Cadence OrCAD PCB Designer 16.6

Cadence OrCAD PCB Designer 16.6
Electronic Design Project 2
Cadence OrCAD PCB Designer 16.6
Professor John H. Davies
2014 August 12
After completing these laboratories, you will be able to:
• analyse a simple, one-transistor amplifier by hand
• use simulation to optimise the design of the amplifier
• lay out a one-sided printed circuit board (PCB) for the amplifier with manual routing
• lay out an instrumentation amplifier based on three opamps, comparing one-sided
and double-sided boards with automatic routing, and produce photomasks for production
• lay out a mixed-signal system, comparable with the final project in this course, following standard procedures for schematic capture.
Please ensure that you have the following two items for every laboratory or you will be sent
away to buy them.
• A bound, A4 laboratory notebook for making notes, recording results and storing printouts.
• University printer credits so that you can print the circuits, layouts and the results of your
simulations. Printouts should be attached firmly into your laboratory book for future
The first part of these laboratories, which is a ‘pencil and paper’ analysis of a one-transistor
amplifier, must be written up in your laboratory book as you do it. The remaining parts do not
need much of a record to be kept but you will find it useful to make a note of tricks and tips for
using OrCAD. This will be valuable when you have to design your own circuits later this year
and in subsequent projects.
These laboratories form part of your professional development because it is expected that
every electronic engineer should be able to design, populate and test a printed circuit board
(PCB). You must therefore complete the first two designs to gain credit for this course. Most
of the marks are awarded simply for completion but an extra mark is granted for a good layout
of the final design. Late work will be considered for credit but marks will not be awarded. This
penalty is relaxed for direct entrants, who are allowed until the Easter vacation to complete the
One-transistor amplifier: simple analysis
Schematic capture and simulation
Preparation for PCB layout
OrCAD PCB Editor
Instrumentation amplifier – single-sided board
Instrumentation amplifier – double-sided board
A mixed-signal system
A How to correct a layout if you spot an error in the circuit
B Summary: PCB design flow
These exercises introduce you to schematic capture, simulation and PCB layout using Cadence
OrCAD PCB Designer with PSpice. This suite comprises three main applications.
• Capture is used to draw the circuit on the screen (schematic capture). It is easy to
incorporate changes to the design and to correct errors. (On the other hand, it is much
faster to develop the outline of a circuit using pencil and paper, as we shall do for the first
• PSpice simulates a captured circuit so that you can investigate its performance. Plots
were produced by a separate application called Probe in the past and I’ll stick to this
name, although this functionality has long been integrated into PSpice.
• 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 your
components on the PCB. The output is a set of files that can be sent to a manufacturer or
printouts for the electronics workshop in the Rankine Building.
The first two applications should be familiar from last year but the third is new. These programs
can be used on networked Windows PCs throughout Engineering. The licensing arrangements
do not permit access outwith the School but you may apply for a full licence to use OrCAD on
your own PC. See moodle for a link.
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’. Allegro is widely
used in industry and is similar to the Cadence software for laying out integrated circuits (ICs),
which you will experience in Digital Circuit Design 3.
Fixup. The libraries for Capture and PCB Editor have some incompatibilities that must be
corrected by Fixups. ¦
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. You might wonder why footprints are needed as well as electrical symbols. The reason
is that 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 0.100 apart
• 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 only the number of layers of copper, called etch in PCB Designer. This tutorial covers
• single-sided boards, which have components on top and copper on the bottom,
• double-sided boards, which have copper on both surfaces.
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 4.4 on page 14. We use 25/25 rules, which
are extremely coarse by modern standards but produce boards that are easy for inexperienced
students to solder.
Figure 1. Cadence Help system with the Navigation pane opened.
Extensive documentation is provided with OrCAD. Please try this before asking a demonstrator
because it is part of the learning process. Most professional software is so complicated that even
experts make regular use of the help files. An unhelpful feature of the Cadence help system
is that it opens only with the page associated with the most recent action rather than offering
the full range of documents. Go to the menu bar of the Cadence Help page and choose View >
Show Navigation, which produces a screen like that in figure 1. Use the navigation panel on
the left to choose the appropriate product and type the desired topic into the Topics box.
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.
One-transistor amplifier: simple analysis
Figure 2 shows the circuit of a simple amplifier with one transistor. It is intended to amplify
audio signals, say from 20 Hz – 20 kHz. The first step in any design is to sketch the circuit using
pencil and paper and estimate whether it is likely to work correctly. You will not learn how to
design this particular circuit until Analogue Electronics 2 later in the year so we shall ‘reverse
engineer’ it instead. The calculations are simple and should be done in your laboratory book.
You should be pleasantly surprised to find that you don’t need to know much about transistors
to analyse this. In fact you did most of it in Electronic Engineering 1Y. Make sure that you
recognise the emitter, base and collector of the transistor.
Figure 2. A simple, one-transistor amplifier that can be simulated using Spice.
We first find the bias point, also called the operating point or quiescent point. This means
the conditions when no signal is applied and the circuit is ‘resting’. The 1 Vac source can
therefore be ignored.
1. Resistors R1 and R2 form a simple potential divider from the power supply V2 if we ignore
the transistor Q1 attached to the mid-point. (We should go back and check this assumption when the currents are known.) Calculate the voltage on the base of the transistor.
Remember that ‘the voltage on the base’ really means ‘the potential difference between
the base and ground’.
2. The base–emitter junction of a transistor is a forward-biassed diode (hence the arrow on
its symbol) and therefore has a voltage of Vbe ≈ 0.7 V across it. Use this to calculate the
voltage on the emitter.
3. We now know the voltage across the resistor R4 . Calculate the current through it.
4. The current into the base of a transistor is much smaller than the currents at the other
two terminals, so the current flowing into the collector is nearly equal to that flowing
out of the emitter. Calculate the voltage dropped across R3 and hence the voltage on the
This has shown why the four resistors are needed but not the capacitors. What is the expression
for the impedance of a capacitor (remember that it is complex) and how does its magnitude
depend on frequency? The capacitors in this circuit allow AC to pass – the signals that we wish
to amplify – but block the DC voltages that set the bias point.
• We have seen that the base of the transistor is kept at a particular voltage by the potential
divider, which sets the bias point. The capacitor C1 on the input isolates this voltage from
the previous stage of the system but lets the signal through.
• Look at the circuit through which the input AC signal flows. It passes through the capacitor C1 , the base–emitter junction of the transistor, then R4 and C2 in parallel, and back to
the ground connection of the input. Only the part of the voltage across the base–emitter
junction gets amplified; the rest is wasted and should therefore be made as small as possible. This means that we would like to get rid of R4 but this cannot be done because it is
needed to set the bias point – it determines the current through the transistor, as you saw
The bypass capacitor C2 across the resistor R4 reduces the wasted signal voltage. The bias is
DC so it all flows through the resistor. The signal is AC so it can also flow through the capacitor.
The aim is to make almost all of the signal flow through C2 , which must therefore have a much
smaller impedance than the resistor. Ideally the impedance of C2 should obey |ZC ( f )| R4 for
all frequencies in the signal.
5. Is this true for the values in figure 2?
Finally, estimate the voltage gain of the circuit. This needs some background on transistors that
you have not yet covered so I’ll just quote the result. The gain is given by
= −gm R3
where gm is called the transconductance of the transistor, defined by ∂ Ic /∂Vbe . Its value is
given by
gm =
where Ic is the collector current at the bias point, which you have calculated already, and VT
is called the thermal voltage. This is in turn given by VT = kB T /e where kB is Boltzmann’s
constant (remember this from physics courses?), T is the absolute temperature and e is the
magnitude of the electronic charge. Don’t worry about the formula because VT ≈ 25 mV at
room temperature, which is easy to remember (or 1/VT ≈ 40 V−1 ). Now you can calculate the
transconductance and voltage gain.
6. Express the gain both as a ratio and in decibels (dB).
* Milestone: Show your results to a member of staff and be prepared to explain them.
An interesting feature is that we haven’t used any details of the transistor at all! This makes
it easy to design circuits based on bipolar junction transistors, to give them their full name.
Now we’ll capture the circuit in OrCAD, simulate it and check these estimates.
Schematic capture and simulation
Always create a fresh folder (directory) for every new project in OrCAD otherwise you will
encounter strange errors, from which it seems impossible to recover. It also keeps your work
Start OrCAD Capture (use Search programs and files on the Start menu if you cannot
find it). There is a short delay while the software is loaded and the licence server is accessed.
Alternatively, you are asked if you wish to use Demo mode if no licence can be found. You
may be offered a Cadence Product Choices box, in which case you should choose OrCAD
PCB Designer with PSpice. The screen eventually shows the OrCAD Capture main window
with a menu bar and tool bar. A sub-window at the bottom shows the session log.
Create a project
The first step in any design is always to create a project in OrCAD.
1. Create a new folder in Windows to hold all files for the project. I suggest that you first
go to My Documents, create a new folder for this course, then create a folder within this
folder for each design.
2. Select File > New > Project from the menu bar of Capture. I use ‘>’ throughout this
document to show the levels of a hierarchical menu.
3. In the New Project dialog box:
• Select an Analog or Mixed A/D project. This choice is essential or you will not be
able to simulate the circuit.
• Click on the Browse key, select your H drive and navigate to the new directory that
you created for this design. Click OK.
• Give the project a meaningful name. Use only letters, numbers, spaces, – and _.
Do not use brackets or other characters because this will eventually cause OrCAD to
crash and it is complicated to recover from this error (easier to restart from scratch).
• The path and directory now show in the location box (if you can see them – they
are usually too long). Click OK in the New Project dialog box.
• Click Next.
4. Select the Create a blank project button in the small dialog box that appears and click
5. Your project will now be created. The Project Manager window at the top left shows the
files associated with your design and the resources used, such as library files. Its title is
the full pathname of your project, which is usually far too long to fit. Check that the File
tab is selected if the view looks unfamiliar.
