).

Once the project is set up, the next step is to open the Schematic page (if it is not already open) and begin placing parts from the Place dropdown menu. When the Place Part dialog box opens (see Figure 3-4), it shows a list of libraries (in the Libraries window) and a list of the parts (in the Part List window) within a library. If you select a part within one of the libraries, you can see what the part looks like in the preview window, as pointed out in Figure 3-4(a). The libraries listed in the Libraries window are ones that were added by the PC Board Wizard when you set up the current project and libraries that were added to the list during previous projects. You can add other libraries to the list by clicking the Add Library… button. Likewise, you can remove a library from the list by selecting it and clicking on the Remove Library button. The libraries that are listed may be from the Capture or the PSpice library. It is not obvious which library it is from just by looking at the name, (compare Figures 3-4(a) and 3-4(b)). However, if you have Windows ToolTips turned on and hold your mouse over the library name, the ToolTips text box will show the path of the library, (see Figure 3-4(a)). From the path, you can tell which type of library it is. Another important note is that, if a PSpice or Layout library (not a PCB Editor library) is associated with the Capture part, you will see one or both of the icons below the part preview window, as shown in Figure 3-4(b). If no icons are present, it means that it is just a Capture schematic part that has no footprint or PSpice template (models) assigned to it.

As you place parts in your design, Capture keeps track of the parts and stores the information in a database file generated the moment you place your first part. This file has a .DBK extension. After you finish your design and tell Capture to make the PCB Editor netlist, Capture generates three more files that describe which parts were used and how they were connected. The files are pstxnet.dat (the netlist file), pstxprt.dat (the reference designator and device type file), and pstchip.dat (a device definition file also used for pin swapping, etc.); and they are located in the Outputs folder. These files are also used when back-annotating information from PCB Editor to Capture. More on back-annotation is discussed in the PCB Design Examples. For the most part, these files are used behind the scenes, and you need not know much about them for what we cover in this text. If you want to know more about them, please see Allegro® PCB Editor Users Guide: Transferring Logic Design Data (algrologic.pdf, p. 18) which is located in the OrCAD documents folder.

Another file that gets created is the netrev.lst file, which is a netlisting report generated when the PCB Editor netlist files are created. If there is a problem during the netlisting process, this is where the errors and warnings are documented. If you have trouble trying to create a netlist, open this file with Microsoft Word or another text application and search for the word error or warning. An example of a netlist error is given in the PCB Design Examples.

Before we start talking about the tool set, we examine a couple terms that should be defined up front, so the descriptions of the tools make more sense. These important terms follow:

At this point in Chapter 2, PCB Editor was launched, the board design ( name.brd) was opened with all default settings, and a blank work area was presented to you. From this point you made a board outline, placed the parts on your board, autorouted the board, and produced the artwork for it. To be fluent at these tasks, you need to know how to use the PCB Editor tools. We now take a tour of the PCB Editor environment and tool set.

Note: From the time you start your design in Capture to the time the artwork is produced in PCB Editor, nearly 30 files can be generated, which together fully describe your design. If you save more than one project in the same folder, it can become very cluttered. It is a good idea to set up a “MyProjects” folder that contains subfolders for each project.

The Design window is the working environment for a board design (see Figure 2-12). From the Design window, you have access to the tools you need to handle parts, route traces, and perform back annotations (design updates from PCB Editor to Capture). Hundreds of tasks can be executed from the Design window menus. Since they are covered in detail in the Allegro® User’s Guide, a detailed discussion of the menus is not given here, but the key menu options are discussed in the Examples as the need arises. The toolbar is discussed next.

By default, two toolbars are displayed. You can move them wherever you want or turn them off. To add tool bars, select View → Customize Toolbar… from the menu. This section does not describe the tools in great detail but serves as an introduction only. The use of the tools are demonstrated in the design examples and described further in Allegro® PCB Editor User Guide: Getting Started with Physical Design (algrostart.pdf).

