29-08-2016, 10:56 AM
1451301764-pcbdesigner.pdf (Size: 1.01 MB / Downloads: 12)
Preamble
This document introduces the basic features of OrCAD PCB Designer. It is aimed primarily at
novices with limited experience of construction who have never designed a PCB before. For
this reason I concentrate on pin-through-hole devices (although surface-mount devices are no
more difficult) on single and double-sided boards. I strongly recommend Mitzner’s book [1]
instead if you are an experienced designer, interested in more advanced PCBs for commercial
production.
Other readers may be experienced users of OrCAD Layout who are obliged to switch to
PCB Editor; I hope that they don’t feel that their intelligence is insulted! I’ve highlighted some
of the most significant differences between Layout and PCB Editor. (I think that PCB Designer
refers to the complete suite while PCB Editor is the specific application for editing PCBs but
it’s not entirely clear.)
I adapted this document from an introductory class and have removed several features that
are unlikely to be of interest to most readers. For example, we have developed a local library of
footprints for PCBs constructed by students. The pads are enlarged to allow easy soldering and
the symbols contain features to discourage common design errors, such as tracks to inaccessible
pads underneath connectors. However, I’ve retained the instructions to produce photomasks
directly with the Plot command, rather than with Gerber files. This is helpful if you make
PCBs in-house by traditional processes, which is often the case for student projects.
Differences between versions 16.0, 16.2 and 16.3
Version 16.3 of OrCAD was released in late 2009, following 16.2 in late 2008. The What’s New
document exceeds 90 pages but most of the changes aren’t relevant to an introductory tutorial.
Here are the most important new features in version 16.2.
• The appearance of Capture has been updated to match PCB Editor. Buttons are now
larger and their purpose is sometimes clearer. A bar of tabs can be used to switch between
windows.
• Cross-probing between Capture and PCB Editor has been improved.
• The Plot command can leave drill holes open, which may be helpful for PCBs drilled by
hand.
• The software is installed in the same way, regardless of whether you have a licence or not.
Applications simply run in demonstration mode if they cannot find a licence. The demo
version is a great improvement on previous editions but the installer has a peculiarity:
you are forced to specify a licence server even if you wish to use only the demo mode. A
bogus server such as 5280@localhost should get around this problem.
This tutorial is affected less by changes from 16.2 to 16.3.
• A board can now be ‘flipped’ (viewed from underneath rather than from the top) and
rotated in 3D but this is of limited value for the simple designs described here.
• Jumpers have been added to assist the design of single-sided boards.
2
• The autorouter is now called Allegro (or OrCAD) PCB Router rather than SPECCTRA.
Board files written by version 16.3 of PCB Editor cannot be read by version 16.2, nor can those
written by 16.2 be read by version 16.0. (This contradicts the statement in Getting Started with
Physical Design that ‘Allegro PCB Editor databases are backward-compatible with their major
version number (the number to the left of the dot)’.) Use the menu item File > Export > Save
design to 16.2. . . (or 16.01. . .) to write a file compatible with an earlier version. (The jargon
is to downrev the design.) I have not yet updated this document for version 16.5.
Prospectus
This document falls into two major parts.
• The main body is a tutorial that guides you through the layout of two simple PCBs. First
is a one-transistor amplifier, which is really straightforward but allows you to concentrate
on the interface of the applications. The second design is an instrumentation amplifier,
which is laid out on single and double-sided PCBs using the autorouter. I also show how
to produce manufacturing data for this design.
• The appendices contain a collection of techniques that you might find useful. Links to
these are given in the tutorials.
PCB Editor has so many features, even in its OrCAD version, that I cover only a small fraction
of them.
1 Introduction
The Cadence OrCAD PCB Designer suite comprises three main applications.
• Capture is used to draw the circuit on the screen (schematic capture). A netlist, which
describes the components and their interconnections, is the link to PSpice and PCB Editor.
• PSpice simulates a captured circuit. I do not describe PSpice in this tutorial.