6. Expand the Design Resources folder in the project, then the design (with extension
.dsn), then the SCHEMATIC1 folder and finally double-click PAGE1 to open the schematic
page for your design. Locate the Title box in the lower right-hand corner, double-click
on the placeholders, which are in angle brackets <>, and replace them with a descriptive
title and so on.
Draw the circuit
Lay out the circuit in figure 2 on page 5. The method is exactly the same as last year but here
are a few tips in case you have forgotten.
Jargon: The label that identifies each component on the schematic drawing is called its reference or refdes, short for reference designator. For example, the transistor has refdes Q1. Each
refdes must be unique, meaing that no other component can be called Q1. Capture assigns a
unique refdes automatically: do not change it! ¦
• Libraries must be chosen from the pspice folder, otherwise the components will not have
PSpice models and you will not be able to simulate them.
• Basic components like resistors are in the analog library, sources such as VDC are in
source and the param block is in special. Use Search if you can’t guess where a component is located. You will probably need to do this for the transistor. See the note
• The capacitor C2 is an electrolytic type, which must be installed with the correct polarity
or it will explode. Its parameter CMAX is the maximum working voltage, which is not
needed for simulation but is important when you pick out a real component. Set it to
16 V, which is a common value.
• Always join components with wires, not by placing them so close that their pins overlap.
• All circuits must have a ground node called 0 (zero) for simulation. Use Place > Ground. . .
from the menu bar or the ground button on the right.
• PSpice is unhelpful about notation. Usage like 10^6 doesn’t work but it won’t tell you!
(It will just stop at the caret and take the value as 10.) Use 1e6 or 1Meg instead – not 1M
because a single m or M means milli, not mega.
• Wires and components sometimes become joined incorrectly if you move them about.
Use Place > Junction or the junction tool from the buttons on the right to eliminate
spurious connections.
• I like to use off-page connectors to label nodes such as input and output, where the
voltages will be plotted. Place them from the menu or button. The names appear in
Probe and make it much easier to identify the traces.
• Your circuit need not match mine exactly. It does not matter if the components have different references, for example if R1 and R2 are interchanged. The values and connections
must be the same but the references need not match, so do not edit them.
Figure 3 on the next page shows a reminder of how to search for a part using the Place Part
panel. You must click on the button next to Search for Part to expand the panel and check
that Capture searches the appropriate directories by clicking the button next to the Path box.
We want to simulate the circuit and must therefore choose parts from the pspice directory (and
sub-directories). You can then type the name of the component that you wish to find into the
Search For box and Capture will attempt to locate it.
Figure 3. (a) Place Part panel with the Search for Part area expanded and (b) Path set up to
search the pspice directory.
Simulate the circuit
Set up a Simulation Profile to make an AC Sweep of the circuit from 10 Hz to 100 kHz. The
sweep should be logarithmic in decades with 10 points per decade. Run the simulation. Go
back to Capture and click the V button to Enable Bias Voltage Display. Do the values agree
with the pencil-and-paper calculations? Check the currents through the transistor too.
Next, plot the voltage gain in decibels (dB). You may remember how to do this from the RC
filter last year but here is a short cut in Capture.
1. Choose PSpice > Markers > Advanced > dB Magnitude of Voltage from the menu bar
and click on the output from the amplifier. This places a marker labelled VDB.
2. You should now find a decibel plot in PSpice. This requires an input voltage of 1 Vac.
Does the gain match the estimated value and is it reasonably constant with frequency?
I found that the gain did not behave as expected (so now I have given you the answer to
the first question!) and suspect that the capacitor C2 across the emitter resistor R4 is too small.
Check this by simulating the circuit for a set of values of C2 . This requires a parameter. You
should remember how to do this but the procedure is clumsy so here is a reminder.
1. Place a param block on your schematic from the special library.
2. Open the Property Editor for the param block with one of these three methods (I’ll only
mention one in future): choose Edit > Properties. . . from the menu bar, select the Edit
Properties. . . contextual menu item or double-click the block.
3. Choose New property. . . to create the parameter. Give it a name, such as Cap2, and a
default value (use its previous, fixed value). Click OK to dismiss the dialog box.
4. The parameter does not appear on the schematic by default so you must select the newly
added row/column in the spreadsheet, click the Display button, select Name and Value
and click OK. Close the Property Editor. You should now see your parameter in the block.
5. Change the value of C2 from a fixed value to the parameter witht its name in curly brackets, like {Cap2}.
6. Create a new simulation profile.
(a) Leave the general settings unchanged, which gives the same frequency sweep as
(b) Select the check box for Parametric Sweep.
(c) Choose Global parameter and enter Cap2 as Parameter name.
(d) Set the Sweep type to logarithmic sweep with one value per decade from 0.1 µF to
1000 µF.
Run the simulation and make a plot in decibels as described above. The plot should show
a set of 5 lines this time.
Print the plot and label the curves with the corresponding values of Cap2 by hand (the software
cannot do this). Add the calculated value of gain as well. The printout looks better if you make
the lines thicker. (If you print in black and white, set the number of trace colours to zero so that
the curves show up.) How is the gain related to the calculated value? Does a larger value of C2
improve the performance? What value would you recommend?
* Milestone: Explain your results and recommended value of C2 to a member of staff.
Preparation for PCB layout
Once the design of the circuit has been finalised, it can be laid out on a printed circuit board
(PCB). This takes a few steps before you leave Capture. The overall design flow for making a
PCB is shown in figure 4 on the following page with a summary in section B on page 50.
Edit the circuit
First, the ‘virtual components’ in the schematic must be replaced by real components. Here
this means the voltage sources and param block. Sometimes a battery is mounted on a PCB
to supply power but you cannot build a real circuit with a param block! (Well, you could use
a pair of sockets and unplug the component to change it.) The real circuit requires connectors
PCB Router
PCB Editor
Set up bare board
(outline, design rules)
Change Order
Place and arrange
Export to
PCB Router
Route board
Route board
Gloss board
Spread and
mitre tracks
Route board
Return to
PCB Editor
Check placement
of vias
Annotate and print
Figure 4. Design flow for making a PCB with Capture and PCB Editor. The three paths for
PCB Editor depend on whether the tracks are drawn manually (as in the first design), automatically within PCB Editor, or by running the automatic router as a separate application.
2 16V
Figure 5. The simple, one-transistor amplifier with only real components, ready for layout. The
pin numbers on the electrolytic capacitor are not normally visible but are shown to illustrate a
Figure 6. Edit Part window and Pin Properties dialogue box for correcting the numbering of
the pins of the electrolytic capacitor.
for input, output and power as shown in figure 5. The types of connector are HEADER 2 and
the like. They are in the connector library, which is in the directory one level above the pspice
directory (Cadence/SPB_16.6/tools/capture/library/). The connectors are oriented so that pin
1 is connected to ground in both cases. It is shown by a square marker on the PCB. Change
the ‘values’ of the connectors to make them more descriptive than the defaults. For example, I
changed HEADER 2 to Input for J1. Do not change the refdes, only the value. Add text to label
the pins of each connector and put your name on the circuit or you won’t be able to identify it
when it comes out of the printer.
Fixup. The electrolytic capacitor C_elect in the analog library is incompatible with its footprint. The pins of the footprint are numbered 1, 2 but those of the capacitor are p, n. This means
that the software cannot match the capacitor to its footprint. Edit the electrolytic capacitor and
change the numbers of its pins to resolve this.
1. Select the electrolytic capacitor and choose Edit > Part from the menu bar. A window
opens with an enlarged view of the capacitor.
2. The positive pin is shown as a circle on the left. Select it and and choose Edit > Properties. . . . This brings up the Pin Properties dialogue box, shown in figure 6.
3. Change the Number to 1 and click OK. Don’t worry about the name of the pin.
4. The negative pin is shown as a red line on the right. Change its Number to 2.
5. Choose File > Close. You have the choice of updating this part alone, or all ‘part instances’ – that means all C_elect components in your design. There is only one so it
doesn’t matter whether you choose Update Current or Update All in this case.
I made the pin numbers visible for the electrolytic capacitor in figure 5 on the previous page as
a reminder of this fixup. You need not do this. ¦
Print the schematic drawing and stick it into your laboratory book. The circuit takes up only
a small part of the page so it is a good idea to choose File > Print Area > Set and mark out a
rectangle that includes only the part of the page that you wish to print.
Table 1. Components, names in Capture and footprints for the one-transistor amplifier. The
names are not case-sensitive.
Capture name
Footprint name
C, polarised
GU-TO5 (letter ‘oh’ not number zero)
* Milestone: Have your drawing checked before you go any further. It is much easier to
correct mistakes at this stage.
Add footprints
The main task in preparing the design for layout is to associate a footprint with each component.
The footprint shows the physical outline of the components including the copper pads to which
the pins are soldered. Most pads are either circular or oval except for pin 1, which has square
corners to identify it. The components in the pspice library have footprints already but they are
unsuitable for us. We must therefore enter the correct footprints, which are listed in table 1 for
this circuit. Please type carefully and don’t muddle the letter ‘O’ with the numeral ‘0’.
1. Drag the cursor over your schematic drawing so that all the components are enclosed in
a rectangle. Do not include the title box.
2. Choose Edit > Properties. . . from the menu bar, which brings up the Properties spreadsheet.
3. Type each name into the PCB Footprint field of the Properties spreadsheet. All the
resistors have same footprint so use copy and paste for speed.
A problem with footprints. . .
PCB Editor comes with a library of footprints but they are intended for commercial production
and are unsuitable for boards made in the university. We have therefore designed a local library
of footprints that are more suitable for boards mades by students. Their names begin with GUto distinguish them. A catalogue is included at the end of this handout, which you should be
able to match with components kept in stores.
Design rules check
The next step is a Design Rules Check to ensure that no errors have been introduced.
1. Click on the Project Manager window and highlight your design (with extension .dsn).
2. Select Tools > Design Rules Check. . . from the menu bar.
3. Under Design Rules select both Run Electrical Rules (probably selected already) and
Run Physical Rules (probably not).