The control panel is an area containing three tabs that show or hide collapsible window panes. The panes are shown in Figure 3-5 in their default condition (no tools or commands active). The panes are dynamic, so what is displayed depends on what tool is active or what type of object you selected at that moment. From these panes, you can control visibility and selectability of objects and what particular tools can do (extent of effect, etc.) when you use them. The panes are collapsible, so that they do not take up design window space, but you can pin them in place by toggling the stick pin icon. You can also close them altogether by clicking the X in the upper right corner. To display them select View → Window → Options/Find/Visibility from the menu bar. Each pane is described briefly. You see examples of them in action during the design examples.

The Command window (Figure 3-7) provides you with information, gives instructions, and allows you to enter commands at the Command prompt. Most of the commands you often use are also located on the toolbar and in the menus, but the Command window can give you greater control of the tools (if you know the commands). The documentation folder in the OrCAD directory has manuals (called command references) for these commands. The manuals are listed alphabetically by the first letter of the command followed by coms. So, for example, if you are looking for instructions on how to use the Command window to perform a manual routing task ( add connect) look in the acoms document folder (or use the Online Help tool and search for Add Connect).

The WorldView shown in Figure 3-8 is located in the lower right-hand corner of the design window and gives you a bird’s-eye overview of large boards. The white square represents your monitor, and the green outline represents the PCB’s outline. WorldView is interactive. If you use the highlight tool and select a part or net (whether by clicking on it or by selecting it from a list using the Find pane), the object will be displayed in the WorldView. If you right click inside of it, a pop-up menu is displayed that lets you change the size and location of the view in the design area.

The status bar (shown in Figure 3-9) is located along the bottom of the design window, below the Command window and WorldView window. At the far left of the bar, the Command Status section lets you know if a command is active and running. If a tool has been selected (e.g., Move), the name or function of the tool is listed at the far left; and when a command is running, the colored box turns red. When the command has finished executing, the box turns green again.

The x, y coordinates indicate the location of your cursor. The accuracy of the display is based on the design accuracy, which you can change in the Design Parameters dialog box (select Setup → Design Parameters → Design from the menu). The coordinates are absolute (based on the origin of the design) or relative (based on the last mouse pick). You can toggle between the two at any time using the A (or R) button, as described later.

The P button is interactive. Clicking it produces a Pick dialog box, which you can use to enter coordinate points in the work area using the keyboard rather than selecting a point with the mouse. This is useful for drawing outlines and so forth on large designs, so that you need not pan around the design trying to find and select a particular point. The x and y coordinates in the Pick box are entered with space between them, not a comma.

The A (or R) button determines whether the coordinates are absolute or relative. Absolute coordinates show the cursor position relative to the design origin. Relative coordinates show the cursor x and y distance relative to the last pick point you made (whether a tool was active or not).

The Application Mode text box informs you of whether PCB Editor is in Etch Edit ( EE) mode or General Edit ( GE) mode (described previously). The DRC Status box lets you know at a glance if the design rule check is up to date and if any errors exist by the color of the box. If the box is any color other than green (see Figure 3-8), then you need to update the DRC and use a DRC report to locate any errors if they exist.

The Color dialog box (Figure 3-10) is used to define custom colors for classes and subclasses and allows you to control the visibility of specific objects belonging to those classes ( Xs indicate the object is visible, open boxes indicate they are invisible). The Color dialog box can be displayed by selecting the Color button, , on the toolbar. As mentioned previously, the Color dialog box performs some of the same functions as the colored and check boxes in the Visibility and Options panes, but as the figure shows, you have much greater control of objects and layers.

Color button

The Layout Cross Section dialog box, shown in Figure 3-11, is where you define your board’s layer stack-up. From this dialog box, you can add or delete layers, define their physical and electrical properties (if you want to), and define positive and negative properties to routing and plane layers, respectively. The Layout Cross Section dialog box is displayed using the Xsection button, . Examples of setting up layer stack-ups are given in the PCB Design Examples.