• PCB Editor (Allegro) is the application for laying out a printed circuit board. It includes
an automatic router that works out the arrangement of tracks needed to connect the components
on the PCB. The output from PCB Editor is a plot or a set of files that can be
sent to a manufacturer.
The overall design flow for making a PCB is shown in figure 1 on the following page with a
summary in section 7 on page 46.
PCB Editor replaces the earlier application, Layout, which is now discontinued. OrCAD
PCB Designer is the most basic version of Cadence’s Allegro suite for PCB design and much
of the documentation refers to ‘Allegro’ rather than ‘PCB Editor’.
Fixup. The libraries for Capture and PCB Editor have some incompatibilities that must be
corrected by Fixups. I hope to find smoother ways around these difficulties in the future
Libraries, files, directories and design rules
Three types of information are needed for each component, corresponding to the three main
applications listed above.
• Electrical symbols are used to draw the circuit in Capture.
• Electrical models allow you to simulate the circuit in PSpice.
• Footprints or package symbols show the physical size and shapes of the pads (where
the pins are soldered to the board) and the outline of the package. They are used to lay
out the circuit in PCB Editor.
These are stored in different sets of libraries and you must select the files needed for a particular
design. Footprints are needed as well as electrical symbols because components with the same
electrical behaviour come in different packages. For example, an integrated circuit might come
in two versions:
• a traditional, plastic dual-in-line package (PDIP) with pins 0.1
00 apart
4
• a smaller, surface-mount device (SMD) with pins only 0.5 mm apart, if it has pins at all
The opposite is also true: resistors of a particular shape come in a wide range of values.
Further information is needed to describe the characteristics of the printed circuit board on
which the components are mounted. The details are important for high-speed designs but we
need to know only the number of layers of copper, called etch in PCB Designer. This tutorial
covers only single-sided boards, which have components on top and copper on the bottom,
and double-sided boards, which have copper on both surfaces but usually components only on
the top. Fancier boards often have two internal planes of copper used for power and ground;
complex designs need further layers.
Design rules are required to lay out the circuit on the PCB. The full details are complex but
the basic rules specify the minimum width of tracks and the gap between them. Manufacturers
often express these numbers in the format 10/8, meaning minimum widths of 10 for tracks and
8 for gaps (although the numbers are usually the same). The units are almost always mils, which
mean thousands of an inch; see section 2.5 on page 10. I use 25/25 rules in this tutorial, which
are extremely coarse but produce boards that are easy for inexperienced students to solder.
Further design rules control a diverse range of features, such as the spacing between tracks
and pads, whether vias are permitted and the impedance of tracks (they act like transmission
lines at high frequency). These rules are adjusted with the Constraint Manager, which we’ll
encounter in section 4.4 on page 29.
Fixup. Older versions of OrCAD prefer designs to be stored in OrCAD_Data rather than My
Documents and may reject filenames that contain spaces. If you get inexplicable errors about
unexpected arguments or incomplete file names, try copying the design to OrCAD_Data and
removing spaces from the names of all directories and files. ❦
1.2 Help!
All programs provide extensive online help. Appendix A on page 47 explains how to use the
Cadence Help system and guides you around the major documents supplied with PCB Designer.
Many commands in PCB Editor have names that are not obviously related to the corresponding
item on the menus so I have pointed these out.
2 One-transistor amplifier: Schematic capture
The first design is a one-transistor amplifier. It has only a few components and will be laid out
on a huge board to make the routing straightforward: The challenge is to learn the software.
The initial step is to draw the circuit in Capture.
Capture treats each circuit design as a project and a project manager shows the logical
relation between the files required. It is essential to create a new directory for each project.
Strange errors can occur if you have more than one project in a directory, from which it seems
impossible to recover. It also keeps your work organised. OrCAD creates a subdirectory for
PSpice files and an allegro subdirectory for PCB files. You should know this by now but
a reminder is never a bad idea: Save your work frequently and take regular backups of
important circuits.