4. Click OK. A dialog box may report One or more errors or warnings were encountered.
Do you wish to view the messages in the session log? Agree to this and review the
report in the Session log window. No positive message is given to confirm that all rules
have been passed successfully, just an absence of complaints. Ask for help if you do not
understand a message – don’t just ignore it.
5. Return to your drawing and correct any errors, shown by green circles (a strange choice
of colour). Repeat until the Design Rules Check runs silently.
6. You may wish to run the Design Rules Check and select Action > Delete existing DRC
markers to get rid of the green circles. They do not vanish by themselves.
Make an empty board in PCB Editor
The simplest way of creating a PCB is first to set up an empty PCB, then to add your components and connections to the board. This follows the design flow shown in figure 4 on page 11.
First create a directory allegro within your directory for the current project. PCB Editor
likes to keep its files in a directory with this name. Then choose PCB Editor from the Start
menu, which opens the OrCAD PCB Designer application (Cadence seem muddled about the
name). I’ll leave the details of the interface until later because we need only two dialogue boxes
for this step.
Set up the search paths for footprints
I mentioned above that we use a local library of footprints rather than those supplied with PCB
Editor and must therefore tell the applications where to find our library. You should only have
to do this once.
1. Choose Setup > User Preferences. . . from the menu bar, which brings up the User
Preferences Editor.
2. Expand Paths in the list of Categories and choose the Library folder.
3. First change psmpath, where PCB Editor looks for package symbols (footprints). Click
on the Value button, which shows only ‘. . . ’, to bring up a box entitled psmpath Items.
4. Click the New (Insert) button (the leftmost one), which adds an empty item to the list
with another ‘. . . ’ button. Click this button, which brings up the usual Windows Select
Directory box.
5. Navigate to the Q drive, find the allegro directory, then pcb_lib and finally symbols.
Click OK to select this directory.
Figure 7. Completed dialogue box for setting up psmpath. Your directory path is different.
6. Next we must tell PCB Editor to look in our local directory before the default libraries,
denoted by $psmpath. Click on $psmpath followed by the Move Down arrow. The psmpath Items box should now look like figure 7 except that your directories are different
(my computer is not on the same network). Click OK.
7. Follow the same procedure to add the padstacks directory within pcb_lib to padpath.
Padstacks are the copper islands used for mounting components, including holes for pinthrough-hole components.
8. Click OK to dismiss the User Preferences Editor.
Define the board
Choose File > New. . . from the menu. In the first dialogue box, set the Drawing Type to Board
(wizard). Click Browse. . . , navigate to your new allegro directory and give the board a name
such as empty.brd. Click Open then OK to bring up the new board wizard. This takes you
through several screens to define the parameters of the PCB. Some of these are obvious, such
as the size of the board, while others set up the design rules – the width of tracks on the PCB,
how much space must be left between them, and so on.
1. The first screen is purely descriptive. Read it, then click Next >.
2. This asks for a board template. We don’t have one so select No (probably the default)
and click Next >.
3. You are next asked for a ‘tech’ file. This is short for a technology file, which specifies the
design rules – number of layers, widths and separation of tracks and so on. We won’t use
one for this design so select No and click Next >.
4. This asks for a board symbol. We don’t have one so select No again and click Next >.
5. We now reach the screens for the parameters that must be set up. The units should
be Mils. These are not millimeters but the American term for thousandths of an inch;
1 mm ≈ 40 mils. All dimensions are given in these units so get used to them.
Leave the drawing size at A. This is an American size but you aren’t allowed European
A4 if the units are mils. Leave the origin at the centre.
6. Set the grid spacing to be 100 mils.
The Etch layer count is the number of copper layers on the board – the number of layers
of tracks for signals and power. Leave this at 2, although we shall use only one layer in
the first design.
Don’t worry about the artwork films – we don’t use them.
7. Leave the names of the layers as Top and Bottom and their types as Routing Layer.
8. Enter 25 for the Minimum Line width (in mils). This value will propagate into the other
boxes. It means 0.02500 or about 0.64 mm, which is very wide for a track nowadays but
makes the board easy to produce and solder by hand.
For the Default via padstack, click on the button with . . . and choose GU-VIA80. This
design is far too simple to need vias, which carry a signal from one layer of the PCB to
another, but they may be required in future projects.
9. Rectangular board (it’s curious that a circular board is the default).
10. Enter a width of 3000 and height of 2000 mils. This defines the board outline as 300 × 200 .
There is no corner cutoff.
Specify the Route keepin distance as 100. A keepin means that objects must be kept
inside the specified region. In this case it means that tracks cannot go any closer than
100 mils to the edge of the board. It gives a border around the PCB to aid handling and
manufacture. (We’ll encounter keepouts as well later.)
Set the Package keepin distance to 250. Components must be placed within this keepin
and therefore cannot be closer than 250 mils to the edge of the board. The gap between
the two keepins allows you to run tracks around the outside of all the components, which
is often helpful on a more complicated board.
11. Click Finish – that’s it.
This has set up the design rules and made an empty board, which you can see in the main
window of PCB Editor, shown in figure 9 on page 19. Three rectangles are visible for the board
outline, route keepin and package keepin. Choose File > Save and close PCB Editor.
The next step is to return to Capture and send the circuit to PCB Editor so that it can be
added to the empty board.
Create a netlist
The information about your design is sent from Capture to PCB Editor in the form of a netlist,
which contains a description of the circuit and its components. (The netlist comprises three
files but you don’t need to look at them.)
Figure 8. Completed dialogue box for netlisting the design and sending it to PCB Editor. Your
file names are different.
1. Highlight your design (the object whose name ends in .dsn) in the Project Manager
window of Capture.
2. Select Tools > Create Netlist. . . from the menu bar, which brings up a dialogue box as
in figure 8. Make sure that the PCB Editor tab is active.
3. Check that the PCB Footprint box contains PCB Footprint.
4. Check that the box underneath for Create PCB Editor Netlist is selected.
5. Under Options, the Netlist Files Directory should be shown as allegro. Select Create or
Update PCB Editor Board (Netrev).
6. For Input Board File, choose the empty board that you have just set up. Click on the
‘. . . ’ button to navigate.
7. The Output Board File usually shows something sensible automatically; edit it if not. It
should use the new allegro directory.
8. Under Board Launching Option, select Open Board in OrCAD PCB Editor because our
licence doesn’t cover the full version of Allegro.
9. The entries in the dialogue box should now resemble figure 8 except for the pathnames.
Click OK to dismiss this dialog box and start the netlister.
You are warned that your design will be saved by Capture, then a Progress box shows the
various processes needed: Netlisting the design followed by Updating OrCAD PCB Editor
Board. PCB Editor is then launched with your new board.
• A Warning box may tell you that Netrev succeeded with warnings. Check the Session
Log if this happens. Messages about RVMAX and CMAX can be ignored; these are
maximum voltage ratings of the components and are not important for this circuit. Pay
attention to any others and seek advice if they are unclear.
• OrCAD PCB Editor warns you that Database was last saved by a higher tier tool,
which you can ignore.
You should now see your empty board outline on the screen of PCB Editor again; the components are invisible at this stage.
OrCAD PCB Editor
OrCAD PCB Editor is the basic version of the Allegro PCB Editor from Cadence. Despite
being ‘basic’ it is vastly more powerful than is needed for the simple designs that we shall
lay out in this course. Its interface may feel unfamiliar because the application was originally
developed for unix and has been ported to Windows with minimal changes. Some distinctive
features are obvious almost immediately.
• The design window, which shows your board, has no scroll bars.
• One design is always open; you cannot open more than one, nor close the current design
without opening a new one or exiting the application.
• There is no ‘null’ tool, such as the pointer shown by most drawing applications when no
other tool is selected.
An important aspect of the interface is that tools can be used in two ways.
• First choose a command, either from the menu bar or by clicking a button, then the
element of the design on which the tool should operate.
• Select the object first, then the command from the contextual menu by right-clicking.
I shall use both methods in the tutorials, picking whichever seems most natural at the time.
However, confusion can arise when you change from one method to the other. It is therefore a
good idea when switching to disable any active tool (right-click and choose Done if it is offered)
and clear any selection (left-click outside the board or right-click and choose Selection Set >
Clear All Selections).
The screen
The main elements of the application are shown in figure 9 on the next page.
• Design window, occupying most of the screen, where you lay out the PCB. It always
shows the board viewed from the top; the bottom layer is seen through the board as if it
were transparent.
• Menu bar along the top as usual.
Figure 9. Screenshot of OrCAD PCB Editor with an empty board; the black background
has been changed to white for a clearer printout. The rectangles show the board outline (outer),
route keepin and package keepin (inner). The Find and Options control panels have been pinned
open on the right.
• Toolbars in two rows under the menu bar and a further column down the left-hand side.
Their arrangement depends on the size of the screen. Hover the pointer over a button to
reveal its function.
• Control panels with tabs on the right-hand side. Each panel pops out when you move
the pointer over its tab. Click the pin to lock a panel open.
– Find selects the type of object that is highlighted when you move the mouse around
the drawing.
– Options changes according to the current mode and command; it selects the active
class and subclass when PCB Editor is idle, then offers appropriate options when a
command is chosen.
– Visibility hides layers of etch while routing the board.
I strongly recommend that you keep the Find and Options panels pinned open as in figure
9; Visibility is less useful in boards with only one or two layers of etch.
• Command console window at the bottom left of the screen. This prints a running log
of your actions and is useful to show when Allegro is waiting for input from you. It also
displays the output from commands such as Design Rules Check.
• Worldview window at bottom right shows how the relation between the board outline
and the view in the main design window. It is useful for moving the design window
around the board as we shall soon see.
• Status bar at the bottom of the screen. It shows the coordinates of the pointer (crosshairs).
The P (Pick) button is useful for typing coordinates instead of clicking with the mouse if
your hand is unsteady.
At the far right is a coloured block called DRC, which stands for Design Rules Check.
It may be yellow because checking is not up to date. Usually it should be green to show
that automatic checking is turned on and that no errors are detected.