Xsection button

The Constraint Manager, shown in Figure 3-12, is where you set routing and component placement rules for your board design. The Constraint Manager can be launched using the Cmgr button, , by selecting Setup → Constraints … from the menu, or by typing cmgr at the >prompt in the Command window. The Constraint Manager has four tabs and each tab has several views (indicated by folders and icons). From these tabs and views, you have very precise control over routing characteristics for every net (e.g., trace width and spacing, what vias are used, routing enabled, locking traces, etc.), every component, and shapes.

Cmgr button

Note: The Constraint Manager takes a moment to load, but if it is taking a long time to load, check the Command window. This tool will not load if a command is still active, and the Command window (and status bar) will tell you if that is the case. If so, you need to stop the current command by right clicking in the work space and selecting Done from the pop-up menu.

Once the board is laid out and routed, the artwork must be generated. The information in the board design is separated into specific data files (Gerber files), which are used by the board manufacturer to make the different parts of your board. The Artwork Control Form (Figure 3-14) is used to specify all the different types of layers for which Gerber files will be created and the format of the files. You can add as many layers as necessary to fully define your board design. Chapter 10 describes how to set up the Artwork Control Form based on a board layout example.

The drill files are generated by selecting Manufacture → NC → NC Drill… from the menu. The drill files are generated from drill settings that you specify in the NC Parameters dialog box (shown in Figure 3-15). The use of this dialog box is discussed further in Chapter 9.

The number and types of files generated by the Artwork Control Form depends on the complexity of your board and the requirements of your board manufacturer. Most of the artwork files correspond to the layers with which you work in the layout environment, but some of the files do not. For example, files are generated for etch and silkscreen layers and drill files, all of which depend on the output format you chose. The two most common types of output formats are RS-274D and RS-274X (also known as Excellon). The Excellon format is typically used, but your board manufacturer should tell you which specific files it needs and which format it prefers. Artwork instructions are set up from the Manufacture → Artwork menu, and we will look at specific settings in Chapter 9.

Some of the terminology used in the PCB fabrication business is left over from the early PCB manufacturing days. Drill tapes and apertures are such terms. Nowadays, a drill tape is just an electronic file that describes drill holes and sizes just like any of the other files describes its data. However, originally the drill tape was actually a role of paper or Mylar with holes punched into it that described hole sizes and locations for early computer numerical control (CNC) machines, but it is still sometimes called a drill tape. Here is another example. In Chapter 1, the current technology of photoplotting and laser direct imaging was discussed. In contrast, the older technology used a xenon flash lamp and a shutter to expose photosensitive film or glass plates. The shutter controlled the exposure and an aperture controlled the size of the exposed area. Any shape or drawing could be made by having apertures of different sizes and shapes. Light would be shone through the selected aperture and moved in the ± x direction, and the film was moved in the ± y direction. Opening and closing the shutter in one area (to make a pad) was called a flash, while holding the shutter open and moving the light source or film in the x and y directions (to make a trace) was called a draw. The technology today is more advanced, but the concept is the same, and the same terminology is used. Figure 3-16 shows a list of the apertures the Artwork Control Form uses, where you will notice D codes and flash geometries (circles, rectangles, and flash symbols). A Gerber D code is a just a chronological number that specifies the size and shape of the aperture used on a given layer. Flash symbols (e.g., D code D20 in the figure) are used to produce thermal reliefs, which are used to connect plated through holes to copper planes. The procedure for drawing thermal flash symbols is described in Chapter 8 and the use of them is described in the PCB Design Examples.

You should now be familiar with the PCB design flow and PCB Editor tool set. In the following chapters, we look at how to assign footprints to parts from within Capture, how to make your own Capture parts, how to make new footprints with PCB Editor, and how to set up the PCB Editor’s Constraint Manager to route complex boards.