A lot of jargon is associated with Allegro. It often refers to your design as the database, because
that’s what it is from the point of view of the computer. The various elements of the design
are classified into classes and subclasses, which I’ll write as class/subclass in the instructions.
Here are some common examples.
• The Etch class includes the regions of copper that act as pads for the components and
the tracks that carry the signals between them. Our designs have two subclasses of etch,
Top and Bottom. They are coloured green and yellow respectively.
• The Board Geometry class includes the Outline, which we have already seen. Subclasses Silkscreen_Bottom and Silkscreen_Top are used for text to annotate the board.
• We have also seen the Package Keepin class, used to prevent components being placed
too close to the edge of the board. It has no subclasses.
The active class and subclass can be chosen in the Options control panel but PCB Editor usually
selects them automatically when you make a tool active.
Moving around the design
Two methods can be used to pan or roam around the design – move the display to the region of
• Use the arrow keys on the keyboard.
• Hold down the middle button of the mouse and drag. A confusing feature of this is that
it drags the window over the design. This means that the design moves in the opposite
direction to your drag. It is the reverse of the hand ‘grabber’ in applications such as
Acrobat, which drag the design under the window.
But I have only a two-button mouse! Many two-button mice have a scroll wheel, which
acts as the middle button when pressed.
You will also need to zoom into the design to concentrate on small details or zoom out to review
the complete layout. Again there are two methods.
Figure 10. The Placement dialogue box, showing the components for the one-transistor amplifier. Transistor Q1 is ready to be placed on the board.
• Use the commands under the View menu or the corresponding buttons and shortcuts.
Zoom Fit fills the window with your complete design, which is often helpful.
• The scroll wheel of the mouse zooms in and out, centred on the current position of the
The WorldView window can also be used to zoom and pan. If you drag a rectangle here, that
becomes the area shown in the main window.
I could write a lot more about the interface but it is more fun to place the components and
route the PCB.
Place and arrange the components
Choose Place > Manually. . . from the menu bar to start placing the components. This brings
up the Placement dialogue box shown in figure 10. The Placement List tab should be active
and the list should show Components by refdes with the components in your design listed
below. It is straightforward to place the components for this simple design. See figure 11 on
the next page for guidance.
1. Start with the transistor. Click the box next to Q1 in the Placement dialogue. Its outline
appears in the Quickview box.
2. Move the cursor out of the Placement box on to your design. The outline of the transistor
is attached to the cursor. Left-click to place it centrally on your board. The outline is
filled in and a small P for ‘placed’ appears in the Placement box next to the refdes.
Figure 11. Screenshot of the board for the simple, one-transistor amplifier after all components have been placed and arranged. Cyan lines of the ratsnest show the connections between
3. Place the connectors for input and output next. Select the boxes for both J1 and J2.
Move the mouse onto the design and a two-pin header for J1 appears on the cursor. Click
somewhere near the left-hand side to place it. Don’t worry about its orientation for now.
4. The outline of J2 now appears automatically on the cursor; place this on the right-hand
5. Next place the four resistors. Put them in the same positions relative to the transistor that
they have on your schematic drawing. This makes the circuit easier to wire. Refer to
your schematic drawing to identify each resistor.
Keep all components inside the inner purple rectangle, which shows the Package Keepin.
It turns green if you try to place any part of a component outside it.
6. Place the two capacitors in the same way. This completes the placement so dismiss the
dialogue box.
The components are joined by a set of cyan lines called the ratsnest to show their logical
connections. These lines will be turned into copper tracks when you route the board. The lines
of the ratsnest simply take the shortest path between components and therefore cross other
lines. Real tracks cannot do this. It is therefore vital to adjust the orientation and position of the
placed components to reduce the number of crossings in the ratsnest and make routing easier.
Before doing this, experiment by moving the mouse around the design window without
clicking. Elements of the design are highlighted and an explanatory note appears as the mouse
passes over; there is no need to click on an object to highlight it as in many drawing programs.
If you hover the cursor over the outline of the transistor, for example, the message Component
Instance "Q1" is shown. The mouse may highlight the outline of a component, its pins, text or
lines of the ratsnest. How can we be sure to move a complete component, not just a part of it?
Moving a pin by itself would be a seriously bad idea, for example.
Figure 12. The Find control panel set up so that only symbols can be selected.
This is where the Find control panel is useful. Open it by moving the mouse over its tab if
it is not pinned open already, click the All Off button, then select Symbols as in figure 12. Only
complete symbols for components are now highlighted under the mouse. Individual pins are
no longer selected, for instance. This makes it much easier to move and rotate components.
• The simplest way of moving a component is to left-click on it and drag, holding the
mouse down.
• Alternatively, move the mouse over a component, right-click and choose Move from the
contextual menu. Left-click in its final location.
• To rotate a selected component, right-click, choose Spin and move the mouse around to
get the desired orientation.
• Both of these actions can also be chosen from the Edit menu and the toolbar has a Move
• Do not use the Mirror command, which is different from the commands in Capture. Here
it moves the component from the top to the bottom of the PCB. This design is not that
Move and rotate the components to simplify the ratsnest. This design is easy because no crossings are required if you follow the schematic drawing, which makes routing trivial.
When you have placed and arranged all the components, update the design rules check by
choosing Tools > Update DRC from the menu bar. The DRC block near the bottom right of the
window turns green and the Command window shows No DRC errors detected if everything
is correct. If you have placed a component outside the keepin, for example, the message would
be DRC done; 1 errors detected. The error is shown by a tiny red ‘butterfly’ marker on the
design. Move the component inside the keepin and the marker disappears.
Save your design with a new name for the populated board. Unusually, Allegro asks you
if you wish to overwrite an existing file when you Save it. You may wish to save successive
Figure 13. Screenshot of the routed board for the simple, one-transistor amplifier. The tracks
are yellow, which shows that they are on the bottom of the board (and hard to see on the
printout). Your screen may not match this image exactly because it depends on which classes
are active at the time.
versions under different names in case you need to go back and repeat a step. Allegro does not
save backups automatically.
Route the board
The electrical connections depicted by the ratsnest must now be replaced by copper tracks on
the PCB. This procedure is called routing the board. The layers of copper are called etch in
Allegro because of the usual manufacturing process. Tracks should be drawn on the bottom
of the board with the components on the top (where they go by default). The wires from the
components pass through the holes in the pads and are soldered to the tracks on the bottom of
the board.
Jargon: cline is short for connecting line, a segment of a copper track. A plain line may show
the edge of the board or the outline of a component and is not a conductor. ¦
Keep the layout of tracks as straightforward as possible – imagine that you are soldering
the board yourself. Do not make life difficult by running tracks unnecessarily close to pads, for
instance. You should aim for something like the layout shown in figure 13 but there is no need
to follow this precisely.
Draw the tracks as follows. Before starting, check that no objects are selected (left-click
outside the board or right-click and choose Selection Set > Clear All Selections) and that no
tool is active (right-click and choose Done if it is offered). Pin the Find and Options control
panels open, which makes it easier to control the tools.
1. Choose Route > Connect from the menu bar.
2. The Options control panel changes to reflect the current activity and it now shows the
layers available for routing. We want all the tracks to go on the bottom of the board so
Figure 14. (a) Options and (b) Find control panels for the Add Connect command, and (c) Options for Slide.
change the Act (active) layer to Bottom, which is painted yellow. You can also change
the Alt (alternate) layer to Top, which is painted green, but we need only one layer for
this circuit. Line lock should be 45 (degrees), which determines the allowed change in
direction of a track. See figure 14(a).
The Find control panel (figure 14(b)) is automatically configured to select the relevant
objects for routing: pins, vias, shapes, cline segments and ratsnests. (Shapes are typically
areas of etch, which is why they are active.)
3. Left-click on a pin to start routing a segment – the part of a track that runs from one pin
to another. A segment of the ratsnest highlights to show that it is available for routing.
4. Move the mouse towards the pin at the other end of the highlighted ratsnest. A thick
yellow line is drawn to show the copper track and replaces the line of the ratsnest.
5. Click at intermediate points to fix corners. These automatically turn through 45°, which
is good practice. It is a bad idea to draw 90° corners because they are prone to breakage
during etching.
6. Click on the destination pin to complete the track.
7. Repeat to route all segments of the ratsnest. Right-click and choose Done when you have
Run a design rules check to detect any problems with routing. For further details, choose
Display > Status. . . from the menu bar. The section on Symbols and nets should show that
everything has been placed and routed, while DRC errors should be shown as Up To Date with
no errors. Save your board.
If you zoom in on your layout, you will see text on the tracks that you have drawn. These
are the names of the nets, which were assigned by Capture. By default the names are something
like N12649 and we shall give some of them more meaningful names in the next design so that
they can be identified readily.
Oops! – I made a mistake
There are several ways of undoing an error.
• Right-click the mouse and choose Oops. This undoes the most recent partial action, such
as drawing the last segment of a track.
• Right-click and choose Cancel, which undoes the last complete action.
• Try Edit > Undo to go further back.
• If you have made a complete mess, go to the menu File > Recent Designs and reload
your design without saving changes (there is no Revert to Saved command). This abandons all changes since you last saved the file, which I hope was not too long ago. . . .
My tracks don’t look very good: How can I improve them?
PCB Editor offers many ways of adjusting the tracks. First make sure that you are not still using
the Connect tool by right-clicking and choosing Done if this appears on the contextual menu.
Small adjustments to routed tracks can be made with the Route > Slide tool, which loads the
Options control panel as shown in figure 14(c) on the previous page. I suggest that you change
Bubble from its default of Shove preferred, because this encourages Allegro to move tracks
around in a startling manner; Hug only is more gentle. Click and release the mouse button on
a segment to select it, slide it around and click again when you are satisfied with the result.
For larger changes, you might wish to remove part of a track or the complete track and
redraw it. Proceed as follows.
• Move the mouse over a cline segment, which should highlight. If it does not, open the
Find control panel and choose All On.
• You can delete the etch at three levels using the contextual menu:
– Delete removes the segment – a single straight line of track between corners or
– Connect Line > Delete removes the complete track (cline) between the two nearest
pins or junctions.
– Net > Ripup etch unroutes the complete net.
• Use Route > Connect to redraw the track.
This nicely illustrates the way in which PCB Editor allows a hierarchy of selections: just a
segment, a complete line, or the whole net.
Aaarghh! – I’ve just spotted an error in the circuit
If you spot an error in the circuit, rather than the layout, follow the instructions in section A
on page 49. You can correct the schematic drawing in Capture and send a new netlist to PCB
Editor, which makes only the minimum number of alterations to your board. It is not necessary
to repeat the whole layout. This is one of the advantages of computer-aided design.
Add text
Next add some text to the board to make it easier to fabricate and use. In particular, all connectors (headers) must have the function of each pin identified as on the schematic. Your name
would be useful too. There is no need to add a label for each component because the refdes and
value are shown automatically. Text and the outlines of components are printed on a commercial board using ink or paint as a layer called the silkscreen. We cannot produce a silkscreen in
the university and text must therefore be placed on the copper (etch) layers.
1. Start by putting your name on the board. Choose Add > Text from the menu.
2. Use the Options control panel to select the destination for the text. You are probably
getting the hang of the interface by now: choose a command, select options, then do it.
• Put essential text such as your name on the bottom layer of copper because this is
part of every board. The Active Class should therefore be Etch and the Subclass
should be Bottom.
• Text on the bottom of the board should be mirrored so that it reads correctly from
below, so select the Mirror box.
• Text block is a confusing way of specifying the size of text. A larger number for the
block produces larger text. Something like 4 is about right for your name.
3. Click in the design where you would like the text and type. Hit Return (Enter) to get a
new line. Click to begin a new block of text elsewhere or right-click and choose Done
when you have finished.
4. Now add some text on top of the board to identify the connectors. Again choose Add >
Text but this time set the active class and subclass to Etch/Top. Turn off the mirroring
and reduce the size to 2.
Add text for Input and Ground near the input connector and Power, Output and Ground
by the output connector. Keep the text away from the pads: It is printed in copper and
could cause a short circuit.
Congratulations! – you have finished your first PCB. Don’t forget to save it.
Print the design
The simplest way of printing the design is to ‘plot’ it (the usage goes back to the days of pen
plotters). Select File > Plot Setup. . . from the menu and choose the following settings.
• Usually the Plot scaling should be unity so that the size of the printout matches that of
the PCB. This board is so simple that it is better to enlarge the drawing so enter 2 instead.
• Change the Default line weight to 10, otherwise the outlines are thin and indistinct.
• Select Auto center under Plot orientation.
• Set the Plot method to Color and close the dialogue box.
Open the Options control panel and set the active class to Etch/Bottom. This emphasizes the
most important features. Now print your layout with File > Plot. . . .
• Click on the Setup. . . button. Check that the paper size is correct and is in landscape
orientation. Confirm also that a colour printer is selected.
• Choose OK to print your layout.
The image should resemble figure 13 on page 24 except that colours on the plot are opaque.
Stick the output in your laboratory book.
This plot is not useful for manufacturing the PCB. In the next design I’ll show you how to
get printouts that can be used to make your PCB in the university.
* Milestone: Ask a member of staff to assess your finished design.
Instrumentation amplifier – single-sided board
The second design is another classic circuit, shown in figure 15 on the following page. This is
an instrumentation amplifier based on three opamps. You will study its operation in Analogue
Electronics 2. Its main characteristics are as follows.
• Both inputs v+ and v− have a high input resistance because each is connected directly to
the non-inverting input of an opamp.
• The third opamp acts as a subtracter to pick out the difference between its inputs (it can
provide gain as well but I have chosen not to do this).
• The gain for differential signals (the difference v+ − v− ) can be adjusted with the single
resistor R2 .
• The gain for common-mode signals (which have v+ = v− ) is very low.
The circuit is used to amplify a small difference in voltage between its two inputs while rejecting a large background or noise voltage that affects the two inputs equally. This is often needed
with sensors, so remember this in Team Design Project 3. It may also be helpful in the project
for this course.
In practice it is unlikely that the circuit would be built using three separate packages with
single opamps as in this design. Complete instrumentation amplifiers are available in 8-pin
packages. Even if these were unsuitable, a quad package that contains four opamps could be
used although these lack the pins for trimming the offset voltage. We shall not simulate this
circuit, just lay out the PCB. The LF411 is a widely used opamp.
NC = 8
NC = 8
Offset null
16 V
16 V
+15 V
0 V
-15 V
NC = 8
SET = 0.5
Figure 15. Instrumentation amplifier based on three opamps. The label NC = 8 on the opamps
is not normally visible and will be explained later.
Schematic capture
Create a new directory for this design, as always, and start a new project in Capture. Place the
components on the schematic but do not connect them yet. The only unfamiliar component
should be the potentiometer, which is called POT – search for it.
Power supply rails are normally hidden to simplify schematic drawings. Here the power
pins of the opamps are connected to named power symbols. Capture considers all power symbols with the same name to be connected together. Ground (earth) symbols work in the same
way. (Often the power pins themselves are hidden, as we’ll see in the final design.) Connect
the power supplies as follows.
1. Select Place > Power. . . or click the power symbol button on the toolbar and select
VCC_CIRCLE from the CAPSYM library. Use the same symbol for both +15 V and
−15 V supplies. Place one near each power pin, mirror it vertically if necessary and
connect it to the pin with a short wire.
2. Double-click the name of each power symbol in turn and change the name to VCC for
positive and VEE for negative supplies respectively. This is a standard usage (but there
are many others). Check the orientation of the opamps carefully! Some are mirrored
vertically to make the circuit clearer and this reverses the power connections as well.
3. In the same way, select Place > Ground. . . or click the ground button. Use GND from
CAPSYM for the ground (earth) symbols. These symbols must have the same name
throughout your drawing or they will not be linked.
Wire the components and add text to identify the pins of the two connectors.
Two of the opamps have unconnected pins. This is deliberate because they are for offset
adjustment and it is only necessary to do this on one opamp. PCB Editor must be told about
this, otherwise it assumes that you omitted the connections by mistake and flags an error. Show
that the pins are deliberately unconnected by choosing Place > No Connect from the menu
bar or clicking the button, then clicking on the pins. A small cross appears as in figure 15 on
the previous page. PCB Editor requires every pin to be connected or explicitly marked as not
Next enter the footprints. You must work out which to use for yourself. The real components
are available in the laboratory and you must match them to the catalogue of our local library,
which is shown at the end of this handout. It is best to install ICs in sockets for student projects,
rather than soldering them directly to the PCB, so choose one of the GU-DIPSOCK footprints
for the opamps.
Fixup. Incompatibilities between Capture and PCB Editor must again be corrected before
making the netlist. First, the pins of the electrolytic capacitors are wrongly numbered. Repeat
the instructions in section 4.1 on page 10 to fix this. ¦
Fixup. A new problem is that only 7 pins are defined on the electrical symbols for the opamps
but the package has 8 pins. You might hope that the software would assume that undefined pins
are not connected but it does not: It must be told this formally.
1. Select one of the opamps and choose Edit > Part, which brings up the Part Editor.
2. Choose Options > Part Properties. . . , which brings up the list of User Properties.
3. Click the New. . . button. Give the new property the name NC, which stands for No Connect, and the value 8, which is the number of the unconnected pin. (Use a list separated
by commas, such as 7,8, if more pins are not connected.)
4. Click OK to get rid of the dialog boxes and close the Part Editor. Choose Update All so
that this change is applied to all LF411 parts in your design.
The NC property was made visible on the schematic in figure 15 on the previous page, which
therefore shows NC = 8, but you need not do this. ¦
Run a Design Rules Check and correct any errors. Print your schematic when it has been
completed and survived the DRC.
* Milestone: Have your drawing checked before you go any further.
Create the PCB and place the components
Remember to make an allegro directory first. Set up the board as before (section 4.4 on page 14)
but make it 3.500 × 2.500 , which gives you plenty of room for the larger number of components.
Save the board and quit from PCB Editor. Back in Capture, create a netlist and send the design
to PCB Editor as before. Check the Session Log: Ignore any warnings about RVMAX but
investigate any others.
We’ll place the components using a different technique this time. Choose Place > Quickplace. . . from the menu bar. The defaults should be suitable (Place all components, Around
package keepin, Top). Click Place then OK. Your components are now arranged at the top of
the board, ready for you to move them into position.
Move the components onto the board, arrange them to resemble the schematic drawing and
adjust them to make the ratsnest simple with as few crossings as possible (it is not possible to
eliminate all of the crossings). This step is really important. It is easy to route the tracks on
a well-placed board; conversely, a poorly-placed board needs long, convoluted tracks or may
even be unroutable.
Run a Design Rules Check when the components have all been placed and save your board.
Add mounting holes
Most PCBs need to be mounted inside a piece of equipment and therefore need holes for fixings.
Mounting holes and similar features are called mechanical symbols and are placed in a slightly
different way from electronic components because they are not part of the netlist.
1. Select Place > Manually. . . to open the Placement dialogue box, bring the Advanced
Settings tab forward and choose to Display definitions from Library. This is necessary
because the symbols are not in the database imported from Capture.
2. Return to the Placement List tab and select Mechanical symbols from the drop-down list.
3. Use the same procedure as before to place a GU-MOUNTING156 symbol near each
5 00
. Do not place the holes
corner of the board. This is a hole of diameter 156 mils or 32
too close to the edge or the board may break when it is drilled.
Mounting holes are shown on my routed PCB in figure 21 on page 36.
Preparation for routing
Power tracks are usually made wider than signal tracks because they have to carry more current.
Our tracks are already so wide that it’s barely necessary but we’ll do it for future reference.
1. Choose Setup > Constraints > Physical. . . from the menu bar. This brings up the
Constraint Manager and a Tip of the Day if you are unlucky (sigh).
2. The left-hand part of the window shows the various properties that can be edited. Click
on All Layers under Net. See figure 16 on the following page for guidance.
3. The main part of the window now shows a list of the nets in your design. Most of them
have random-looking numbers, such as N00451, but a few are named. These are the
nets that carry power, to which we assigned names in Capture: VCC, VEE and GND or
something similar, depending on the symbol that you chose.
4. Change the minimum width for these three nets from 25 to 50 mil.
5. Choose File > Close to return to PCB Editor.
Save a copy of your board before routing so that you can use it for double-sided routing.
Figure 16. Constraint manager after changing the widths of the three power nets but before
correcting the vias.
Autorouting a single-sided board
The instrumentation amplifier is simple enough that it is easy to route the tracks by hand. However, manual routing is impracticable for large boards and we shall therefore use the OrCAD
PCB Router to gain experience of the procedure. You will do this twice: first as a single-sided
board, as in the one-transistor amplifier, and later as a double-sided board. It is possible to
route all tracks on the single-sided board if you have laid it out well but the double-sided board
should have a simpler layout with a smaller total length of track.
Two approaches are available for automatic routing, both shown in figure 4 on page 11.
Everything can be done from within PCB Editor or you can run PCB Router as a separate
application. The first is more convenient (when it works) but the second offers finer control.
Autorouting from within PCB Editor
Choose Route > PCB Router > Route Automatic. . . from the menu bar. This brings up the
Automatic Router dialogue box shown in figure 17 on the following page. Unfortunately it
often causes a fatal error message similar to SPECCTRA quit unexpectedly with an exit code
of 3, in which case you must use the second method – jump to the next heading.
Select Use smart router for the Strategy. For a single-sided board deselect the box next to
the TOP Routing Subclass. You might wish to experiment with the Routing Direction for the
bottom layer. Click Route and wait for the results to come back. Use the Results button to get
a report on the routing and check the Completion percentage to ensure that all nets were routed
successfully. Confirm this with Display > Status. . . and save your board.
If you can’t locate DRC errors, choose Tools > Quick Reports > Design Rules Check
Report from the menu bar. This gives a table of all errors including hyperlinks to their location.
After all tracks have been successfully routed, choose Route > Gloss > Line Parameters. . .
from the menu bar. Glossing means to tidy up the design. This includes spreading tracks apart
where possible and replacing 90° corners by 45° bends (mitering). Accept the defaults and
Figure 17. Dialog box for running the autorouter from within PCB Editor.
gloss your design. Finally, use Tools > Quick Reports > Etch Length by Layer Report to find
the lengths of the tracks and add them up. In general, a better design has shorter tracks.
Autorouting with OrCAD PCB Router
Use the manual equivalent of the flow described in the previous section if automatic routing
does not work from PCB Editor. It’s a bit clumsier but gives better control over the process and
makes it easier to experiment with different settings.
Note. At some point you may get a Licensing Error warning from PCB Router. Click Ignore
Feature for This Session if it appears. ¦
1. Choose File > Export > Router from the menu bar of PCB Editor. It asks you for a
name for the Auto-Router Design file and you can probably accept the suggestion. Click
Run. You may be warned about overwriting the file, which isn’t a problem. A message
Translation Completed should appear, after which you can close the box.
2. Start PCB Router from the Windows Start menu. You are presented with the fairly complicated dialogue box shown in figure 18 on the next page. Use the Browse. . . buttons
to open the following two files.
Figure 18. Startup dialogue box for importing a design into PCB Router.
Figure 19. Screenshot of PCB Router, ready to route the instrumentation amplifier. I have
changed the background of the window to white for a clearer printout.
Figure 20. Settings in the Layers box for single-sided routing on the bottom layer and doublesided routing on both layers.
• For the Design / Session File (the first), choose the file that you just exported from
PCB Editor.
• For the Do File (the last), choose the file with _rules appended to the name of your
board file.
Click Start Allegro PCB Router to dismiss the box. PCB Router starts and you should
now see your components joined by the ratsnest within the outline of the route keepin as
in figure 19 on the preceding page. Some components have shaded footprints, which I’ll
explain later.
3. Tell PCB Router to route only the bottom layer. Choose View > Layers. . . from the menu
bar. Turn routing off for the top layer by clicking on the drop-down menu next to TOP
as shown in figure 20 and selecting the symbol. You might like to experiment with the
setting of the BOTTOM layer. The directions are hints to the router but in practice tracks
will be drawn in both directions. Click Close when you have finished.
4. Choose Autoroute > Route. . . . Leave Smart selected and click OK. The autorouter
will work away and you will see Message: Smart_route finished, completion rate:
100.00% if all is well. The tracks should be in colour, yellow for the bottom, if they are
routed successfully. Sometimes they are drawn white, which should indicate a design
rules error, even when they appear to be correct – I don’t know why.
See the suggestions below if the autorouter is unable to route your board.
5. Two further commands improve the tracks for assembly. First choose Autoroute > Post
Route > Spread Wires. . . and accept the defaults. This spreads the tracks away from
each other and from the solder pads.
6. You’ll have noticed that the autorouted board has 90° bends in the tracks, which I told
you to avoid when you routed the board by hand. We’ll now sort this out. Run Autoroute
> Post Route > [Un]Miter Corners. . . and accept the defaults. The corners are rounded
off and tracks run diagonally where possible.
7. To see the details of the finished layout, choose Report > Route Status. This will show a
lot more than you want to know! Look near the bottom and confirm that the Unconnected
length is zero. Record the Routed length in your notebook.
8. Choose File > Quit. . . and agree to Save and Quit. This writes a session file that
describes the routed tracks.
Figure 21. My one-sided layout after autorouting.
9. Return to PCB Editor and choose File > Import > Router. . . . Locate the Session File
whose name matches your board and click Run. You should see a message Translation
Completed. Close the box.
10. The window now shows your design with tracks instead of the ratsnest. Save it under a
different name to preserve the unrouted board for later.
Help! – My board won’t route
Here are some suggestions for helping the autorouter.
1. If routing has almost worked (only one or two unrouted segments), try changing the hints
given to the router. For the one-sided board there is only the suggested direction of tracks.
It is best to unroute the board and begin afresh. Choose Edit > Delete Wires > All Wires
from the menu bar of PCB Router or reload the unrouted version of your board in PCB
2. If you are far from success, look at the layout to see where the problems lie. Often one
particular track prevents successful routing. Can you rearrange the components to solve
the problem?
Quit from PCB Router without saving, or reload the previous version of your board in
PCB Editor. Rearrange or reorientate components to make the ratsnest simpler and ease
the problem before trying the autorouter again.
If none of this works, get advice from a demonstrator.
Figure 22. Part of the Color Dialog box, showing the settings for the Stack-Up to plot the
bottom layer.
Final touches
Put your name on the bottom etch layer, run a final design rule check, save your routed board
and make a coloured plot as before. My layout is shown in figure 21 on the preceding page. It is
a poor board in many respects despite the successful routing. The power tracks are excessively
long in particular. It is not hard to see how the components could be rearranged to improve the
This section explains how to get a black-and-white plot that can be used as a photomask to
manufacture your board in the university. I’m afraid that the procedure is complicated because
Allegro is not intended for such a primitive process. A further difficulty is that we need holes
in the pads to guide the drill. The general idea is to hide unwanted elements of the design and
to colour the desired features black. Save your design first.
1. Open the Color Dialog box with Display > Color/Visibility. . . from the menu bar.
2. Click the button to turn Global Visibility Off, agree to Make all classes invisible in the
small dialogue and click Apply in the main dialogue (this is needed after every change to
see the effect). The design vanishes from the design window.
3. Click the Display folder in the list on the left. We must change the Background colour
of the window so that tracks show up after their colour has been changed to black. Click
on the white swatch in the Color swatches (samples of each colour) near the bottom of
the window, then click the swatch next to Background, which turns white. Click Apply
to update the design window, which also turns white.
4. Now we need make the desired features visible again and paint them black. Start by
selecting Board Geometry from the list on the left. This brings up a set of Subclasses to
the right. Select the checkbox next to Outline to turn it on. Change its colour to black by
clicking in the black swatch in the Color region, then the swatch next to Outline. Finally,
click Apply and the board outline becomes visible in the design window.
Figure 23. Printout at actual size for manufacturing a single-sided board (bottom layer only)
with holes in the pads to guide the drill.
5. This must be repeated for all the features that we wish to print. For the bottom of a PCB
these are Stack-Up/Conductor/Bottom/Pin, Via and Etch. Activate and make them black
as shown in figure 22 on the previous page. Click Apply and your tracks appear.
6. Finally we must make the drill holes white. They are normally hidden in a layer called
the filmmask, which must be made visible. Click All for Filmmaskbottom to activate it
and change its colour to white. Click OK to close the Color Dialog.
7. The holes do not yet appear on the screen because they are ‘under’ the etch. Go to the
Options control panel and choose the Pin/Filmmaskbottom class, which makes it active
and draws it on top of everything else. Pale holes appear on the pads as desired. This
completes the bottom of the PCB.
8. Check the Plot Setup. Set the Scaling factor to 1.00 so that the mask has the correct
dimensions for the finished PCB. Leave the Default line weight as 10 or text may be too
thin for reliable etching.
9. Finally, choose File > Plot. . . as usual and you should get a beautiful picture with the
board outline and etch as in figure 23.
After all this, quit from PCB Editor without saving (or reload your design) to avoid messing up
the colours next time you use it.
* Milestone: Ask a member of staff to assess your design.
Instrumentation amplifier – double-sided board
We will now route the board using both sides. This makes it easier to lay out more complicated
boards and the university can produce both single and double-sided PCBs. However, use a
Two free vias
covers top
of joint
Commercial: Home-made: Soldered only on
platedwire soldered
bottom: no
through hole
top and connection between
top and bottom
Soldered top and
bottom: via formed by
pin of component
to top
Figure 24. Cross-section of a double-sided printed circuit board showing free vias formed by
a plated-through hole and a wire through a non-plated hole soldered top and bottom. A via can
also be formed using a pin-through-hole component but not at a connector because it covers the
top pad.
single side for your designs wherever possible. Many problems occur with double-sided PCBs,
mostly from badly placed vias, as I’ll now explain.
Double-sided PCBs
Figure 24 shows a cross-section of a double-sided PCB. Commercially produced PCBs have
plated-through holes (PTHs), which means that the copper plating extends through the holes
and joins the pads on the two sides of the board. A free via is a hole that is used purely to
move a track from one side of the board to the other, rather than to mount a component. The
plating carries current between the layers. Unfortunately we cannot plate through holes in the
university, which means that free vias need more effort: A wire must be pushed through each
hole and soldered top and bottom to join the layers of etch. You may remember this from the
novelty lights in Electronic Engineering 1X.
The wires of through-hole components can also be used as vias. This works well for some
components, such as resistors and capacitors. However, it fails for others, such as connectors,
because it is impossible to solder the pad on top of the board – it is hidden under the base of
the connector. The pins of an integrated circuit can be used as vias if they are soldered directly
to the board but it is safer to put ICs in sockets for PCBs that are assembled by hand and these
hide the pads too. Vias must therefore be placed with great care if the PCB does not have
plated-through holes.
To illustrate these problems, figure 25 on the following page shows a poor two-sided layout.
It obeys the design rules but is hard or impossible to assemble by hand.
• The board has five free vias, far too many for a board that could be routed successfully
with only one layer. The worst via is under U3, which is unacceptable for a home-made
via because the wire in the via would obstruct the integrated circuit. (There would be no
problem on a commercial board with plated-through holes.) Another via is very close to
the trimmer (R8) and it would be difficult to solder this without damaging the trimmer.
You would have to solder the via first and keep it neat.
• Several pins of resistors act as vias – R3 has two, for instance. These are easy.
Figure 25. Screenshot of a poor double-sided layout with several badly-placed vias. One is
under an integrated circuit and another is very close to the trimmer (R8). Some tracks run to
the top pads of integrated circuits, which would not be acceptable if the ICs were in sockets.
• Some pins of the integrated circuits are connected to tracks on both the top and bottom.
This is not a problem if the IC is soldered directly to the board but won’t work if it is in
a socket.
• The connectors (J1 and J2) and the trimmer (R8) have tracks only to the bottom of their
pins. This is why the via is needed near R8. No tracks run to the top because the symbols
for these components have route keepouts on the top, which forbid the router from placing
tracks there. The footprints have diagonal shading in PCB Router to show this, visible in
figure 19 on page 34.
The general rule is to avoid vias wherever possible. Every via requires two soldered joints (top
and bottom), which dramatically reduces reliability.
Double-sided routing
Re-open the unrouted version of your board and route it using both sides.
1. Remember the Default via padstack when you used the new board wizard? We specified
GU-VIA80. Unfortunately another type of via called simply VIA appears in the design
and is used by default. It is too small to be soldered by hand and must be removed.
Fixup. Choose Setup > Constraints > Physical. . . from the menu bar. Select Physical
Constraint Set > All Layers to bring up the spreadsheet shown in figure 16 on page 32.
The column headed Vias for the DEFAULT row probably has VIA:GU-VIA80. Highlight
this cell and choose Edit > Change. . . . Remove VIA from the Via list on the right and
Figure 26. Constraint manager for changing the spacing around vias. The row of cells under
Thru Via To has been selected and the value 25 typed into the first cell. This will fill the other
cells selected after hitting the Enter key.
click OK. The cell now contains only GU-VIA80, which is what we want. Close the
Constraint Manager and return to PCB Editor. ¦
2. The new board wizard set up several spacings based on the minimum line width of
25 mils. Unfortunately it does not set up the spacing around vias, which is only 5 mils
by default. This is too small for reliable construction by hand and should be increased to
match the other spacings.
Fixup. Choose Setup > Constraints > Spacing. . . from the menu bar to open the
Constraint Manager and select All Layers > Vias as in figure 26. Drag the mouse to
select all the cells under Thru Via To in the DEFAULT row. Type 25 and hit Enter, which
copies this value into all cells selected. Close the Constraint Manager and save your
board. ¦
3. Run the autorouter from within PCB Editor or export the board to PCB Router as before.
This time you should allow routing on both layers, which is the default. Note the routed
length and the number of vias; a good design may have none at all, which is a bonus.
Remember to gloss or space and mitre the tracks.
4. Import the tracks into PCB Editor if you used PCB Router. Save the routed board under
a new name.
Move any vias in inconvenient places, such as that under U3 in figure 25 on the preceding page.
If you are lucky you may be able to Slide the via but it is often better to rip up the complete
track and re-route it by hand. Other tracks must often be moved to create space for the via.
• Select the cline or net with the offending via, right-click and choose Delete or Ripup
etch from the contextual menu.
Figure 27. Double-sided layout after improving the layout and moving the badly-placed vias.
• Select the connect tool and check in the Options control panel that the active and alternate
layers are correct.
• Draw out the segments of the track as usual.
• Double-click when you reach the point where a via is needed. A via is inserted and
routing switches to the alternate layer.
• Continue routing to complete the track.
I made several changes to my board to get the final version in figure 27.
• The via was moved from under U3 to a clear region of PCB.
• Another via was moved away from R8.
• The via near C1 was eliminated by rerouting the tracks slightly.
• Several tracks were moved from the top to the bottom, which makes the board easier to
solder by hand.
• It would have been better to edit the board further so that all tracks leave the ICs on the
bottom of the board. This would require extensive rerouting and more vias to be inserted.
I also prefer to avoid vias in the tracks for power and ground.
The GU-DIPSOCK footprints have route keepouts on the top that force all tracks to use the
bottom pads.
Finally, add your name to both layers of etch (mirrored on the bottom but not on the top) to
identify them. Plot the finished board in colour with a scaling factor of 2 for clarity.
* Milestone: Ask a member of staff to assess your finished design.
Photomasks for double-sided boards
This is for future reference only; you are not required to produce photomasks for the doublesided design in this laboratory.
Separate masks for the top and bottom layers are required for production. Follow the instructions in section 6.7 on page 37 for the bottom and repeat the process with two small
changes for the top photomask.
1. Activate and colour the top subclasses instead of the bottom subclasses.
2. Open Plot Setup and choose Mirror under Plot orientation.
The top plot must be mirrored because the printed side of the mask is turned over and placed
next to the copper when the photoresist is exposed. A good check is that text should be mirrored
on both masks for a double-sided board. (The text on the bottom is also mirrored on your
computer’s screen but the text on the top is mirrored only on the plot.)
A mixed-signal system
The final design is a mixed-signal system, which means that it includes both analogue and
digital components. It is a sound level meter. This design is based on a project used for
EDP2 in the past and on the laboratories for Microelectronic Systems 1. These are its principal
features, some of which should be familiar.
• The sound is detected by a microphone and amplified by an inverting opamp circuit with
an offset voltage to allow operation from a single power supply.
• The output of the amplifier enters an analogue-to-digital converter in the LPC1768.
• The numerical output is displayed on a dual 7-segment display. The digits are multiplexed to save pins, meaning that only one digit is alight at a time. First the units are
shown, then the tens, then the units again and so on. The two MOSFETs Q1A and Q1B
select the active digit. The multiplexing is fast enough that the eye sees both digits active
• The system is powered from a battery, not the USB connection to the mbed, so that it
works standalone. Power from the battery is fed to the VIN pin of the mbed module,
where it goes to a voltage regulator that produces a regulated 3.3 V supply, which powers
both the mbed itself and the rest of the system through the P3V3REGOUT pin.
The circuit has a few features that may be less familiar.
• The 7-segment display is made up of LEDs, each of which needs a resistor in series
to limit the current. These are in packs of 4 to save space, called single-in-line (SIL)
packages. They have 8 pins for 4 independent resistors, all in a single line spaced by
0.100 . (Numerous types of network of resistors are available.)
4 2
3 1
ComCath1 ComCath2
Place 100nF close to power pins of opamp
Cath1 4
Figure 28. Sound level meter using an LPC1768 mbed and a dual 7-segment display.
Electret microphone
Figure 29. Pin-through-hole and surface-mount (gull wing) integrated circuits. Some surfacemount packages have solder pads underneath them, usually for heatsinks.
• The MOSFETs are in a dual package, which is why they are numbered Q1A and Q1B
rather than Q1 and Q2. In other words, a single 8-pin package contains 2 MOSFETs. The
drain of the MOSFET is connected to two pins rather than one because these pins carry
most heat out of the MOSFET as well as the current. Both should be connected. Finally,
the MOSFETs are in a surface mount package rather than a traditional, pin-through-hole
package. This means that the package goes on the same side of the board as the tracks
that connect to it, rather than the opposite side. Figure 29 shows the difference.
• Two test points, TP1 and TP2, have been included. These are just pins that stick up
from the PCB. It is essential to provide a test point for ground so that you can connect
the ground clip of an oscilloscope probe. Other points are useful to test the signal at
important points of the circuit.
• Two decoupling capacitors, C3 and C4, are included to keep noise on the power supply
out of the opamp. They can be drawn near the opamp but often they are all grouped
together to avoid cluttering the circuit. The general rule is to provide a single 10 µF
electrolytic (polarised) capacitor for the overall system plus a 100 nF multi-layer ceramic
capacitor across the power pins of every component, as close as possible to the component on the PCB. It does not matter where the capacitors go on the schematic drawing
but the placement on the PCB is critical.
Schematic drawing
The schematic drawing in figure 28 is not complete. You need to make some changes and
additions to it. It is not just a copying exercise!
Figure 30. Three ways of connecting power pins to the supply rails.
Several new aspects of standard practice are illustrated on the schematic drawing. The most
important is the treatment of power pins. These can be connected to the supply rails in three
ways, shown in figure 30 on the preceding page. Power pins and symbols have the special
property that they are automatically connected to other pins and symbols with the same name.
Their shapes do not matter, just their names.
(a) Complete wires are drawn, which rapidly gets clumsy in larger circuits.
(b) Power pins are wired to power symbols, whose names match corresponding symbols on
the power rails. These are VCC and VEE here as used in figure 15 on page 29.
(c) No wires are drawn to the power pins on the components; they are connected purely by
name. Power symbols with the same names as the power pins must be connected to the
appropriate supply rail. These are V+ and V− here (typical for opamps). Sometimes
the pins and their names are not shown on the components at all, particularly for digital
components. (When did you last draw the power supply on an AND gate?)
Now draw and complete the circuit yourself following these guidelines.
• You may wish to take passive components from library/discrete rather than library/pspice/
analog. These cause fewer warnings from the netlister.
• Some components are in a local Capture library called EDP2LIB.OLB. Download this
from the moodle page, copy it to your project folder for this design and add it to the list
in Capture.
• The two MOSFETs are in a single package, FDS9926A. Capture automatically uses
successive MOSFETs in a multiple package until it runs out and needs a further package.
Thus they are numbered Q1A, Q1B, Q2A. . . automatically.
• The power pins of the opamp are not shown at all. Find the names of these pins by selecting the opamp, opening the Property Editor and making the Pins sheet active instead
of the usual Parts. This shows the numbers and names of the pins. Add power symbols
with these names to the power supplies to provide the correct connections. Do not edit
the opamp itself in any way. This is a single supply system so one connection should go
to ground and the other to the positive rail.
• Many other connections are also made by name rather than drawing lines, using a net
alias. All wires with the same name are connected together.
1. Draw a short wire on the appropriate pins.
2. Choose Place > Net Alias. . . from the menu bar or use the button on the toolbar.
3. Enter the name for the Alias and click OK.
4. Click on the wire(s) that you wish to name.
Several nets are named so that they can be identified easily in PCB Editor.
• The pushbutton is in our local library and the symbol requires four pins because the
physical pushbutton has four pins and the schematic must match this.
• The power switch is a single pole, double throw (SPDT) switch rather than a simple
on–off (single pole, single throw or SPST) switch to match the component in stores.
Follow the same steps as before, summarised in Appendix B on page 50. The components are
available so that you can insert the correct footprints. Use the real components, not guesswork.
* Milestone: Ask a member of staff to check your schematic drawing before proceeding.
The procedure is generally the same as for earlier designs. However, it is a little different if
you want to try a single-sided board because of the surface-mount package for the MOSFETs.
This has to go on the same side of the board as the tracks so you must Mirror it in PCB Editor
to place it on the bottom rather than the top.
All the footprints should be in the standard library but you may need to download EDP2PCBLIB from the moodle page if any are missing. Download the zipped archive and unzip
it into your allegro folder. Check these footprints against the symbols in Capture and the real
components carefully. In particular, make sure that the pin numbers match.
Here are some tips to help you product a good layout for the PCB.
• Aim to keep the display away from the analogue circuit.
• The circuit around the 7-segment display was designed for a simple layout with an older
microcontroller. It may not be the best with the mbed and you might wish to redesign
this, provided that you use the same range of pins on the mbed.
• Make all power and ground tracks wider as usual.
• The two capacitors in parallel are for decoupling noise and must be positioned carefully
when you lay out the PCB (their location on the schematic is irrelevant). The 100 nF
capacitor should be as close as possible to the power pins of the opamp. The 10 µF
electrolytic capacitor is less critical.
Most of the design should work as before but you may encounter a puzzling new feature of
PCB Editor: the nets for VDD and ground do not appear in the ratsnest. The reason is that
separate planes (layers of copper) in the PCB are often used for power and ground, in which
case there is no point in showing the connections – they are made directly to the planes. PCB
Editor therefore hides power nets by default. This isn’t useful for our single and double-sided
boards so make the nets visible as follows.
1. Choose Edit > Net Properties. . . to bring up the Constraint Manager, then Net and
General Properties.
2. Find column headed No Rat. The entry is probably On in the rows for VDD and GND.
Change these entries to (Clear), which should empty the cells.
3. Quit from the Constraint Manager and the nets should appear in the ratsnest. Seek expert
advice if they remain invisible.
* Milestone: Ask a member of staff to assess your finished design.
Congratulations! Read Mitzner’s book [1] if you would like to learn more about PCB Editor. A handout on more advanced techniques is available on moodle under General Information
> Laboratories, which you can enter as a guest. For example, it explains how to add a copper
pour to a PCB as a ground plane and how to create footprints (package symbols).
[1] Kraig Mitzner, Complete PCB Design using OrCAD Capture and PCB Editor, Newnes
(Elsevier), 2009, ISBN 9780750689717, about £40. Read this book if you wish to learn
more about PCB Designer. Highly recommended. Mitzner covers many features that are
not explained in these notes and explains the background theory, which I barely touch.
The only disadvantage is that Mitzner concentrates on practice for commercial boards,
reasonably enough, but we have to follow a slightly different process for boards made in
the university.
[2] Clive Maxfield, Bebop to the Boolean Boogie: An unconventional guide to electronics,
3rd edition, Newnes, 2009, ISBN 9781856175074. You might not guess from its title but
this includes a wide-ranging description of modern components and construction including
PCBs. An entertaining read.
How to correct a layout if you spot an error in the circuit
It would be highly irritating if you had to repeat the whole layout after making a change to a
circuit. The good news is that it is surprisingly easy to make corrections and that you already
know the steps.
1. Save your board in its current state and quit from PCB Editor.
2. Re-open Capture and make the corrections to your circuit. Always run a DRC before
3. Repeat the instructions in section 4.5 on page 16 for creating a netlist and sending it to
PCB Editor with these small changes.
• For Input Board File, choose the board that you just saved in PCB Editor – the most
recent version of your layout.
• Use a distinct name for the Output Board File to create a new board.
4. The new board opens in PCB Editor with the minimum number of changes to accommodate the revisions to your circuit. You will have to place any extra components and
re-route any tracks that were disturbed.
The jargon for this process is that Capture sends an Engineering Change Order (ECO) to PCB
Summary: PCB design flow
This checklist is adapted from a handout by Mr I. Young. Save your work frequently!
1. Make a new directory for each design. Create an allegro directory within it.
2. Start Capture, create a new project in the new directory and draw the circuit.
o Select an Analog or Mixed A/D project if you wish to simulate the circuit. Alternatively, the PC Board Wizard gives you the choice of simulation or not and offers
appropriate libraries.
o Use libraries in the library/pspice directory if you wish to simulate your design.
If not, use libraries in the library directory, one level higher. Take passive components from library/discrete rather than library/pspice/analog. These cause fewer
warnings from the netlister.
o A helpful, local library of symbols is available in Q:/TDP3_ORCAD/Projects.olb.
o Use wires to join components, symbols and junctions – don’t just push them together.
o Provide power connections for all integrated circuits. If power pins are hidden you
must place power symbols with matching names on the supply rails.
o Include a battery or a connector for a power supply.
o Check the circuit carefully before starting the layout: It is much easier to correct
mistakes now. If you spot an error in the circuit later, refer to appendix A.
3. Prepare the schematic for PCB Editor.
o Get the real components first so that you can match them to footprints.
o Edit components with incorrectly numbered pins, such as the electrolytic capacitor
in the analog library.
o Mark all unconnected pins with the No Connect symbol.
o Place any unused parts of multi-part packages (opamps for example). Connect their
pins appropriately: inputs should often be grounded but outputs should generally
be left unconnected.
o Add the No Connect property NC to packages with pins that are not shown on the
symbol in Capture (for example, pin 8 of single opamps in DIP8 packages).
o Add footprints from our local library, prefix GU-. The symbols are in the directory
Q/allegro/pcb_lib/symbols. In most cases you should use the dipsock footprints
rather than dip for integrated circuits to prevent tracks running to the top pads.
o Run a Design Rules Check using both electrical and physical rules. Check the
Session Log even if no warning dialogue box is shown and correct any errors. Print
the final schematic to guide the layout.
4. Create an empty board in PCB Editor using the New Board Wizard.
o Set up the search paths if necessary. Add Q:/allegro/pcb_lib/symbols to psmpath
and /padstacks to padpath.
o Use 25 mil design rules so that your board will be easy to etch and solder.
o Make the size of board generous; you can reduce it later.
o Choose gu-via80 for the default via.
5. Netlist the design in Capture. Check all warnings in the the Session Log carefully even
if PCB Editor appears to be launched successfully.
6. Place the components on the board in PCB Editor. Pin the Find and Options panels open
to control the operation of the tools.
o Take time to arrange and orient the components to simplify the ratsnest as far as
possible. This step is critical to get a well-routed board.
o Add mounting holes if required. Do not place them too close to the edge.
o Use Setup > Constraints > Physical. . . to increase the width of tracks for the
power supplies and other tracks that carry a heavy current.
o Fix the list of vias so that only gu-via80 is shown and increase the spacing around
o Update the Design Rules Check and correct any errors.
7. Route the board.
o Manual routing is best for a simple design (which includes most of ours).
o If you must use the autorouter, try a single-sided board first. Use Display > Status. . . to check that the completion rate is 100%.
o If only a few tracks are not routed automatically, complete them by hand and place
vias where they are easy to solder. Use wires on top instead of a double-sided board.
o If you must use a double-sided board, review the results of the autorouter carefully.
Move any vias and tracks to pads on the top that cannot be soldered easily.
o Gloss the design in PCB Editor or PCB Router.
8. Add text on the etch layer(s) to identify the board and connectors. Mirror text on the
9. Write photomasks as pdf files at actual size. Follow the instructions carefully and remember to select a filmmask in the Options control panel so that guide holes appear in
the pads. Mirror the top photomask for a double-sided board.
10. Take your board (.brd) and pdf files to Mr A. Phillips in the electronics workshop (room
712A). He will check the layout, print the photomasks and arrange for the PCB to be
produced. Finished boards are left in pigeonholes in the electronics stores, just outside
the workshop.
Mr Phillips is always happy to assist students with PCB design. Please ask him if you need a
footprint for a component that is not in the library or if you encounter problems that are not
solved by this handout.
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF